Autodesk Inventor LT uses Extensible Markup Language (XML) files as a means of storing style information externally from Autodesk Inventor LT documents. The schema of the Autodesk Inventor LT Style Library XML files is subject to change from release to release.

XML files are used in two different ways to store style information:

Style Libraries - a group of predefined XML files that Autodesk Inventor LT documents actively reference
Exported styles - one or more files with the extension .styxml, used to share styles between documents outside of a style Library

NoteAutodesk® does not support the editing or use of these XML files outside of the tools provided inside Autodesk Inventor LT and the Style Library Manager stand-alone tool. Any manual edits to these files may result in corruption of data and render the files unusable by Autodesk Inventor LT.

You use the Style and Standard Editor to add and change styles, but they are saved in the current document. They are not available for use in other documents unless you save the style to the style library.

NoteBe certain that you want to replace the style library version of a style before you use Save to Style Library. The changed style could affect formatting in all other documents that use the style.

General Style Management Rules

There are two general mechanisms of Autodesk Inventor LT styles management: Style Name/Value and Substyles. All management interactions between documents, styles, and Style Libraries use these two mechanisms to ensure that the end object using a style has all required information.

Style Name/Value

Autodesk Inventor LT uses the style name as the unique style identifier. No two styles of the same type can have the same name in the same container. For example, inside a single drawing, there can only be one dimension style named "Default (ANSI)".However, there can be a dimension style named "Default (ANSI)", and a text style name "Default (ANSI)" in the same drawing, because they are two different style types. When Autodesk Inventor LT compares two styles of the same name, it checks all of the properties in each style to see if they are equal. This comparison is a value comparison. If a style in a document has a name match to a style in a library, and the values of these two styles are equal (every attribute is the same value), it is considered an exact Name/Value match. The concept of a Name/Value match is used by Autodesk Inventor LT to perform automated tasks.

Substyles

Styles encapsulate and reuse sets of properties. Autodesk Inventor LT takes advantage of this encapsulation to reuse one type of property set as a subset of another. One style can reference another style that contains needed information. When a style is referenced by another style, it is regarded as a substyle.

For example, dimension styles have three substyles:

Primary Text Style: used to format the primary units in a dimension.
Tolerance Text Style (optional): used to format the tolerances units.
Leader Style: used to format Hole Notes and Leader Notes.

A style only knows the name of its substyle. It knows nothing about the values of the properties contained in the substyle. When Autodesk Inventor LT checks if a style in one container (a document or a style library) is an exact Name/Value match to a style in another container, it verifies that each style is referencing a substyle of the same name. A Name/Value match between the substyles is not necessary for the owning style to have an exact Name/Value match.

When a style is copied from one container to another, Autodesk Inventor LT ensures that any substyle required by the parent style is present in the destination container. If the substyle does not exist in the destination container, it is copied along with the parent style. If the substyle does exist, the destination’s version of the substyle is used.

Note

Documents in Style Management: Documents, and the objects inside of a document, are the consumer of styles. Documents are the main point of interaction and management. All style creation, editing, and management between a document and a style library is done in the context of an Autodesk Inventor LT document.
Style Libraries in Style Management: Style libraries are the central storage location of styles for documents set to use the library. The style library is designed to assist in the management of styles between multiple documents and multiple users. The style library provides a means of insuring all users have access to the most current style information.
Templates in Style Management: Prior to Autodesk Inventor LT 9, templates were the primary source of styles. With style libraries, the role of templates in style management changes depending on the Use Style Library setting of the document. Templates now specify which styles are to be used by default when a new document is created. When a style library is used, the style definitions are copied from the style library when a new document is created.

Managing Styles Using Style Libraries

In parts, all styles from the active library, as well as styles cached in the local document, are shown in the style drop-drop list or wherever a style is chosen. In drawings, only styles that are locally cached, or are part of the active standard, are displayed and available for selection.

Day-to-day interactions between a document and a style library are transparent. Any style used inside of a document is automatically copied (cached) to that document. It ensures that the document has required style information if a library becomes unavailable.

Considerations that influence what styles (or version of a style) are available:

The document version of a style always overrides. If a style is in both a document and a library, and the two do not have the same values, the version in the document is used. Editing styles always takes place inside of a document. The style library cannot be edited directly.
In drawings, styles are filtered by the active standard. Each standard has a list of Available Styles (found on the Available Styles tab of the Standard edit window). These styles appear at the top of the Styles drop-down list of drawing documents as well as style editors that reference a substyle.
NoteThese styles are not the only ones that can be used in the document.
Any style cached in a document is available for use. It allows styles that are not part of a library to be used in a document

Automated Management of Styles in Autodesk Inventor LT

The most common tasks of managing styles between documents and style libraries are performed automatically by Autodesk Inventor LT.

Automatic Copy into Document:

When a style from the library is used, it is copied into the document automatically with all necessary substyles.

Automatic Style Cleanup:

Styles that are automatically copied into a document are automatically removed from that document whenever they are no longer in use. It allows the document to remain uncluttered of unused metadata without need for user intervention.

Automatic cleanup only happens when Autodesk Inventor LT is sure that no style data is lost if the style is removed. Styles are only automatically removed from a document if:

The style was copied by Autodesk Inventor LT automatically into the document.
The style is not used by any other object or is a substyle of any other style in the document.
The style is an exact Name/Value match to a style in the current library

If Autodesk Inventor LT cannot find an exact Name/Value match for the style in the library, or if a style was manually cached from a library into a document using the Style and Standard Editor’s Cache in Document function, Autodesk Inventor LT leaves the style in the document until it is manually purged.

Manual Management of Styles in Documents

You perform the majority of style management tasks inside of Autodesk Inventor LT. You can:

Edit and create styles
Rename styles
Import and export styles
Manually copy styles into documents
Update styles
Remove styles manually

TipSee also the Manage Styles in Documents help page for more information.

What is affected when I modify a style?

Styles in drawings are related to the active drafting standard of the drawing. The active drafting standard specifies the styles used to format drawings. Each standard has major style types such as dimensions, which each specify the formatting for individual attributes. Styles define, for example:

Line weights and leader styles
Arrowheads and other terminators
Dimension and text styles
Symbols and options available for drawing annotations
Center mark style and size
Hatch pattern choices

Styles in parts control lighting attributes.

Because some styles rely on other styles for formatting (such as the text style used to format dimensions), a change can ripple through all other styles that reference the changed style.

Modified styles affect the current document only, unless you use Manage tab Styles and Standards panel Save and then update other documents from the style library.

How can I see the styles I want to modify?

In the Style and Standard Editor dialog box, you can specify the style list. Click the arrow on the Filter and choose:

Active Standard(Drawings only) to show only the list of available styles for the active standard of the drawing.
Local Styles to show only the styles in the document.
All Styles to show all Local Styles, and styles in the Style Library.

Procedures

Manage styles in documents

You perform the majority of style management tasks inside of Autodesk Inventor LT by using Style and Standard Editor.

Edit and create styles

The most common task involving the direct management of styles is either editing a style or creating a style. Styles are always edited or created inside an Autodesk Inventor LT document (part or drawing). Styles are edited in Style and Standard Editor, even if the style was not copied into the document. Styles are automatically copied from the library into a document for edit. Because the style library cannot be edited directly, an edited or newly created style must be saved to the library from a document.

To save a style to a library:

Right-click the style in the Style and Standard Editor, and select Save to Style Library
Select Save Styles to Style Library from the Manage tab in Autodesk Inventor LT.

NoteSaving a style to a library only saves its substyles if they do not exist in the library. If a substyle already exists, it must be saved explicitly to replace the library definition. Substyles are saved to a library with the referencing style using the Manage tab

Styles and Standards panel

Save command.

Rename styles

To rename the style in Style and Standard Editor, right-click the style name and select Rename Cached Style.

Renaming a style in Style and Standard Editor only affects the copy of a style of the document. The library copy of a style is never effected by this function.

There are two effects of renaming a cached style:

All objects using the old style, and all locally cached styles using the old style as a substyle, now use the renamed style.
Once a style is renamed, it looses any link to a style library (is considered to have no match to a style in a library), unless its name is changed to a name that matches another style in the library itself.

NoteA locally cached style cannot be renamed to the same name as a style that is already cached. For example, if two lighting styles exist in a document, one named Shop Floor and another named Shop Floor-24, then Shop Floor cannot be renamed to Shop Floor-24. However, if Shop Floor is in a document, and a lighting style named Shop Floor-30 exists in the current library, Shop Floor can be renamed to Shop Floor-30, since Shop Floor-30 did not exist in the document.

Import and export styles

Style libraries are not the only means of sharing styles. The Pre-R9 Organizer command used to copy styles between documents has been replaced with an Import/Export function. This command is accessed from Style and Standard Editor. Styles are exported to a *.styxml file, and then imported into other Autodesk Inventor LT documents.

The differences between using a style library to share styles and using import/export are:

No active link is made to an exported style file, meaning there is no update style mechanism for exported styles.
On Import, any style of the same name is automatically overwritten by the imported values of the style. When you update from a style library, replacing styles and substyles must be confirmed or done explicitly by the user.
The *.styxml file is a self contained file that includes all substyles required by exported styles. A style library keeps each type of style in a distinct, separate XML file.

Copy styles into documents

Use Style and Standard Editor to copy styles from a style library into a document: Select the styles, right-click, and select Cache in Document.

NoteManually copied styles stay in the document until they are manually purged, even if they are not used by objects in the document itself. It is a useful mechanism for sending a document to another person along with all of the styles they might need, but do not want to share your entire library.

Update styles

When a style in the style library changes, update the style to apply the style changes in all documents using the style. Updating a style is always a manual process. When the style was edited locally in the document, additional confirmations may be requested to update a style.

To update a style from the library:

On the ribbon, click Manage tab Styles and Standards panel Update.
In Style and Standard Editor, select the styles, right-click, and select Update Style.
Note: Updating a style this way does not update its substyles. Substyles must be updated separately.

Remove styles

Styles not used by an object or another style can be removed from a document manually at any time.

To remove unused styles, click Manage tab Styles and Standards panel Purge. All styles and substyles which are not used in the current document are purged in a single operation.

To remove only a particular style, select the style in Style and Standard Editor, right-click, and select Purge Style.

To remove the selected style and all its substyles, select a style in Style and Standard Editor, right-click, and select Purge Style & Substyle.

TipIf a style cannot be purged from a document, check the following to verify if a style is referenced by:

An object (sketch geometry or sketch text in Drawing Resources)
Any Standard cached in a drawing. The style may be referenced as an Available Style.
Any Object Default style cached in a drawing. Object Defaults can be set to use styles that are not Available Styles in a standard.
Other styles that commonly use the style as a substyle. The most common styles used as substyles are: Text styles (used by most drawing styles), Leader styles (used by most drawing styles), and Layers (used by Standards and Object Defaults).

Styles in templates

Templates define default styles for new documents. The default styles required by a document are listed in Document Settings on the Active Standard tab (Access: Tools tabOptions panel Document Settings).

The default styles that are defined for each document type are:

Drawings:

Standard.

Parts:

Lighting, Material.

When a new document is created, the styles for that document are pulled from the style library. However, styles in a template that are not in the library are added to the new document as well.

Material management for iPart Factories

iPart factories can specify material and appearance assets in the iPart factory table. When a part is converted into an iPart for the first time, appearance and material assets in the part document are cached in the iPart factory document. It insures that an iPart factory can publish iPart members with the intended material and appearance. If you are using the material and appearance libraries provided it is not necessary to include every material or appearance as these can be assigned to the iPart member after instantiation.

Materials and appearances included in an iPart factory remain cached until manually removed.

Styles and external data

Fonts (used by text styles) and images (optionally used by custom appearances) are not stored inside an Autodesk Inventor LT document or style library. This type of external data is not managed by Autodesk Inventor LT and must be managed manually.

Create, edit, or purge styles

You can use the Style and Standard Editor to create, edit, or purge styles. New or edited styles are saved in the standard style of the current document, unless you specifically select Manage tab Styles and Standards panel Save.

NoteBe careful when saving a style to the style library. The style replaces the library version and can affect all other documents that use the style.

Create a style

You create a style by copying an existing style and modifying it to suit your requirements.

On the ribbon, click Manage tab Styles and Standards panel Styles Editorto open the dialog box.
In the style list browser, click to expand a style type, and then select a style you want to use as the basis of the new style.
Right-click the style, and then select New Style or click New.
- Enter a name for the new style or accept the default "Copy of ..." name.
- For drawing styles, select the Add to Standard check box to add the new style to the available styles list in the active standard style.
Click OK. The new style is listed in the style type browser.

TipYou can click Reset to return to the default values in the new style, but do it before you click Save.

Edit a current style

You can edit a style in your current document, but it does not affect other documents.

On the ribbon, click Manage tab Styles and Standards panel Styles Editorto open the dialog box.
In the style list browser, locate the style type you want to modify, and then double-click to show it in the window.
Modify settings as required, and then click Save. The previous version is replaced by the modifications.

TipYou can click Reset to discard the changes you have made to the style, but do it before you click Save.

Purge styles from the current document

If you know there are styles in your document that you do not intend to use, you can purge the unwanted styles.

You can purge styles two ways:

Purge Styles deletes the top-level styles from the document, such as dimension style, but retains other styles that the style referenced. For example, the dimension style uses the text style as a substyle. Purge Styles only deletes the dimension style, not the text style.
Purge Styles and Substyles deletes both the top-level style from the document, but also the referenced substyle. In the dimension example, both the dimension style and the text style are purged.

NoteYou cannot purge a style that is in use in the document. For example, the dimension style uses the text style as a substyle so the text style cannot be deleted.

On the ribbon, click Manage tab Styles and Standards panel Purge.
In the Purge Styles dialog box, unused styles are listed.
Click column headers to sort contents as needed. In the Purge column, unused styles are automatically labeled Yes but you can click individual styles to switch to No.
Click Yes to All or No to All to reset individual settings and mark all styles at once.
Select the Purge Sub-Styles check box to remove unused substyles with a parent style. Clear the check box to retain substyles when a parent style is purged.
Select the Purge Styles from all Child Documents check box to purge unused styles from the current document and all referenced documents. Not available for part documents.
Click OK to purge styles or Cancel to close the dialog box without purging.

You can use Undo to recover styles purged from the current document.

Replace styles in drawings

Through file migration or copy and paste, you may have a file that has an unwanted style, such as a dimension style. Use Replace Style to replace the old styles with a new style to make all styles uniform.

Replace Style substitutes all references of a style with another style of the same type, including object references to styles and style references to substyles. and style and substyle references. Only local styles are replaced.

Open the drawing file that contains styles you want to change.
On the ribbon, click Manage tab Styles and Standards panel Styles Editor. In the Style and Standard Editor dialog box, navigate to the style you want to replace, and then right-click and select Replace Style.
In the Replace Style dialog box, the style to replace is identified. In the With box, click the arrow and select the replacement style from the list, and then click OK.
If desired, select the Purge Replaced Style check box to purge the old style automatically.
Click Done to quit.

If appropriate, you can select multiple styles to replace with a new style.

In the Style and Standard Editor browser, double-click a style folder to list all styles in the edit window.
In the styles box, click and select Local Styles.
Hold down the CTRL key and select multiple local styles.
Right-click and select Replace Style.
In the Replace Style dialog box, select the replacement style from the list and click OK. In the Styles Editor, click Done to quit.

Import or export styles

You can use import and export to copy styles between documents. The style is exported in a special *.styxml file, which is then imported into another Autodesk Inventor LT document.

Sharing styles by importing and exporting is different from using a style library to share styles. Some guidelines to keep in mind when importing and exporting styles:

No active link can be made to an exported style file, so Update Style cannot be used to update an exported style.
When importing a style, an existing style with the same name is automatically replaced by the imported style. When updating from a style library, styles are not replaced automatically. Confirm when a style with the same name is encountered.
An exported style (an *.xtysml file) is self-contained; it includes all substyles used by an exported style. For example, an exported dimension style also includes the text and leader substyles.
A style library maintains each style type in a separate .xml file.

To export styles

On the ribbon, click Manage tab Styles and Standards panel Styles Editor.
In the Style and Standard Editor, locate the style you want to export and then right-click and select Export.
In the Export Style Definition dialog box, browse to a location and enter a name for the exported style. A file is created with the .styxml extension.

If the exported style has substyles, such as a dimension style using the text style as a substyle, it is also exported in the same file.

To import styles

On the ribbon, click Manage tab Styles and Standards panel Styles Editor.
In the Style and Standard Editor, click Import.
In the Import Style Definition dialog box, browse to a location and select the desired file with the .styxml extension.

References

Purge Styles

Purges unused styles and substyles from the current document. Dependent substyles are not listed.

Some style types require substyles to be fully defined. For example, a dimension style needs a text substyle to define the font used to display the dimension. The text style in this case is used indirectly as a substyle of the dimension style, but the same text style may be used directly in another case, such as when a text style is applied to a block of text.

Access:

Ribbon: Manage tab

Styles and Standards panel

Purge

Click a column heading to sort contents. All columns resort to correspond with the new order.
Document Name	Shows file name in which the style is used.
Style Name	Lists styles in the current document.
Type	Identifies the style type.
Changes	Indicates if a style was changed in the document or library.
Purge?	Indicates individual unused styles to delete. If Yes, the style in the document is deleted. If No, the style is retained in the current document.

Click Yes to All to delete all unused styles in the document or No to All to retain the unused styles in the current document.

Select the Purge Substyles check box to delete unused substyles when a referencing style is deleted. Clear the check box to retain the substyles when a parent style is deleted.

Select the Purge Styles from all Child Documents check box to purge styles in referenced files. Child document file names are not listed in the document name column. Clear the check box to purge styles in the parent document only.

Replace styles

Substitutes all references to a selected style with another style of the same type, except for Standard style. Only local styles are replaced.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Styles Editor dialog box, right-click a style in the browser and select Replace Style.

Replace

Shows one or more selected styles. Multiple styles are separated by commas.

Cannot add or delete styles in this box. To add styles, click Cancel and reselect styles to replace in the edit window.

With

Lists the styles of the same type as the style to replace. Click to select the replacement style.

Purge replaced style

Purges the selected style after all references are replaced with references to the new style.

Update styles

Updates styles in the current document, and optionally, in referenced files (child documents), to match the styles in the style library.

Access:

Ribbon: Manage tab

Styles and Standards panel

Update

Click a column heading to sort contents. All columns resort to correspond with the new order.
Document Name	Shows file name in which the style is used.
Style Name	Lists styles in the current document.
Type	Identifies the style type.
Changed	Indicates if a style was changed in the document or library. If the style does not match the library, it is marked Not in Library.
Update?	Switches individual styles to update. If Yes, the style in the document is updated to match the version in the style library. If No, the current document style definition remains in effect.

Click the Update Styles in all Child Documents check box to update styles in referenced files. Child document file names are listed in the document name column. Clear the check box to update styles in the parent document only. Not available in part documents.

Click Yes to All to update all document styles to the library version or No to All to preserve the changed styles in the current document.

Style and Standard Editor

Creates and edits styles. Styles defined in the Style Library and in the active document are listed in the browser pane; available styles depend on the current document type. The selected style contents are shown in the editor pane.

The Style and Standard Editor sets the active standard in a drawing document and, for part documents, sets lighting styles.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles , Styles in the Active Standard (drawings only), or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

For the current document, you can click:

NoteOn the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

Click a style node in the browser to show information about the selected style in the editor window.
Name	Identifies the selected style.
Location	Indicates if the style is located in the Style Library, the current document, or both.
In Use	Indicates if the style is being used by the document.
Changes	Indicates if changes were made to the style. If changes are made only in the current document, the entry is labeled Local. If changes were made to the Style Library, the entry is Library. If both the local and library styles were changed and the values do not match, the entry is Both.

Click to show definitions of styles used in Drawing documents:

Standard	Balloon	Center mark
Datum target	Dimensions	Feature control frame
Hatch	ID	Layers
Leaders	Object defaults	Parts list
Surface texture	Weld bead	Weld symbol

Click to show definitions of styles used in Part documents:

Lighting

Style Libraries

A style library is a common source of styles in Autodesk Inventor LT documents.

Each style library is a collection of .xml files, one for each style type. Only one style library can exist in a folder. Style libraries are stored on any local or network location. A CAD administrator manages shared style libraries.

When to use style libraries?

Use a style library when you:

Work in a workgroup that needs a common source of styles.
Use document formatting changes from a CAD Administrator.
Want to deploy style changes to documents.
Share formatting standards without providing internally controlled templates or documents.

A good time to start using style libraries is when you start a new design project. You can use the default style library associated with the drafting standard, and customize styles according to the company standards.

Procedures

Save styles to a style library

You can create or edit a style in a document, and then save the changed version to the style library. If a style has the same name as a style that exists in the style library, it replaces the library version. Otherwise, the style is added to the library as a new style.

Create or open a document with the styles you want to copy to the style library.
On the ribbon, click Manage tab Styles and Standards panelSave.
A dialog box with a table listing all document styles that do not match the style library displays.
In the Save to Library column, specify the saving status for particular styles. Set Yes to replace the library style with the style from the current document. Set No to keep the library style unchanged.
TipTo mark all styles at once, click Yes to All or No to All.
Click OK to save selected styles to the style library, or Cancel to close the dialog box without saving styles.

NoteWhen you save a style to style library, substyles are automatically included in the process. You are prompted to save referenced substyles that are different from the library.

References

Save styles to style library

Replaces styles in the style library with selected styles from the document.

TipIn other documents, manually update the styles to apply the new versions from the style library.

Access:

Ribbon: Manage tab

Styles and Standards panel

Save

Click a column heading to sort contents. All columns resort to correspond with the new order.
Document Name	Displays the source document.
Style Name	Lists names of styles that differ from styles in the style library.
Type	Identifies the style type.
Location	Indicates whether the style is located both in the style library and in the document, or in the document only.
Changes	Indicates whether the style was changed in the document or library. If the style does not match the library, displays No.
Save to Library?	Switches individual styles to save to the style library. Click the status to change it. Set Yes to replace the library style with the style from the current document. Set No to keep the library style unchanged. NoteStyles that are not in the library are automatically switched to Yes, but can be changed to No.

Click Yes to All to save all styles in the document to the style library or No to All to retain the styles in the current document, but not update the library.

NoteWhen you save a style to a style library, substyles are automatically saved. You are prompted to saved referenced substyles that are different from the library. For example, a dimension style uses a text style as a substyle. If you change the dimension style and text style, saving the dimension style to the style library prompts you to also save the text style to the library.

Transition legacy documents to a style library

Styles are used to format objects in Autodesk Inventor LT documents. In Autodesk Inventor LT 8 and older versions, styles resided in a template or document. Styles can now reside in a style library that contains all style definitions.

Using style libraries, multiple designers access the same styles so formatting is more uniform among documents and styles are easier to update.

How do I get started using a style library?

In the Tools tab Options panel Application Options File tab, you set the Use Styles Library option to indicate how a style library is used by the document.

Set to Read Write to use the style library. This option means that the style library is writable. Designers can create and change styles, and then save them to the style library.
Set to Read Only to make styles available to designers, but prohibit them from replacing the style definitions in the library. Designers can create styles and save them in individual documents, but the library is locked.
NoteThis is the best option to use when getting started with style libraries.

If you are uncertain about losing styles you have already created in existing documents, choose the Read Only option. You have access to library styles, and can analyze which of the previously created styles you want to add to the library. You can then reset the option to Read Write (so the style library is writable), and use the management tool to copy styles into the library.

NoteFiles must migrate from a previous version of Autodesk Inventor LT before their styles can be added to a style library.

What happens to styles in my templates?

A template is a regular Autodesk Inventor LT document that contains styles and other settings you want to use as defaults.

When you set the Use Styles Library option to Read Write or Read Only, and then create a document from a template, Autodesk Inventor LT compares style names to styles in the template. Styles with the same name are retrieved from the style library. A style in the template is refreshed to match the style library version.

If a template contains a style that is not in the library, the style is added to the new document, but not the library. It may be useful if you have a set of custom styles that are not for general use by others using the style library.

Purge styles from templates that you do not intend to use.

What happens to styles in legacy files?

Legacy files usually have documents that each have a set of styles.

Some styles are inherited from the templates used to create documents.
Some styles are created in-process whenever the existing style did not suit the current need.

Consequently, many documents contain custom styles that are not shared among all other documents.

All documents created from a template contain a complete set of the template styles, even if the document does not need all of them. When using styles, purge unused styles from a document to make your file size smaller.

Use Manage tabStyles and Standards panel Purge to remove unused styles from individual documents so you do not overload files with duplicated styles.

As long as a purged style was saved in a style library, it can be retrieved if needed. Styles that resided only in a document and not migrated to a style library are permanently lost.

What tools are available to transition to using styles?

You use Autodesk Inventor LT tools to transition styles:

Use the Style Library Manager to:
- Rename a Style in a library.
- Delete Styles from a library.
- Copy Styles between libraries.
- Create new Style Libraries.
Use the Style and Standard Editor to create and edit styles. The Style and Standard Editor is document-based, that means creation and editing of styles is performed in the context of the document where the style editor is opened.
To perform general style management tasks, use document-based batch commands:
- Update Styles (Manage tab Styles and Standards panel Update) updates styles in the document to match the version in the Style Library.
- Purge Styles (Manage tab Styles and Standards panel Purge) manually removes any unused styles and their associated substyles from a document.
- Save to Style Library (Manage tab Styles and Standards panel Save) saves styles inside of a document to a Style Library.

Using Create New Style Library, copy an existing library to customize, or create an empty style library and copy styles into it. This command is available from the Style Library Manager.

Style Library Manager

The Style Library Manager is used primarily by a CAD administrator to:

Copy styles from one style library to another style library.
Rename styles in a style library.
Delete styles from a style library.

Any changes made to a style library are not available in other documents until the current Autodesk Inventor LT session closes and a new session is reopened.

The Style Management Wizard is a tool for administrators to assist in batch-style management for Autodesk Inventor LT files. Batch processes harvest or purge styles for multiple files in one operation. All files must migrate to the most recent version of Autodesk Inventor LT or they are skipped during batch processing, including assemblies that were migrated but contain components that were not migrated.

Styles Overview

Some styles reference other styles as substyles (for example, the dimension style references the text style as a substyle). When copying a style library, the Style Library Manager opens the Manage Styles dialog box if mismatched substyles are detected in the source and destination libraries. For each substyle, confirm to replace the current version with the source version.

Styles are predefined properties that can be applied to an object. They are used in one of two ways:

To encapsulate a set of formatting properties for annotations, such as dimension or text styles.
To encapsulate a set of cosmetic and physical properties, such as appearance and material.

Styles have traditionally resided in document templates, but the preferred method is to store them in style libraries. Multiple designers can use a style library. They all have access to the same styles.

Some styles use other styles to complete their definition. The referenced style is known as a substyle in this context. When a style is copied, it also copies its required substyles.

Style definitions are stored in style libraries. To learn more about the role of style libraries, see Understanding style libraries.

Many legacy files have custom styles defined in one or more documents. To learn more about how to transition from template and document-created styles, see Learn about transitioning legacy files to a style library.

Style management tips

Consider these practices to preserve styles that you create or edit:

Save styles to the library.
New or edited styles are saved only in the current document. Click Manage tabStyles and Standards panel Save to save a style to the library. After the style is saved in the style library, it is available to other documents. If the library setting is Read Only in the Application Options dialog box, this option is unavailable.
Move several styles from a document to a library.
Click Manage tabStyles and Standards panel Save to move several styles from a document into the styles library. The current file must have its style library setting as Yes to use this option. If the library setting is Read Only or No, this option is unavailable.
Import and export styles
Use the Export context menu option to export a style and its substyles to an external file. Use the Import menu option later to import into other documents.

Procedures

Manage style libraries

Style Library Manager is a stand-alone tool used for the administration of style libraries. This tool works directly with the style library XML files on disk, and is not used in the management of styles inside Autodesk Inventor LT documents. It is accessed from the Microsoft® Windows® Start menu, and is found in the Tools submenu for Autodesk Inventor LT.

Use Style Library Manager to:

Create new style libraries
Manage styles in style libraries
Manage styles between multiple style libraries

Create style libraries

Autodesk Inventor LT installs with a default style library designed to leverage of all new capabilities of styles.

You can create your own style libraries in two different ways: Copy an existing style library or create an empty style library. The target directory for the new library cannot include other style library.

After you create a style library, use Style Library Manager or Style and Standard Editor to add or remove particular styles.

Rename and delete styles inside of a library

Use Style Library Manager to rename styles inside of a library. Renaming a style in the library does not rename the same style in any other library or document. Once a style is renamed, all document copies of the style loose their name match and are considered locally cached style.

The only way to delete a style from a library is through the Style Library Manager.

NoteRename and Delete commands are accessed from the right-click menu when selecting one or more styles.

TipThere is no Undo in the Style Library Manager. Renaming, copying, or deleting of styles cannot be undone. We recommend you create a backup copy of your library before you make changes.

Copy styles between libraries

Styles are copied between libraries using the Style Library Manager. To copy a style from one library to another, load the source library into Style Library Manager and click the Copy Selected Styles command between the Style Library 1 and Style Library 2 panes. See the Style Library Manager Help for more details.

Manage Style Library Contents

A style library is a group of named XML files in a directory. There is one XML file per style type (for example: lighting.xml, text.xml). Since the names of the XML files must be the same for each style library, only one library can exist in a directory.

To be considered a valid style library, all predefined XML files must be present in the directory.

The best way to share a subset of styles from a library (for example, a single standard from a specific library) is to use the Import/Export styles function in the Style and Standard Editor, or create an empty style library and copy the desired styles using the Style Library Manager.

NoteAn exported style file (*.styxml) cannot be used as part of a style library.

Incomplete Style Libraries

Though a style library is made up of several separate XML files, Autodesk Inventor LT and the Style Library Manager treat the library as a single entity. If some of the predefined XML files required for a style library are missing from a directory, Autodesk Inventor LT displays an error message indicating files are missing and cannot be loaded.

Restoring the Autodesk Inventor LT Default Style Library

A utility for restoring the default Design Data directory files is located on the Autodesk Inventor LT Install CD in the Support directory. This utility replaces the original default style library that ships with Autodesk Inventor LT, as well as the Thread.xls and Clearance.xls spreadsheets.

Prevent Style Library Changes

In a multi-user environment, CAD administrators may want to prevent users from changing a style library.

Use a Microsoft Windows file property setting. In Microsoft Windows Explorer, select all the XML files that make up the library or the library directory folder itself, right-click, select Properties, and set to Read Only.

If a single XML file is read-only, the entire library is treated as read-only.

Pack and Go

The Autodesk Inventor LT Pack and Go utility optionally includes a style library. It is included in the Design Data subdirectory.

Create a style library

You can create a style library using one of several methods. In general, new style libraries are created by CAD administrators so that uniform styles are assured throughout all design documents.

Click Start menu Programs Autodesk Autodesk Inventor LT Tools Style Library Manager.
Click the Create New Style Library command above the Style Library 2 pane.
In the Creation Method box, click the arrow to select Copy Existing Style Library or Create Empty Style Library.
In the New Style Library Location box, accept the default location or browse to the folder where you want to store the new library. If the library is accessed by a document, place it in a folder recognized by design file locations.
If copying a style library, in the Source Style Library to Copy box, accept the default library or browse to the library you want to copy. This option is unavailable if you create an empty library.
Click OK to create the library and close the dialog box.

Exit the Style Library Manager. Use the Style and Standard Editor to customize the styles in the new style library.

Copy, rename, or delete library styles

The Style Library Manager is primarily used by CAD administrators to copy, rename, and delete library styles. The CAD administrator controls the style library contents and assures that designers using styles have the same style definitions, assuring uniform document formatting.

The Style Library Manager uses the Create New Style Library command to create new style libraries.

In general, style libraries are read-only, except to make necessary changes. The Styles Library Manager uses the read-only file property, and disregards the library status specified by the Use Style Library=Read Only option in Application Options.

Any changes made to a style library are not available in other documents until the current Autodesk Inventor LT session closes and a new session is opened.

You can create new styles or rename styles in a document, but they affect only that document. Take a separate step to save a new or changed style to a style library to replace the library version. Access to the style library may be controlled by the CAD administrator.

Copy styles from one style library to another style library

You can develop style libraries that are specific to a given design document. This procedure copies styles you have already defined in one style library to another style library.

Click Start menu Programs Autodesk Autodesk Inventor LT Tools Style Library Manager.
In Styles Library 1, click the down arrow to select or click Browse to locate the style library whose styles you want to copy.
In the Choose Style Type column, click a style type to list all defined styles in Style Library 1.
In Style Library 2, click the down arrow to select or click Browse to locate a style library.
If appropriate, click Create New Style Library:
- In Creation Method, select Copy Existing Style Library or Create Empty Style Library.
- Browse to the folder where the library is located.
- If copying a style library, click the arrow or browse to select the Source Library for Copy. The existing styles are listed in the Style Library 2 window.
Click one or more styles, and then click to add them to Style Library 2.
Continue to click style types to add to Style Library 1, and then select and add them to Style Library 2.

Styles in one library might not match the styles in another library. Compare the styles in both libraries.

	Click Show All Styles to list all styles in both style libraries.
	Click Show Mismatched Styles to show styles whose definitions are different in the two libraries. Mismatched styles are shown in red.
	Click Show Unique Styles to show styles that exist in one library but not the other. Unique styles are shown in blue.

Click the right and left arrows to add or remove styles as desired.
If mismatched substyles are detected, the Manage Styles dialog box opens. Indicate to overwrite the version of the substyle in the destination library or retain the current version.
Click Close to save the libraries.

NoteOnly the selected style is copied from one Style Library to another. Substyles are only copied if they do not exist in the destination library. If a style exists with the same name, the destination version is used.

Rename styles in a style library

A style name can change in the style library, but all documents that reference the old name lose their association to that style.

Click Start menu Programs Autodesk Autodesk Inventor LT Tools Style Library Manager.
Click the arrow or browse to the library whose style you want to rename.
In the Style Library 1 or 2 window, right-click a style name and select Rename.
A warning asks you to confirm that documents links to the style will be broken. Click Yes to continue or No to cancel renaming. If Yes, enter the new style name.
Continue renaming as needed, and then click Close to save the changes.

Delete styles from a style library

A style can be deleted from a style library, but all documents that reference the old name lose their association to that style.

Click Start menu Programs Autodesk Autodesk Inventor LT Tools Style Library Manager.
In the Style Library 1 or 2 window, click the arrow or browse to the library whose styles you want to delete.
Select a style type in the Choose Style Type list. Then right-click a style name in the Style Library 1 or 2 window and select Delete.
A warning asks you to confirm that the style will be permanently deleted from the style library. Click Yes to delete the style or No to cancel delete.
NoteYou cannot use Undo to reverse a deletion.
Continue deleting as needed. When finished, click Exit to close the Style Library Manager dialog box.

TipUse Manage tab

Styles and Standards panel

Purge to remove unused styles from the current document, and optionally, all referenced documents.

References

Style Library Manager

The Style Library Manager is used primarily by a CAD administrator to:

Copy styles from one style library to another style library.
Rename styles in a style library.
Delete styles from a style library.

Any changes made to a style library are not available in other documents until the current Autodesk Inventor LT session closes and a new session is reopened.

NoteIf the source library substyles are not copied, substyles from the destination style library are used instead. The overall definition of the dimension style changes, because the set of substyles it uses has different characteristics compared to the source.

The Style Library Manager also accesses the Create New Style Library dialog box to create new style libraries.

Access:

Click Start menu Programs Autodesk Autodesk Inventor LT Tools Style Library Manager. In the Style Library Manager dialog box, click a style type to populate the Style Library pane with defined styles.

Choose Style Type

Lists all style types. Click a style type to show all definitions in the Style Library column.

Style Library 1

Shows styles of the selected type in the specified library.
Arrow	Lists available style libraries. Click to select.
Browse	Click to browse to the appropriate style library.

Style Library 2

Shows styles of the selected type in the specified library.
Arrow	Lists available style libraries. Click to select.
Create New Style Library	Creates a style library by copying an existing library or creating an empty library, specifies its location, and names the source library to copy, if applicable.
Browse	Click to browse to the appropriate style library.

Comparing Styles Between Definitions

If a style exists in both Style Libraries and is an exact name value match (that is, Equal), then the text in the style lists has a normal font display.

If a style exists in both Style Libraries, is an exact name match, and is not a value match (that is, Not Equal), then the text for this style name displays as bold, underlined, and red.

If a style only exists in one Style Library (that is, is Unique), then the text for this style name displays as bold, underline, and blue.

Filter commands

Shows differences between the lists in the style libraries:

	Click Show All Styles to list all styles in both style libraries.
	Click Show Mismatched Styles to show styles whose definitions are different in the two libraries.
	Click Show Unique Styles to show styles that exist in one library but not the other.

Copy style commands

	Copies selected styles from Style Library 1 to Style Library 2.
	Copies selected styles from Style Library 2 to Style Library 1.

Substyles are only copied from one style library to another if they do not exist in the target library. To avoid replacing an existing style accidentally, you are prompted to replace the target style with the source style. It occurs if a substyle exists in the target style library, and it is different from the substyle in the source library.

Manage styles dialog box

When copying a style library, if a source style and one or more of its substyles differ from the destination library, you are asked to select which substyles to copy to the destination library.

For example, a dimension style uses the text style as a substyle. If the text substyle referenced by the dimension style is different from the text style in the destination style library, confirm to replace the destination text style with the text substyle from the source style library.

If you choose to use a combination of Yes and No in the Overwrite column, the style in the destination style library is not identical characteristics compared to the source.

Access:

In the Style Library Manager dialog box, click the Show Unique Styles command or Show Mismatched Styles command to list styles in red text. Listed styles do not match in the source and destination style libraries. Right-click a red style name and then click the arrow button to copy it. The Manage Styles dialog box opens.

Style Name	Lists the destination style name and its standard.
Path	Shows the path of the destination style.
Type	Lists the style type.
Overwrite?	The default setting is No. For each listed style, click in the column to switch to Yes.

To set all styles at once, click Yes to All (to overwrite styles in the destination library) or No to All (to copy only the parent style, but not the substyles).

Create New Style Library

Creates a style library by specifying the creation method, the library location, and the source library.

Access:

Click Start menu Programs Autodesk Autodesk Inventor LT Tools Style Library Manager. In the Style Library Manager, click Create New Style Library.

In the Create New Style Library dialog box:

Creation Method selects how you want to create the library. Click the arrow to choose Copy Existing Style Library, and then modify as appropriate or Create Empty Style Library, and then select styles from one or more libraries.

New Style Library Location browses to the folder where you want to store the new library.

Source Style Library to Copy browses to the library you want to copy when the creation method is Copy. Unavailable when the creation method creates an empty style library.

Style Management Wizard

Styles in drawings

When you create a drawing, it is automatically assigned an active drafting standard. The active standard controls styles used to format dimensions, text, line weights, terminators, and other drawing annotations and properties. Add or edit styles in the current document. If you want other designers to use the custom styles, save them to the style library or apply them in a drawing template.

All objects in drawings are by default formatted using a By Standard setting for the object layer and object style. The By Standard setting is configured in the Object Defaults style.

The Object Defaults style maps individual types of drawing objects to specific styles and layers. Unlike other styles used by the Standard style, there is only one Object Defaults style per standard.

Setting a style for a selected object

The Styles list on the Annotate tab of the ribbon displays the current style of a selected object in the drawing. By default, objects use the By Standard object style specified in Object Defaults. To change the style for a selected object, select another style from the Styles list. The formatting of the selected object changes according to the new style.

NoteIf any of the style attributes are overridden for the object, the overrides are lost when a new style is applied.

Setting a style for multiple selected objects of the same object type

When you select more than one object of the same type, and they are all defined by the same style, the Styles list shows the style name. Selecting a new style affects all selected objects.

If you have selected more than one object of the same type, but they are defined by different styles, the Styles list is blank. You can select a style from the list to reformat all selected objects with one style.

What does By Standard mean?

A drawing object such as a dimension needs a layer and an object style to specify many of its formatting properties. When creating the drawing object, the default value for the layer and object style is By Standard, and the object has the name of the active standard style. Autodesk Inventor LT evaluates objects using the By Standard layer or object style and finds the layer or object style associated with the standard.

What happens when the object default style is modified?

When you modify the object default style, all objects that reference that style update to the new settings, just like any other style.

For example, suppose you are working in a drawing where the active standard is MyStandard. MyStandard uses an object default style called MyObjectDefaults. You edit MyObjectDefaults and change the default layer for the Diameter Dimension object to MyDimensionLayer. The result is that all diameter dimensions created using MyStandard, with the layer set to By Standard, updated to use MyDimensionLayer.

What happens if the standard is modified by selecting a different object default style?

Building on the concept of modifying an object default styles, you can edit a standard style and select a different object defaults style. Doing so, you can update an entire drawing. All objects referencing the standard update to reflect the settings in the new object defaults style.

This approach is useful when reformatting a drawing from Company A's standard layer scheme to Company B's standard layer scheme.

Procedures

Set the default style and layer for individual drawing objects

The default style and layer for a type of drawing objects is specified in the Object Defaults style.

Select Manage tab Styles and Standards panel Styles Editor.
In the Style and Standard Editor dialog box, expand the Object Defaults node in the browser, and select the Object Defaults style.
In the Object Defaults window, set styles and layers for individual object types. Click a current Object Style or Layer, and select a new style or layer from the list.
Click Save to save the edits.
Click Done to close the Style and Standard Editor.

Set the balloon style

Use the Style and Standard Editor dialog box to edit a balloon style.

Select Manage tab Styles and Standards panel Styles Editor to open the Style and Standard Editor dialog box.
Expand the Balloon node in the browser, and select a balloon style to edit.
NoteTo create a balloon style, select an existing balloon style to use it as a template. Then click New, and set the properties in the New Local Style dialog box.
In the Balloon Style window, in the Substyles box, set the referenced leader and text styles to use in balloons.
In Balloon Formatting window, set the balloon shape, properties to display, and symbol size.
Set default offset spacing, if desired.
Add a comment, if appropriate.
Click Save to save the edits.
Click Done to close the Style and Standard Editor.

TipTo set a balloon style as the default for balloons, assign the style to the Balloon Object Type in Object Defaults.

Set the default datum target style

Use the Style and Standard Editor to set the attributes for the datum target style you plan to use in drawings.

Select Manage tab Styles and Standards panel Styles Editor to open the Style and Standard Editor.
In the browser, select the drafting standard whose styles you want to edit.
Click Datum Target to expand, and then double-click a listed style.
In the Datum Target Style window, set attributes on the Display and Units tabs.
Click Save to save changes to the style, and then click Done.

Changes to the style are saved in the current document only. Use Manage tab Styles and Standards panel Save to replace the version of the style in the style library. Use caution because this procedure can affect other documents that use the style.

Set up or edit hole note format

The format for hole notes is controlled by the hole note's associated dimension style. Before you begin a drawing, define a dimension style with a hole note definition for each hole type.

Set up hole note format in the dimension style

Select Manage tab Styles and Standards panel Styles Editor to open the Style and Standard Editor. Expand the Dimension style category, and then double-click a dimension style.
In the Dimension Style window, click New to create a style, if needed.
- In the New Style Name dialog box, accept the default "Copy of Default (xxx)" or enter a new name.
- Select the Add to Standard check box so the new style is available to all documents that use the standard. Click OK.
Click the Notes/Leaders tab to view the hole settings.
Select the hole and thread type.
In the Options box:
- Clear the check mark from Use Default to edit settings.
- If available, select Tap Drill to apply settings to selected hole and thread types.
- Select Part Units to use model units for hole notes.
- Click Precision and Tolerance to specify preferences for precision and tolerance parameters in the Precision and Tolerance dialog box.
- Click Apply to All to apply selected settings to all hole and thread types, including settings in the Precision and Tolerance dialog box.
Click Values and Symbols buttons to add their variable names in the edit box.
In the General Settings box:
- Click Edit Quantity Note to set contents of quantity notes in the dialog box.
- Click the arrow to select a Leader Style. If appropriate, click Edit Leader Style to close the dimension style and change leader style characteristics.
- Select the check box to set text justification.
- Click the arrow to select leader text orientation.
- Click the arrow to select leader text alignment relative to the landing line.
In Thread Note Settings, select Custom Designation to apply the custom thread designation field from the Thread.xls spreadsheet instead of the default note.
Select another hole and thread type and define its settings. Repeat for each hole type in the drawing.

NoteSave the settings before you close the dialog box.

Edit format for a selected hole note

In the drawing view, right-click a hole note, and select Edit Hole Note or double-click a hole note. In the Edit Hole Note dialog box, Hole Type, and Thread Type cannot be edited.
In the Options box:
- Clear the check mark from Use Default to edit settings.
- If available, select Tap Drill to apply settings to the selected hole and thread type.
- Select Part Units to use model units for the hole note.
- Click Precision and Tolerance to specify preferences for precision and tolerance parameters in the Precision and Tolerance dialog box.
- Click Edit Quantity Note to change settings in the Quantity Note dialog box.
In the edit box, click and Backspace to remove existing values.
Click Values and Symbols buttons to add their variable names in the edit box.
Click OK to apply the new settings to the selected hole note.

Set the default style for the feature control frame

Use the Styles and Standard Editor to set the attributes for feature control frames you add to a drawing.

Select Manage tab Styles and Standards panel Styles Editor to open the Style and Standard Editor dialog box.
Click to expand the Feature Control Frame listings in the browser and then double-click one of the styles.
On the General and Units tabs, set the desired attributes.
Click Save to save the default settings for the current document.

To make the settings available to all documents that use the style library, choose Manage tab Styles and Standards panel Save. You may not be able to save changes to the style library if it is locked to prevent unauthorized changes.

Set defaults for sketch and section hatching

The Standard and the Hatch style control hatching in drawings.

Hatch styles specify hatch attributes, for example, pattern or scale. If you edit a hatch style, all existing hatch objects that use the style change (only your overrides are kept).

You assign a Hatch style to the Section Hatch object and to the Sketch Hatch object in Object Defaults. The Hatch style is then used when you create a cut view or sketch hatch.

The Standard defines Material Hatch Pattern Defaults and Preset Values for the Section Hatch Angle. Both these properties control hatching in section views and other types of cut views.

TipChanges to the style settings are in effect for the current document only. Save the style to the style library to make it available to other documents.

Edit a hatch style

Edit the Hatch style to set the default hatch attributes for section and sketch hatches.

Select Manage tab Styles and Standards panel Styles Editor to open the Style and Standard Editor.
In the styles list, expand Hatch, and then click one of the listed Hatch styles.
TipTo create a Hatch style, click New, and specify the name of the new style.
On the Hatch Style panel, set hatch attributes:
- Select a pattern from the Pattern list.
- Set the pattern Angle, Scale, and Shift.
- Select Double to create a copy of the hatch rotated by 90 degrees.
- If appropriate, add a comment
To add a hatch pattern to the list:
- Select Other from the Pattern list.
- In the Select Hatch Pattern dialog box, select Offered for the hatch pattern to add in the Pattern list.
- Select a hatch pattern to use it as the default pattern in the Hatch style.
- Click OK to close the Select Hatch Pattern dialog box.
To load hatch patterns from an external PAT file:
- Select Other from the Pattern list.
- In the Select Hatch Pattern dialog box, click Load.
- In the Load Hatch Pattern dialog box, click the Explore Directories button to display the Select Hatch Pattern File dialog box.
- In the Select Hatch Pattern File dialog box, locate a PAT file, select it, and click Open. Valid hatch patterns from the selected PAT file display in the Load Hatch Patterns dialog box.
- Select one or more hatch patterns to load and click OK.
- In the Select Hatch Pattern File dialog box, select Offered for hatch patterns to add in the Pattern list of hatch-related dialog boxes.
- Select a hatch pattern to use it as the default pattern in the Hatch style.
- Click OK to close the Select Hatch Pattern dialog box.
Click Save to save the changes to the current document, and then click Done to close the dialog box.

NoteTo use a hatch style as the default, assign the hatch style to the Section Hatch or Sketch Hatch object type in Object Defaults.

Show Me how to define a hatch style and set it as the default for sketch hatch fills

Set default rotation angles for hatch patterns in section views

Default Section Hatch Angles for cut views are specified on the General tab of the Standard style pane. The final hatch rotation in cut views includes the default section hatch angle and the rotation angle defined in the Hatch style.

NoteThe default hatch rotation angles apply on creating section views. If the default setting changes, existing section views keep the hatch rotation angle as a property override.

Select Manage tab Styles and Standards panel Styles Editor to open the Style and Standard Editor.
In the styles list, expand Hatch, and then click one of the listed Hatch styles.
On the General tab in the Standard window, select Section Hatch Angle from the Preset Values list.
Edit the list of rotation angles. Click New to add a rotation angle to the list. Click Delete to remove a rotation angle from the list.
NoteAngles in the Preset Values list use the angle degree unit. You can enter deg or rad to specify the unit in the Add New Hatch Angle dialog box. Values in radians are automatically converted to degrees after you click OK or Apply in the Add New Hatch Angle dialog box.
Click Save to save the edits and click Done to close the Style and Standard Editor.

Map materials to hatch patterns

Mapping between materials and hatch patterns determines hatch patterns in cut views. If no hatch pattern is specified for a material, the hatch pattern from the current Hatch style is used.

Select Manage tab Styles and Standards panel Styles Editor to open the Style and Standard Editor.
In the styles list, expand Standard, and then click one of the listed standards.
Click the Material Hatch Pattern Defaults tab in the Standard window.
In the Default Hatch Pattern list, select the default hatch pattern for a new material added in the mapping.
Create a list of materials in the mapping table:
- Import materials from part files (click From File...), or from the material library (click From Library).
  TipChange the Default Hatch Style to correspond to the hatch style desired for the imported materials.
- Add materials to the list manually: Click at the last row in the table and enter the material name.
- To rename a material, select the corresponding row, and enter the new material name.
- To delete a material from the mapping table, select the material, right-click in the window, and click Delete.
Map materials to hatch patterns:
- To change the mapping for a material, click the Hatch Pattern field and select a new hatch pattern from the list.
- To change the mapping for several materials at the same time, use Ctrl or Shift to create a multiple selection. Then click the Hatch Pattern field corresponding to one of the selected materials, and select a new hatch pattern from the list.
Click Save to save the changes to the current document, and then click Done to close the dialog box.

Break hatching around drawing annotations

Select the Cross Hatch Clipping option on the Drawing tab of the Document Settings dialog box to break hatching around drawing annotations in cut views.

Notes:

To enable clipping around user-defined symbols, select the Symbol Clipping option for individual symbol instances.
The cross hatch clipping is not supported for datum targets and in isometric views.

TipHatching is clipped on the bounding box of note text. If appropriate, change the size of the bounding box to resize the clipped area.

Set the default parts list style

Use the Style and Standard Editor dialog box to add or modify the parts list style attributes. Changes affect the current document only unless you click Manage tab Styles and Standards panel Save.

Use caution if you save the new or changed default settings to the style library. You replace the current version in the style library that can affect other documents that reference the style.

Click Manage tab Styles and Standards panel Styles Editor. In the styles browser, expand the Parts List folder. Then select a parts list style from the list.
In the Parts List Style panel, set the default text style for parts lists. In the Heading and Table Settings area, set the heading and title options, text style, and other parts list properties.
Click Column Chooser to open the Column Chooser dialog box, and then define the columns to include in parts lists.
Click Grouping to open the Group Settings dialog box, and define keys for grouping parts list rows.
Click Filter to open the Filter Settings dialog box, and define parts list filters. Parts list filters specified in a parts list style are available for all parts list in the drawing which use the particular parts list style. If you disable the Filter option in the style, filters are not applied by default, but are available for a later use.
Use the parts list columns table to define default properties for parts list columns:
- Edit values in the table to change column headings and widths.
- To specify formatting attributes and substitution values, right-click an item in the Property column, and select Format Column. Then specify formatting attributes and substitution values in the Format Column dialog box.
Click Save to save the changed style in the current document, and then click Done to close the dialog box.

Set the default style for revision tables and tags

Use the Style and Standard Editor dialog box to set the default style for revision tables and tags.

Select Manage tab Styles and Standards panel Styles Editor to open the Style and Standard Editor dialog box.
Expand the Revision Table entry, and select the revision table style to change.
On the Revision Tables tab, set the defaults for revision tables.
On the Revision Tags tab, set the defaults for revision tags.
Add a comment, if appropriate.
Click Done to save the changes and close the Style and Standard Editor dialog box.

TipYou can access the Revision Tables style from the right-click menu. Select a revision table or revision tag on the drawing sheet, right-click, and then choose Edit Revision Table Style from the menu.

Set the default text style

The default text style in a drawing is defined by the active drafting standard.

Click Manage tab Styles and Standards panel Styles Editor to open the Style and Standard Editor.
In the dialog box, select a standard to base the style on.
Select a style name from the list, or select New to create a custom text style. If you create a style, Autodesk Inventor LT copies the default text style.
Rename the style with another name.
Set the text format by making selections in the dialog box.
Save the new text style and close the Style and Standard Editor.

Set the style for drawing views and view annotations

Use the Style and Standard Editor to edit the defaults for drawing views and view annotations.

NoteChanges affect the current document only unless you choose Manage tab

Styles and Standards panel

Save.

Edit the view style

On the ribbon, click Manage tab Styles and Standards panel Styles Editor.
In Style and Standard Editor, expand the Standard item. Then select a standard style from the list.
Select the View Preferences tab on the Standard panel.
Set the view label defaults for all types of drawing views from the View Type list:
- Select a View Type.
- Edit the label prefix.
- Select Constrain to Border to constrain the view label to the border of the drawing view.
- Select Use Delimiter to enable using two view label strings separated by a delimiter.
- Edit the view label text in the Display field. Click Insert View Scale or Insert View Identifier to insert the view scale or view identifier property into the Display field. If appropriate, click Edit View Label to edit the view label in the Format Text dialog box.You can add
  NoteModel properties to the view label in the Format Text dialog box. Model properties are ignored in view labels of sketch-based draft view.
- Specify the initial position of the view label to be Above or Below the drawing view.
- Click Toggle Label Visibility to set the label visibility.
Set the Default Thread Edge Display options for section views and top views.
Select the projection type.
Select the front view plane.
Click Save to save the style in the current document, and then click Done to close the dialog box.

Edit the view annotation style

On the ribbon, click Manage tab Styles and Standards panel Styles Editor.
In Style and Standard Editor, expand the View Annotations item. Then select a view annotation style from the list.
On the View Annotation Style panel, select each view type and then edit the settings:
Set defaults for annotation lines in the Format area:
- Select a thumbnail image to specify the appearance of the view definition line.
- For section views, set the Show Entire Row option to display or hide the section line in the base view.
- For auxiliary views, set the Definition in Base View options to display or hide the definition lines for broken-alignment and aligned auxiliary views.
- For detail views, set options for the view label with a leader in the Leader Format section. Select a leader line type from the list. Set the Draw Terminator option to control the display of the leader arrowhead (terminator). Set the orientation and alignment of the view label text on the leader.
In the Terminator area, set properties of the terminator: Specify the length of the leader extension line, select an arrowhead, and specify the arrowhead dimensions.
In the Text Style area, select a text style for view label texts. Click Edit Text Style to edit the selected text style.
If needed, add a comment to the Comments field.
Click Save to save the style in the current document, and then click Done to close the dialog box.

Note(View Identifier) When a section, detail, or auxiliary view is created, alphanumeric auto-indexing is used to generate the view identifier. The following characters are excluded from the indexing sequence by default: I, O, Q, S, X, and Z. You can customize the list of excluded characters on the General tab of the Standard Style panel.

Set default style for weld annotations

Use the Welding Symbol and Weld Bead styles to set the defaults for adding welding symbols, caterpillars, and end fills to a drawing. The weld styles also affect formatting for weld annotations recovered from the model.

Select Manage tab Styles and Standards panel Styles Editor to open the Style and Standard Editor.
In the style browser, click to expand the weld symbol or weld bead styles. Double-click a listed style to display it in the window.
In the Weld Symbol Style, set the desired options and then click Save.
In the Weld Bead Recovery window, set the options for caterpillars and end fills, and then click Save.
Click Done to close the dialog box.

NoteChanges to the style are in effect for the current document only. To make the changes available to all documents, select Manage tab

Styles and Standards panel

Save. The new styles replace the current style definitions. Use caution because the changes could affect other documents that use the style.

Override styles

The object defaults style determines the default layer on which an object resides and the default object style used by the object, if applicable. Using the Style and Standard Editor, you can:

Select the object defaults style to see a table of object types, the associated layer, and the associated object styles.
Change the default object style and layer.

Individual styles and layers for some objects can be overridden on placement or when edited by selecting a new style from the Styles list on the Annotate tab, Format panel. The change affects only the current object.

You can override the line type, line weight, scale and color for a selected edge, of a feature or part using the Edge Properties dialog box.

To override an edge property

In a drawing file, right-click a visible edge and select Properties from the context menu.
In the Edge Properties dialog box, select the drop-down arrow to change the Line Type and Line Weight.
Click the color swatch to change the color.
If applicable, select Scale, and enter a value in the scale text box.
NoteUse the Line Type dialog box to change the linetype to an autocad (LIN) line type.

To override placement of an object

When you select an object to place in a document, such as a datum target symbol, the layers list and the object style list on the Annotate tab have the default value of By Standard. You can select a layer or style before you place the object to override the default values.

On the Annotate tab, click the annotation object to place on the view.
In the Layers list, click the arrow to show available layers. The first option is By Standard, which indicates the object is being set to the layer defined by the active object default style. Click to select a different layer.
In the Style list, click the arrow to show options for the active standard. The first option is By Standard, which indicates the object is set to the active object default style. Click to select a different style.
Click to place the annotation object and then enter any required values.

The placed object is reformatted with the selected layer and style.

To override a selected object

You can change the style of a previously placed object.

In the graphics window, select the object to override.
In the Layers list, click the arrow and select a new layer from the list.
In the Style list, click the arrow and select a new object style from the list.

The selected object is reformatted with the new style.

To override multiple selected objects

You can select more than one object and change the layer for all.

In the graphics window, select the objects to override.
In the layers list, click the arrow and select a new layer from the list.

The selected objects are reformatted with the new layer.

You can also select more than one object and change the object style for all, if they use the same object style (for example, datum targets or dimensions).

In the graphics window, select the object to override.
In the Layers list, click the arrow and select a new layer from the list.
In the Style list, click the arrow and select a new object style from the list.

The selected objects are reformatted with the new style.

NoteTo change the default style of an object, edit the active object default style in the Style and Standard Editor or edit the standard to use a different object default style.

Load hatch patterns from an external PAT file

Select Other from the Pattern list on a hatch-related dialog box to open the Select Hatch Pattern dialog box. For example:
- Select hatching in a cut view, right-click, and click Edit. Then select Other from the Pattern list in the Edit Hatch Pattern dialog box.
- In an active drawing sketch, click Sketch tabDraw panel Fill/Hatch Region. Click a closed sketch profile in the graphic window. Select Other from the Pattern list in the Hatch/Color Fill dialog box.
- On the ribbon, click Manage tab Styles and Standards panel Styles Editor. Expand Hatch styles and click a Hatch style. Select Other from the Pattern list on the Hatch Style panel.
In the Select Hatch Pattern dialog box, click Load.
If appropriate, in the Load Hatch Pattern dialog box, click the Explore Directories button to display the Select Hatch Pattern File dialog box.
In the Select Hatch Pattern File dialog box, locate a PAT file, select it, and click Open. Valid hatch patterns from the selected PAT file display in the Load Hatch Patterns dialog box.
Select one or more hatch patterns to load and click OK.
In the Select Hatch Pattern File dialog box, select Offered for hatch patterns to add in the Pattern list of hatch-related dialog boxes.
Select a hatch pattern to use it as the default pattern in the Pattern list of the superordinate dialog box.
Click OK to close the Select Hatch Pattern dialog box.

TipExport hatches from a drawing to a PAT file: In the Select Hatch Pattern dialog box, select hatch patterns to export and click Export. Then specify the name of the destination PAT file.

Select Line Type (LIN file)

You can load and use line types from AutoCAD *.lin files as the line type for an Autodesk Inventor LT layer.

In a Drawing file (Autodesk Inventor LT Drawing or AutoCAD Drawing), select Annotate tab Format panel Edit Layers.
In the Styles Editor dialog box, select a layer, click the line type drop-list, and then select Other from the bottom of the list.
In the Select Line Type dialog box, click Load to load an additional line type.
In the Load Line Type dialog box, click Browse to find an additional line type from an external *.lin file.
In the Open dialog box, select the *.lin file, and then select Open.
In the Load Line Type dialog box, select the line type to add or SHIFT-select to load multiple line types, and then click OK.
In the Select Line Type dialog box, select a line type from the list to associate with the selected layer, and click OK.

References

Style and Standard Editor - Standard

The active standard determines the styles available for use in a drawing document. Individual styles may be edited in the current document, but the default values for all drawing objects originate with the standard.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, select a Standard style to edit.

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles, Styles in the Active Standard, or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

General tab

Sets format and values for general attributes.
Units	Sets the measurement options for the selected drawing standard. Linear sets the units of measurement. Substyles that refer to this standard use this setting. Click the arrow and select from the list. Decimal Marker specifies the character to use as a decimal. Substyles that refer to this standard use this setting. Click the arrow and select from the list.
Preset Values	Shows the value type displayed in the list. Line Weight, Text Height, Scale, or Section Hatch Angle sets the default values for drawings using the selected standard. Click the arrow to set the value type and then click a value to set. New opens the Add New Line Weight, Add New Text Height, Add New Scale, or Add New Hatch Angle dialog box. Enter a new value in the box, and then click OK to add it to the values list or click Apply to continue adding values. Add New Line Weight accepts only the default units. Add New Text Height accepts only the default units. Add New Scale accepts a new scale but does not validate its format. You can enter two examples of the same scale but with different formats and both are added to the list. Scale entries are grouped by format type in this order: decimal, fractional, multiple, architectural. Add New Hatch Angle accepts deg for degrees (the default unit), or rad for radians. Values in radians are automatically converted to degrees after you click OK or Apply in the Add New Hatch Angle dialog box. Click Cancel to close the dialog box without adding a value to the list. Delete deletes the selected value from the list.
Character Exclude	Edits the list of characters to exclude from automatic alphabetical indexing. List edits the list of excluded characters. Apply to selects drawing annotations where to exclude the listed characters. NoteThe Character Exclude setting applies to indexing of newly created views or table rows. Existing objects in the drawing are not affected.
Global Line Scale	Sets the scale of all line styles in drawings using this standard.
Standard Reference	Specifies drawing behavior specific to the selected standard, such as section view lines.
Comments	Enter a comment about the definition of a particular style, such as date created, created by, or derived from a particular standard.

View Preferences tab

Sets the view label defaults, thread edge display, projection type, and front view plane.

View Label Defaults:
View Type	Select each view type and edit the view label defaults for the selected view type.
Label Prefix	Edits the text to be used as a prefix to the view identifier.
Constrain to Drawing Border	If selected, the view label maintains its relative position to the view boundary.
Use Delimiter	Select Use Delimiter to use two view label strings separated by a delimiter. NoteThe delimiter line is displayed in the drawing regardless of contents of the lower text box.
Display	Edits the view label text.
Edit view label	Edits the text formatting and content of the view label in the Format Text dialog box. NoteThe formatting is not visible in the Display field but is applied to the view label in the drawing.
	Click Insert View Scale to insert the view scale at the cursor position in the text field.
	Click Insert View Identifier to insert the view identifier at the cursor position in the text field.
Position	Sets the default position of the view label. Above places the view label above the drawing view by default. Below places the view label below the drawing view by default.
	Toggle Label Visibility controls the default setting for visibility of the view label.

Default Thread Edge Display

Sets the appearance of thread edges in the drawing. Select the setting for section views and for top views.

Projection type

Sets the projection angle for drawing views. Click the image to select First Angle or Third Angle.

Front View Plane

Sets the preferred viewing plane to use as front view when creating a drawing view. Affects the orientation of all subsequent drawing views, but has no effect on existing views. Use the drop-down control to select Front View Plane as XY, YZ, XZ or From Model.

When From Model option is selected, front view orientation settings from model document are used to calculate view orientations in drawings.

Available Styles tab

Specifies referenced substyles for use with the standard. Some styles require another style to complete its definition. For example, dimension styles reference text styles to format dimension text.

Style Type lists styles specific to drawing documents, each of which may have multiple definitions. Click a style to display definitions.

Choose Styles to Use in Standard lists style definitions and comments, if available. Click the desired style definition to use in the current drawing document.

Object Defaults tab

Shows the current settings of the Object default style.
Active Object Defaults	Selects the object defaults in the active standard and lists them in the window.
Edit Object Defaults style	Activates the Object Defaults style, where you can edit one or more object defaults. For more information, see Style and Standard Editor - Object Defaults Styles.
Object Defaults view	Shows the settings of object defaults selected in the Active Object Defaults.

Material Hatch Pattern Defaults tab

Controls a mapping between materials and hatch patterns.
Default Hatch Pattern	Selects the default hatch pattern for a new material. NoteIf you import materials, all imported materials are mapped to the selected hatch pattern.
	Click the pencil to edit the selected style. When you save the style, the changes are in effect wherever the style is used.
Import Materials	From File... Click to import materials from a part file. Use the Open dialog box to locate the part file. From Library Click to import all materials names from the material library.
Thumbnail	Shows the hatch pattern corresponding to the selected hatch style.
Mapping Table	Displays a list of materials and corresponding hatch patterns. To add a material, click at the last row in the table, and enter the material name. To rename a material, select the corresponding row, and enter the new material name. To change the mapping for a material, click the Hatch Pattern field and select a new hatch pattern from the list. To change the mapping for several materials at the same time, use Ctrl or Shift to create a multiple selection, then click the Hatch Pattern field corresponding to a selected material, and select a new hatch pattern from the list. To delete a material from the mapping table, select the material, right-click in the window, and click Delete.

Style and Standard Editor - Object Defaults Styles

Sets the default object settings that control which styles are associated to an object, including a default layer attribute and a default object style (where applicable). All drawing objects are formatted by a standard and its associative styles.

The Object Defaults style is a substyle of the active standard style. In a drawing document, after a standard is selected, the active Object Default style specifies which layer and object style provides the format definition for a particular object.

Unlike other style types, only one Object Default style is available for each standard. When you select a standard, you set the active Object Default style.

NoteSome objects do not have associative object styles, such as visible and hidden edges.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Object Defaults. Click one of the listed styles to view or edit.

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles, Styles in the Active Standard, or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

The Object Defaults Styles window shows the styles to edit for the active standard, filters the listed objects, and contains comments. NoteClick the top of each column to change the sort order of the items.
Filter	Lists filter definitions. Default setting is All Objects, but the list may be restricted to only Dimension Objects, Leader Object, Model/View Objects, or Text Objects.
Comments	Enter a comment about the definition of a particular style, such as date created, created by, or derived from a particular standard.
Style Type Column	Shows the icon of the Object Style type. If the object has no associated object style, the cell is blank. Display only.
Object Type	Alphabetical list of objects available in a drawing document. Display only. See Objects and associated style types.
Object Style	Sets the default object style defined by the active standard. Select an item in the list and click the arrow to show available styles, and then click to select. See Filter type categories. For example, the Angle Dimension object type may show the Default (ANSI) Dimension style. The style list also includes all dimension styles defined in the active Standard style. You can select an alternate dimension style as the default for the Angle Dimension object.
Layer	Shows the layer style for each object in the Object Defaults list. The list includes all layers defined in the active Standard.

Object default style - Filter type categories

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Object Defaults.

Filter types are listed in the left column and available object types for each category in the right column:

Filter	Object Type
Dimension objects	Angle dimensions Baseline dimensions Diameter dimensions Hole notes Linear dimensions Ordinate dimension sets Ordinate dimensions Origin indicators Radial dimensions
Leader objects	Balloon Datum identifier symbol Datum target (all types) Feature control frame Feature identifier symbol Hole note Hole tag Leader text Origin indicator Revision tag Surface texture symbol Thread notes User-defined symbol (leader only) Weld symbol
Text objects	3D Sketch Geometry Border Text Chamfer Note Configuration Table General Table Leader text Sketch Text Text (General Note) Title Block Text User Defined Symbol Text View/Scale Label
Model/View objects	Auxiliary View Line Break Line Break Out Line Crop Cut Line Detail Cut Line Detail View Callout Hatching Hidden Interference Edge Hidden Simplified Representation Hidden Tangent Edge Hidden Thread Ends Hidden Thread Lines Hidden View Edge Model Weld Annotations Model Weld Symbols Presentation View Trail Line Reference Part Edges Section View Line Sheet Metal Bend Centerline (+) Sheet Metal Bend Centerline (-) Sheet Metal Bend Extent Sheet Metal Punch Center Sheet Metal Roll Centerline Thread Ends Thread Lines Visible Interference Edge Visible Simplified Representation Visible Tangent Edge Visible View Edge Work Axis Work Plane Work Point

Object Defaults style - Objects and associated Style Types

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Object Defaults.

The left column shows a complete list of objects available in drawings and the right column shows the default associated object style.

TipUse this list to help you understand which objects are associated with the same style. For example, all objects associated with DIM STYLE have the same dimension style icon.

3D sketch geometry	NONE
Angle dimension	DEFAULT
Auxiliary View Line	VIEW ANNOTATION STYLE
Balloon	BALLOON STYLE
Baseline dimension	DEFAULT
Border Geometry	NONE
Border Text	NOTE TEXT
Break Line	NONE
Break Out Line	NONE
Caterpillar	WELD BEAD RECOVERY STYLE
Center Mark	CENTER MARK STYLE
Center of Gravity	CENTER MARK STYLE
Centerline	CENTER MARK STYLE
Chamfer Note	DEFAULT
Configuration Table	TABLE
Crop Cut Line	NONE
Datum ID symbol	ID STYLE
Datum target	DATUM TARGET STYLE
Detail cut line	NONE
Detail view callout	VIEW ANNOTATION STYLE
Diameter dimension	DEFAULT
End treatment	WELD BEAD RECOVERY STYLE
Feature control frame	FEATURE CONTROL FRAME STYLE
Feature ID symbol	DATUM ID STYLE
General Table	TABLE STYLE
Hatching	HATCH STYLE
Hidden Interference Edge	NONE
Hidden Simplified Representation	NONE
Hidden Tangent Edge	NONE
Hidden Thread Ends	NONE
Hidden Thread Lines	NONE
Hidden View Edge	NONE
Hole Note	DEFAULT
Hole Table	HOLE TABLE STYLE
Hole Tag	DEFAULT
Leader Text	DEFAULT
Linear Dimension	DEFAULT
Ordinate Dimension	DEFAULT
Ordinate Dimension Set	DEFAULT
Origin Indicator	GENERAL
Overlay View	NONE
Parts List	PARTS LIST STYLE
Presentation view trail line	NONE
Radial Dimension	DEFAULT
Reference Part Edge	NONE
Revision Table	REVISION TABLE STYLE
Revision Tag	REVISION TABLE STYLE
Section View Line	VIEW ANNOTATION STYLE
Sheet Metal Bend Centerline (+)	NONE
Sheet Metal Bend Centerline (-)	NONE
Sheet Metal Bend Extent	NONE
Sheet Metal Punch Center	CENTER MARK STYLE
Sheet Metal Roll Centerline	NONE
Sketch fill/hatch	HATCH STYLE
Sketch geometry	NONE
Sketch text	NOTE TEXT STYLE
Surface texture	SURFACE TEXTURE STYLE
Text (general note)	TEXT STYLE
Thread Ends	NONE
Thread Lines	NONE
Thread Note	DEFAULT
Title Block Geometry	NONE
Title Block Text	NOTE TEXT STYLE
User Defined Symbols (leader only)	GENERAL STYLE
User Defined Symbol Geometry	NONE
User Defined Symbol Text	NOTE TEXT STYLE
View/Scale Label	LABEL TEXT STYLE
Visible Interference Edge	NONE
Visible Simplified Representation	NONE
Visible Tangent Edge	NONE
Visible View Edge	NONE
Weld symbol	WELD SYMBOL STYLE
Work Axis	CENTER MARK STYLE
Work Plane	CENTER MARK STYLE
Work Point	CENTER MARK STYLE

Style and Standard Editor - Balloon Style

Specifies the format of balloons used to annotate drawing views. Balloons identify an item in a parts list. The number in the balloon corresponds with the part number in the parts list.

The Balloon style is a substyle of the active standard.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Balloon. If available, click one of the listed styles to view or edit.

If you prefer, right-click a balloon, and then select Edit Balloon Style.

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles, Styles in the Active Standard, or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

Set balloon attributes in the Balloon Style window:

Substyles specify styles required to define a balloon. The attributes of the leader, alternate leader, and text styles are defined in their own style; balloons reference those attributes for formatting those objects.
	Some substyles can be edited while defining the parent. Click the pencil to edit the selected style. When you save the style, the changes are in effect wherever the style is used.
Leader Style	Click the arrow to list leader styles in the active standard. Click the pencil to open the leader style for editing.
Alternate Leader Style	Click the arrow to list alternate leader styles in the active standard. Alternate leader style is used when a balloon termination is dragged away from its associative edge.
Text Style	Click the arrow to list text styles in the active standard. Balloon text is formatted with this style.

Balloon Formatting specifies attributes for the balloon size and shape.
Shape	Click the arrow to list and select balloon shape.
Property Display	Displays properties specified in the Property Chooser dialog box. Click the command to select or define properties. Selected multiple properties are listed, separated by commas. Balloon shape controls the number of properties displayed.
Symbol Size	Select the Scale to Text Height check box to size the balloon by text height. Not available if the balloon shape is None or Linear.
Size	Clear the Scale to Text Height check box to enter a balloon diameter in linear units, independent of text height. You can enter any unit type and it is converted, if required, according to the specified unit type. Select the Stretch Balloon to Text check box to size the balloon horizontally to accommodate long text strings. Clear the check box to restrict the balloon to the defined size. Not available if the balloon shape is None or Linear.

Default Offset sets the default distance between balloons when you align them. The changed value has no effect on previously created balloons.

In Comments, enter information about the definition of a particular style, such as date created, created by, or derived from a particular standard.

Style and Standard Editor - Center Mark Style

Sets the attributes for manual and automatic center marks and centerlines. The Center Mark style is used by center marks, centerlines, bisector centerlines, centered patterns, work points, work axes, and work planes. Each portion of the center mark may be sized individually.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Center Mark. Click a listed style to view or edit.

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles, Active Standard, or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

Set attributes in the Center Mark Style window:

Individual values correspond to lettered items on the image.
Mark	Sets the size of the center indicator mark.
Gap	Sets the gap distance between the center indicator and the extension line.
Overshoot	Sets the distance that center mark extension lines extend beyond the edges of the features that they define.
Extension	Sets the minimum length of center mark extension lines.
Default Radius	Sets the size of a sick center mark if it is left detached from geometry.
Comments	Enter information about the definition of a particular style, such as date created, created by, or derived from a particular standard.

Style and Standard Editor - Datum Target Style

Sets the formatting attributes for datum target symbols.

The datum target style is a substyle of the standard, but its format may be defined independently of the active standard style.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Datum Target. Click one of the listed styles to view or edit.

If you prefer, right-click a datum target, and then select Edit Datum Target Style.

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles, Styles in the Active Standard, or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

General tab

Substyles are used to define aspects of other styles. The Datum Target style requires leader and text styles as substyles to define the leader formatting and text font.
	Some substyles can be edited while defining the parent style. Click the pencil to edit the selected style. When you save the style, the changes are in effect wherever the style is used.
Leader style	Lists all available leader styles in the active standard.
Text style	Lists available text styles in the active standard.

Symbol Size specifies the symbol size in the text height specified in the Leader style.
Scale to text height	Sizes the bounding shape of the datum target (square, circle, or underline) as the defined text height.
Size	Unavailable if the Scale to Text Height check box is selected. Clear the check box to specify the bounding shape in linear units, independent of text height.

Target Point sets the attributes of datum target points.
Size	Sets the size of the target points. Enter the desired size in the box.
Color	Specifies the color of the target points. Click the color button to display the Color dialog box, and then choose the color.

Area Hatch sets the characteristics of the datum target hatch pattern.
Distance	Sets the spacing between hatch lines. Enter the distance in the box.
Angle	Sets the angle of the hatch for rectangular and circular datum target symbols. Enter the angle in the box.

Line Type sets the line types used by the datum target symbol.

When the line type is set to By Standard, the line type is controlled by the layer on which the Datum Target resides.

Hidden Leader

Sets the line style for hidden leader lines. Click the arrow, and then select a line type from the list.

Boundary

Sets the line style for boundary lines. Click the arrow, and then select a line type from the list.

Enter a Comment about the definition of a particular style, such as date created, created by, or derived from a particular standard.

Units tab

For more information about units, see Units reference.

Style and Standard Editor - Feature Control Frame Style

Specifies the content of a feature control frame. The feature control frame can be stand-alone or attached to a drawing view with a leader line.

The feature control frame style is a substyle of the standard, but its format can be defined independently of the active standard style.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the browser, expand the Feature Control Frame item, and then select a Feature Control Frame style to edit.

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles, Styles in the Active Standard, or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

On the Manage tab, Styles and Standards panel, you can use also these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

General tab

Values set on the General tab are used to specify symbol attributes when creating feature control frames using the Feature Control Frame dialog box.

Geometric Dimensioning and Tolerancing sets the availability of feature control frame symbols. Click the drop-down list and select symbols to view, then select the check box beside symbols to include in the list. Unchecked symbols are filtered out of the list. Selected symbols are available on the Feature Control Frame dialog box.
Geometric Characteristic	Indicates characteristics of the geometry for manufacturing purposes.
Material Removal Modifier	Indicates conditions to meet when material is removed during machining. Modifier characters are added to text at the insertion point in the drawing.
Additional Symbols	Indicated additional symbols used during the design.

Substyles are required by the feature control frame style to define fully. In this case, the feature control frame style is the parent style to leader and text styles.
	Some substyles can be edited while defining the parent style. Click the pencil to edit the selected style. When you save the style, the changes are in effect wherever the style is used.
Leader Style	Lists available leader styles in the active standard. Selection determines appearance of leaders associated with feature control frames.
Text Style	Lists available text styles in the active standard. Selection determines size and font of text in the feature control frame.

Symbol Size is specified relative to text height or independently, appropriate white space is set and applicable comments entered, if appropriate.
Scale to Text Height	Select the check box to size feature control frame symbols to the text height. This value is specified in the Leader style. Clear the check box to size the symbol independent of text height.
Size	Unavailable if the Scale to Text Height check box is selected. If unselected, sets the size of feature control frame symbols, expressed in linear units.
White Space	Sets the space before and after text in the tolerance and datum cells. Enter the amount of white space in the box in linear units.
Comments	Enter a comment about the definition of a particular style, such as date created, created by, or derived from a particular standard.

Options specify appearance of data cells, tolerances, and datum ID symbol.
Merge	For Symbol, Tolerance, and Datum data, specifies whether to combine cells when the data is the same. Click a button to alternate between merging and separating the cells.
Cell Alignment	Adds space to short cells so that pairs of cells align vertically.
Datum Alignment	Available only if Cell Alignment option is switched on. Adds space to Datum ID cell so it is vertically aligned with symbols cells.
Leader Attachment	Controls how a leader is attached to the feature control frame symbol. If selected, the leader is attached to the corner of frame; if not selected, the leader is attached to the middle of frame.
Italicize Datums	Check the box to include datums to be displayed in italic font.
Allow Tolerance 2	Select the check box to enter a second tolerance value in the Feature Control Frame dialog box. Unavailable when the check box is cleared.
Datum Leader Side	Available only if a leader is attached to the corner of frame . Select the check box to position the datum box on the leader side.

Units tab

For more information about units, see Units reference.

Style and Standard Editor - Hatch Style

The Hatch style specifies hatch attributes, for example, pattern or scale. If you edit a hatch style, all existing hatch objects that use the style change (only your overrides are kept).

Notes:

The layer on which the hatch object is created defines the hatch line weight and color. You can override these hatch attributes for hatch objects in the drawing.
Object Defaults set the default Hatch style for Section Hatch and Sketch Hatch objects

The layer on which the hatch object is created defines the hatch line weight and color.

Object Defaults set the default Hatch style for Section Hatch and Sketch Hatch objects.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, expand Hatch, and then select a Hatch style to edit.

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles, Styles in the Active Standard, or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

Pattern	Selects a hatch pattern. Select Other to add hatch patterns to the Pattern list using the Select Hatch Pattern dialog box.
Angle	Rotates the hatch pattern by the specified angle. Enter the desired angle.
Scale	Sets the distance between lines in the hatch. A scale of 1 uses the original distance specified in the hatch pattern. A scale of 0.5 results in line spacing that is one half of the original distance.
Shift	Shifts the hatch pattern to offset it slightly from the original hatch pattern position. Enter the distance for the shift.
Double	Creates a copy of the specified hatch pattern perpendicular to the first hatch pattern.
Comments	Enter a comment about the definition of a particular style, such as date created, created by, or derived from a particular standard.

Style and Standard Editor reference - Hole Table Style

Sets the format for hole table styles used in drawings. The hole table style is a substyle of the standard.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Hole Table. Click one of the listed styles to view or edit.

For the current document, you can click:

New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles or All Styles in the browser.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

Formatting

Sets attributes for hole table formatting.
Title	Sets the text to appear in the hole table title cell.
Text Styles	Sets the default text styles for Title, Column Header, and Data in hole tables. Text formatting is specified in the referenced Text style.
		Click the pencil to open the referenced Text Style. When you save the style, the changes affect wherever the style is used. If you changed the parent style, save changes before you can edit the substyle.
Line Format	Click Outside or Inside to specify the lines to format with Line Weight and Color.
		Line Weight sets By Layer as the default or click the arrow to select a different line weight. Values originate with preset values for line weight on the Standard style.
		Color opens the Color dialog box which controls the color of inner and outer lines of the hole table. By Layer is the default.
Heading	Selects heading position in the hole table. Click arrow to select Top, Bottom, or No Heading. Unlike the parts list dialog box, No Heading does not remove column headers from the table.
Default Column Settings	Specifies the format of hole table columns.
		Column chooser opens the Hole Table Column Chooser dialog box. Lists available properties and selected properties. Click Add and Remove to move properties from one column to another. Click Move Down or Move Up to change the order of the properties. Click New Property to open the Define New Property dialog box. Click Delete to remove a column from the table.
		Property shows the selected columns that appear in the hole table. Right-click to open the Column Chooser or Format Column dialog boxes.
		Column shows the selected column header names. Modify the appearance of the column header text by changing the text. Resize the column by clicking and dragging the column separator.
		Width sets the width of the hole table columns. Enter a specific width for each column or click and drag to resize after the hole table is created.
In Comments enter information about the definition of a particular style, such as date created, created by, or derived from a particular standard.

Options

Sets defaults for row merging, hole tags, tag order, and view filters.

Row Merge Options sets default for merging hole table rows.

None	Preserves legacy hole table formatting. Reformat Table on Custom Hole Match reindexes the hole tags and resorts contents when a Match Custom Hole operation is done. Numbering replaces the alphanumeric hole tags with sequential numbering of the holes in the hole table.
Rollup	Combines the hole note cells for the holes of the same type in the hole table. Only the first hole in a series is still listed in the table. The rolled-up cell adopts the formatting of the first row (hole) in the series. Delete Tags on Rollup preserves legacy behavior. Except for the first in a series of hole tags, deletes tags from the associative view. Clear the check box to preserve tags. Secondary Tag Modifier on Rollup causes all hole tags in the table and view to include the secondary numerator. Clear the check box to drop the secondary modifier. For example, A1, A2, and B1 become A, A, and B.
Combine Notes	Combines description cells for the holes of the same type in the selected hole table. Reformat Table on Custom Hole Match reindexes the hole tags and resorts contents when a Match Custom Hole operation is done. Numbering replaces the alphanumeric hole tags with sequential numbering of the holes in the hole table.
Hole Tag Options sets defaults for formatting hole tags.
	Preserve Tagging causes permanent hole identifiers for each hole tagged when the table is first placed. Clear the check box to respecify holes when holes are added or deleted from the model). Tagging is preserved only with respect to changes to the model, such as when you add, delete, suppress or unsuppress hole features. Manual changes to the hole table, such as when you resort, change tag order, and filter hole types, are not affected.
	Use Leader generates a leader for any hole tag dragged away from the hole with which it is associated. Clear the check box to hide the leader of hole tags dragged away from an associated hole automatically.
Default Tag Order sets default tag order of holes in a hole chart. Existing hole tables are not affected by these settings.
	Arrange by Position tags holes relative to their position on the selected view. Position is arranged with YDIM as the primary key and XDIM as secondary key. If YDIM and XDIM are equal, hole size is the tertiary sorting key, smallest to largest. Arrange by Size tags holes in order by size (smallest to largest). Size refers to the drill diameter (HDIA) parameter for drilled, counterbored, and countersunk holes. The tap drill diameter (TDDIA) is used for threaded holes. If holes are of equal size, holes are sorted by position. Group Hole Types must be unselected. Holes added from a center mark are added to the end of the list. Group Hole Types tags holes by hole type and then by choice of size or position. Existing hole tables are not affected by these settings. The group order is:
		Drilled holes includes extruded cut circles and circular voids. Thru Blind
		Threaded holes Thru: Full Thread, Depth Thread Blind: Full Thread, Depth Thread
		Counterbored holes and Countersunk holes. If a counterbored or countersunk hole is tapped, the tapped designation is disregarded for grouping. Thru Blind
		Center marks
Default Filters (View) sets defaults for features and hole types to include in a view-based hole table. Existing hole tables are not affected by these settings.
	Included Features selects features to include or exclude in views-based hole tables. Select a check box to include hole features, circular cuts, and center marks or clear the check box to exclude them. Hole features allows view-based hole tables to include hole features. Circular cuts allows view-based hole tables to include extruded cuts. Clear the check box to exclude extruded circular cuts from view-based hole tables. Circular cuts are recognized only as drilled thru or drilled blind holes. Center marks allows view-based hole tables to include entries with center marks. Clear the check box to exclude center marks from view-based hole tables. Center marks with visibility turned off are not included in hole tables. Included Hole Types selects hole types to include or exclude in view-based hole tables. Select a check box to include drilled, counterbored, countersunk, or threaded holes. Clear a check box to exclude the hole type from view-based hole tables. Not available if hole features are excluded from view-based hole tables. Drilled holes includes drilled hole features in view-based hole tables. Counterbored holes includes counterbored hole features in view-based hole tables. May be selected when creating selection-based or feature-based hole tables. Clear the check box to exclude from new view-based hole tables, and make edges or counterbored holes unselectable after you add a hole or create a selection-based or feature-based hole table. Threaded holes includes threaded holes in view-based hole tables. Allows selection of threaded holes for adding holes or creating selection-based and feature-based hole tables. Clear the check box to exclude threaded hole features when adding holes or creating a selection-based or feature-based hole table, and when creating new view-based hole tables. Makes edges of threaded hole features unselectable after you add holes or create selection-based or feature-based hole tables. Countersunk holes includes countersunk holes in view-based hole tables. Allows selection of countersunk holes for adding holes or creating selection-based and feature-based hole tables. Clear the check box to exclude countersunk hole features when adding holes or creating a selection-based or feature-based hole table, and when creating new view-based hole tables. Makes edges of countersunk hole features unselectable after you add holes or create selection-based or feature-based hole tables.

Style and Standard Editor - ID Style

Controls formatting for datum ID and feature ID. The ID style is a substyle of the standard, but its format may be defined independently of the active standard style.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the browser pane, click one of the listed ID styles to display its attributes in the window.

If you prefer, right-click a feature or datum ID, and then select Edit Style.

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles, Styles in the Active Standard, or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

Click a Datum ID style to show its attributes.

Substyles

The ID style requires leader and text styles as substyles to define the leader formatting and text font.
	Some substyles can be edited while defining the parent style. Click the pencil to edit the selected style. When you save the style, the changes are in effect wherever the style is used.
Leader style	Lists all available leader styles in the active standard.
Text style	Lists available text styles in the active standard.

Symbol Size

Specifies the symbol size in the unit type specified in the active standard.
Scale to text height	Sizes the bounding shape of the ID (square, circle, or underline) relative to the text height.
Size	Unavailable if the Scale to Text Height check box is selected. Clear the check box to specify the bounding shape in linear units, independent of text height.

Symbol Properties

Specifies the shape, orientation, and the leader landing for the symbol.
Shape	Lists four options for the bounding shape around the ID text (none, rectangle, circle, or underline. Click one to select.
Orientation	Specifies the rotation of the ID symbol when a leader is not used. Click to view the position.
		Orients the ID normal to a selected line or tangent to a selected arc.
		Orients the ID to be horizontal regardless of the orientation of the selected geometry.
Allow Landing	Select the check box to create a horizontal or vertical landing at the end of the last leader segment. Clear the check box if you do not want to create a landing segment.

Comments

Enter a comment about the definition of a particular style, such as date created, created by, or derived from a particular standard.

Standards and Styles Editor - Layers Style

The Layer Style specifies a layer name and attributes for common display properties of drawing objects. Layers visibility turned On or Off in a drawing. The visibility setting is stored in the drawing, not the style library.

All object types and their associated layers are listed in the Object Defaults style, a substyle of the standard style. The Layers Style window presents all layers in a table for editing.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Layers. Click one of the listed layers to edit.

Access:

Ribbon: Annotate tab

Format panel

Edit Layers. In the Style and Standard Editor dialog box, click Layers. Click one of the listed layers to edit.

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles, Styles in the Active Standard, or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to remove unused styles and substyles from the current document.

In the Layer Styles window, modify layer attributes as needed.

NoteChanges to layer attributes are saved only in the current document. To replace the style definition in the Style Library, click Manage tab

Styles and Standards panel

Update.

Click a column heading to reverse the sort order.
Edit pencil	Indicates the layer selected for editing.
Layer Name	Lists layer names in alphabetical order.
On	Sets visibility of a layer. Default setting is On. Click to turn Off. NoteThe layer visibility is not saved to the styles library. You change the layer visibility for a particular drawing.
Color	Sets the layer color. In the drawing, objects on the layer are visible in the selected color. When this column is sorted, the layers are in RGB order, and other layers by alphabetical order.
Line Type	Sets the layer line type. Click to see the current line type and select from the list. Click the line type column heading to sort by the fixed line type order. NoteTo load linetypes from an AutoCAD .lin file, select Other from the bottom of the Line Type list.
Line Weight	Sets thickness of the lines on the layer. Click to enter a value or select a predefined weight from the list. Click the column header to sort by line weight.
Scale by Line Weight	Select the check box to scale the line type based on the line weight. As the line weight increases, the length of segments and spaces in the line pattern also increase. Imported line types in DWG files usually have this setting turned off. Clear the check box to import line types in DWG files without distortion.
Plot	Controls whether the selected layer is plotted. Select the plot icon to switch the plot property to On/Off. When the plot property is set to OFF, the layer continues to display in the drawing, but it does not print or get published .
Add new layers to standard	Select the check box to add newly created layers to the current standard. Clear the check box to add new layers only to the current document.

Style and Standard Editor - Leader Style

Sets attributes for the leader arrowhead, size and weight of the leader terminator, line format, and extension line.

The Leader style is typically referenced by other styles as a substyle. Styles that use the Leader style for formatting include the Feature Control Frame style, Datum Target style, Balloon style, Surface Texture style, Weld Symbol style, and ID style.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Leader. If available, click one of the listed styles to view or edit.

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles, Styles in the Active Standard, or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

Set Leader Style attributes in the Leader Style window.

Terminator

Sets the default arrowhead type and size for the selected leader style.
Arrowhead	Sets the default arrowhead type. Click the arrow to select an arrowhead from the list.
Size (X)	Sets the size of the default arrowhead. Enter a value for width if the terminator is an arrowhead or for diameter if the terminator is a circle.
Height (Y)	Sets the height of the arrowhead relative to the associated line. Enter a value in the box. Not available if the arrowhead selection is not Open, Blank, Closed, or Filled.

Line Format

Specifies the attributes of the line portion of the leader style. By Layer sets the line type or line weight of the leader portion of the object to define by the layer on which the object resides.
Line Type	Lists all line types defined in the active standard.
Line Weight	Lists all line weights defined in the active standard.
Color	Specifies the color of the leader line.

Extension Line

Specifies the offset and overshoot of an extension line created when an arrowhead or other terminator is dragged off of a selected edge.
Extension Line Offset	Sets the space from the end of the selected edge to the beginning of the leader extension line.
Extension Line Overshoot	Defines the length of the leader extension line past the end of the terminator.

All-Around Symbol

Specifies the size of the all-around symbol for Feature Control Frames, Surface symbols, and Weld symbols (circular only).
Scale to Text Height	Select the check box to define the all-around symbol size by the height of text from the text style of the style. Clear the check box to size the symbol independent of the text height.
Diameter	Not available if Scale to Text Height is selected. If unselected, enter a specific symbol size in linear units, independent of text height. Enter units or leave blank to use default units.

Attached Text Position

Specifies the position of the text attached to the leaders on the drawings.
First Above Leader	Select to place the first line of text above the leader. All additional lines are placed below the leader. When you attach only one line of text to the drawing, it is always displayed above the leader.
All Above Leader	Select to place all lines of text above the leader.

Comments

Enter information about the definition of a particular style, such as date created, created by, or derived from a particular standard.

Style and Standard Editor - Parts List Style

Sets the default configuration for the parts list in a drawing or template file.

The Parts List style is a substyle of the active standard style. Its values are linked values. Changes made to parts list attributes affect all parts list objects associated with the standard.

The default values may be changed, but doing so overrides the style in the current document. To reset the value, reapply the style.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Parts List. If available, click one of the listed styles to view or edit.

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles, Styles in the Active Standard, or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

Set Parts List attributes in the Parts List Style window.
Heading and Table Settings specify the format of the title, text styles, and rows of the table.
Title	Assigns a default title for parts lists. Select the check box to show the title on the Parts List in the drawing. Type the title in the box. Clear the check box to remove a title from the parts list.
Text Styles	Sets the default text styles for Title, Column Header, and Data in parts lists. Text formatting is specified in the referenced Text style.
		Click the pencil to open the referenced Text Style. When you save the style, the changes affect wherever the style is used. If you changed the parent style, save changes before you can edit the substyle.
Heading Gap	Sets the vertical space between the text and the cell frame for the parts list heading row. Enter the appropriate space in the box.
Row Gap	Sets the vertical space between the text and the cell frame for the parts list rows. Enter the appropriate space in the box.
Heading	Specifies the formatting of the parts list heading. Click the arrow to select Top, Bottom, or None.
Line Spacing	Sets the line spacing for each row in the parts list. Click the arrow to specify One, Two, or Three lines of text.
Direction	Specifies the default display direction for the parts list. Click the appropriate direction to display the list from the bottom up or the top down.
Default Columns Settings specify the columns to include in the parts list, and group and filtering options.
	Click Column Chooser to open the Parts List Column Chooser dialog box to select columns to include in the parts list.
	Click Grouping to open the Group Settings dialog box and select properties to be used as grouping keys.
	Click Filter to define one or more parts list filters in the Filter Settings dialog box.
Column formatting grid	Shows the format of the parts list. Click the edge of a column header and drag to resize. The Property column lists the selected properties in rows. Right-click a row to open the Column Chooser, Grouping, or Format Column dialog box. Column lists heading names for columns in parts lists. Click in the row to enter a different name. Width sets the default width for each column. Click in the row to enter a different width.
Comments	Enter information about the definition of a particular style, such as date created, created by, or derived from a particular standard.

Style and Standard Editor - Revision Tags tab

Specifies the format for revision tags. The revision tag style is a substyle of the active standard.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor. In the Style and Standard Editor dialog box, expand the Revision Table entry, and click a style.

Alternate method: Right-click a revision tag, and then select Edit Revision Table Style.

Substyles:
Leader Style	Select the default leader style from the list. Click the pencil to open the leader style for editing.
Text Style	Select the default text style from the list.

Some substyles can be edited while defining the parent. Click the pencil to edit the selected style. When you save the style, the changes are in effect wherever the style is used.

Revision Tag Formatting:
Shape	Click the arrow to list and select balloon shape.
Allow Landing Line	Controls if the landing is added to the revision tag.

Style and Standard Editor - Revision Tables tab

Sets the default style for revision tables. The revision table style is a substyle of the standard.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Revision Table. Click one of the listed styles to view or edit.

For the current document, you can click:

New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles or All Styles in the browser.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

Title	Sets the text to appear in the revision table title cell.
Line Format	Click Outside or Inside to specify the lines to format with Line Weight and Color. Line Weight sets By Layer as the default or click the arrow to select a different line weight. Values originate with preset values for line weight on the Standard style. Color opens the Color dialog box which controls the color of inner and outer lines of the revision table. By Layer is the default.
Text Styles	Sets the default text styles for Title, Column Header, and Data in revision tables. Text formatting is specified in the referenced Text style.
		Click the pencil to open the referenced Text Style. When you save the style, the changes affect wherever the style is used. If you changed the parent style, save changes before you can edit the substyle.
Row Gap	Specifies the space between the text and row separator line, above and below the text in the data area.
Heading Gap	Specifies the space above the heading.
Heading	Selects the heading position in the table, the space between the text and row separator line, above and below the text in the heading area. Click the arrow to select Top, Bottom, or No Heading.
Line Spacing	Specifies the number of text rows reserved in each table cell in the data area. Click the arrow to select.
Direction	Sets the display direction for rows in the table. Click the appropriate direction to display the text from the bottom up or the top down.
Default Column Settings	Specifies the format of revision table columns.
		Column chooser opens the Revision Table Column Chooser dialog box. Lists available properties and selected properties. Click Add and Remove to move properties from one column to another. Click Move Down or Move Up to change the order of the properties. Click New Property to open the Define New Property dialog box. Click Delete to remove a column from the table.
		Property shows the selected columns that appear in the revision table. Right-click to open the Column Chooser or Format Column dialog boxes.
		Column shows the selected column header names. Modify the appearance of the column header text by changing the text. Resize the column by clicking and dragging the column separator.
		Width sets the width of the revision table columns. Enter a specific width for each column or click and drag to resize after the revision table is created.
In Comments enter information about the definition of a particular style, such as date created, created by, or derived from a particular standard.

Standards and Styles Editor - Surface Texture Style

Sets the attributes for surface texture symbols. The Surface Texture Style is a substyle of the standard.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Surface Texture. If available, click one of the listed styles to view or edit.

If you prefer, right-click a surface texture symbol in a drawing, and then select Edit Surface Texture Style.

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles, Styles in the Active Standard, or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

Set formatting attributes in the Surface Texture Style window:

Lay Symbol Filter lists all defined machining lay symbols. Select the check box to include the symbol or clear the check box to make it unavailable in the Surface Texture dialog box.

Substyles are required by the surface texture style to define fully. In this case, the surface texture style is the parent style to leader and text styles.
	Some substyles can be edited while defining the parent style. Click the pencil to edit the selected style. When you save the style, the changes are in effect wherever the style is used.
Leader Style	Lists available leader styles in the active standard. Selection determines appearance of leaders associated with surface textures.
Text Style	Lists available text styles in the active standard. Selection determines size and font of text used when numbers are entered with a surface texture.

Symbol

Sets the size of the machining-prohibited symbol. Click the button to switch between the options.

Standard Reference

Specifies the drafting standard that controls surface texture symbol format. Click the arrow to select the desired standard.

The drafting standard can be different from the active standard style. For example, the default value of the Surface Texture style (BSI) is BSI. The surface symbol uses this value to create symbols and compute its extents, such as height.

Comments

Enter a comment about the definition of a particular style, such as date created, created by, or derived from a particular standard.

Style and Standard Editor - Table Style

Sets the format of inspection dimension tables and other industry-specific tables.

You can define table formatting by using the Styles Editor to create a Table style. The Table style is a substyle of the active standard, uses Text as a substyle, and can be exported individually or as part of an exported standard style. Except for the default Table style, you can apply table styles to other tables to reformat them.

NoteYou can reformat tables used in drawings by editing the table and changing the style to which it refers.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Table. Click one of the listed styles to view or edit.

For the current document, you can click:

New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles or All Styles in the browser.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

General formatting

Sets preferences for tables formatted by the table style.
Title	Select the check box to specify a title row. If appropriate, enter text to display in the title row of the table. If you do not specify a title in the table style, tables that reference .csv or .xls files use the file name as the title.
Line Format	Click Outside or Inside to specify the lines to format Line Weight and Color. Line Weight sets By Layer as the default or click the arrow to select a different line weight. Values originate with preset values for line weight on the Standard style. Color opens the Color dialog box which controls the color of inner and outer lines of the table. By Layer is the default.
Text Styles	Specifies the text formats for the Title, Column Header, and Data.
		Click to edit the text style and specify paragraph settings, color, justification, character formatting, and an optional comment.
Row Gap	Specifies the space between the text and row separator line, above and below the text in the data area.
Heading Gap	Specifies the space above the heading.
Heading	Selects the heading position in the table, the space between the text and row separator line, above and below the text in the heading area. Click the arrow to select Top, Bottom, or No Heading.
Line Spacing	Specifies the number of text rows reserved in each table cell in the data area. Click the arrow to select.
Direction	Sets the display direction for rows in the table. Click the appropriate direction to display the text from the bottom up or the top down.

Default Units Formatting tab

Formats table data, except for columns specified individually on the Default Column Settings tab.

Column Width	Specifies the default column width for columns. Columns may be resized in individual tables.
Leading/Trailing Zeroes	Sets the formatting for leading and trailing zeroes.
Justification	For the Heading row and Data rows, specifies left, center, or right justification.
Use Default Formatting	Uses the default settings specified in the standard.
Apply Units Formatting	Enables a custom formatting and units setting for table columns.
	Unit Type selects the type of measurement units.
	Format selects a fractional or decimal format. Fractional formats are available only if Length is selected as Unit Type and inches or feet are selected as Units.
	Precision selects the precision of values displayed in the selected column.
	Fractional Text Scale sets the text scale for numbers in stacked fractions. Available only if a fractional format is selected.
	Units selects the measurement units. If inches or feet are selected, fractional format is available in the Format option.
	Decimal Marker selects the marker for the decimal format. Click the arrow to specify either a period or comma as the decimal character.
	Unit String displays the name of the units next to the value.

Unit type	Format	Precision	Units	Decimal marker	Display unit type
Length	Decimal, fractional	0-8	mm, cm, m, in, ft, micron, mi, yard	period or comma	yes.
Angularity	Decimal Degrees, Deg-Min-Sec	0-8	not available	period or comma	no
Volume	Decimal	0-8	Liter, Gallon	period or comma	yes
Mass	Decimal	0-8	gram, lbmass, slug, kg, ouncemass	period or comma	yes
Comments	Enter information about the definition of a particular style, such as date created, created by, or derived from a particular standard.

Default Column Settings tab

Creates column templates by specifying alternate and more detailed formatting for individual columns, independent of other columns. Columns added from this tab and formats applied to existing columns have precedence over settings from the Default Units Formatting tab.

If the table has more columns than were individually formatted, the remaining columns use settings on the Default Units tab.

If no columns are formatted individually, all columns are formatted by settings on the Default Units Formatting tab.

Add Column

Adds a column to the table, starting with Column 1. The initial width and other column formatting is initially set from the Default Units Formatting tab, but may be changed.

Additional columns are added to the end of the list and are named incrementally, such as Column 1, Column 2, and so on.

Once a column is added, you can change column name, source, and column width:

Name from Source check box is selected by default and names the column from the source data. Clear the check box to enter a column name.
Column can be edited when the Name from Source check box is cleared. Enter a column name.
Width is set by default to 1.000. Enter a new width for each column if desired.

Remove Column

Removes selected column from the table.

To format columns, click in a column name cell to open the Format Column dialog box. For more information, see the Column Format reference.

Format Column - Tables

Sets the formatting and alignment properties for a column in the table.

Access:

To define columns in a Table style: Click Manage tabStyles and Standards panel Styles Editor. In the Style and Standard Editor dialog box, click Table. On the Default Column Settings tab, right-click a column name cell to open the Format Column dialog box.

To edit a table column: Right-click a table and select Edit. In the Edit Table dialog box, click the Format Column command.

Property	Displays the name of the property displayed in the selected column.
Heading	Sets the name of the selected column. To change, enter a different name.
Column Width	Specifies the width of the column.
Leading/Trailing Zeros	Controls the display of leading and trailing zeros.
Justification	Sets the alignment for the column heading and respective cells.
	Heading Sets the alignment for the column heading. Click a button to select left, center, or right alignment.
	Value Sets the alignment for the data in the column. Click a button to select left, center, or right alignment.
Stacked Fractional Text	Enables stacking of numeric fractions. All fractional numerical strings (in 1/2 format) in the selected column are replaced with a stacked numeric fraction in the drawing. Available only when editing a parts list in the drawing and Use Default Formatting is selected.
Stack Properties	Opens the Stack Properties dialog box and sets the format and text scale for stacked fractions. Available only when editing a parts list in the drawing and Use Default Formatting is selected.
Use Default Formatting	Uses the default settings specified in the standard.
Apply Units Formatting	Enables the formatting and units settings for the selected column. Changes made to these settings only apply to the selected column.
	Unit Type selects the type of measurement units.
	Format selects a fractional or decimal format. Fractional formats are available only if Length is selected as Unit Type and inches or feet are selected as Units.
	Precision selects the precision of values displayed in the selected column.
	Fractional Text Scale selects the text scale of numbers in stacked fractions. Available only if a fractional format is selected.
	Units selects the measurement units. If inches or feet are selected, fractional format is available in the Format option.
	Decimal Marker selects the marker for the decimal format. Click the arrow to specify either a period or comma as the decimal character.
	Unit String displays the name of the units next to the value.

Style and Standard Editor - Text Styles

Sets the formatting attributes for text styles.

Other styles can reference the text style as a substyle to set formatting. For example, the dimension style uses the text style to format dimension text and the parts list style uses the text style for parts lists text.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Text. If available, click one of the listed styles to view or edit.

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles, Styles in the Active Standard, or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

The Paragraph Settings box sets spacing, value, stretch, and color. When overridden using the Format Text dialog box, these settings apply to the entire text object only, and cannot be changed for individual lines or characters.
Spacing	Specifies the spacing between the bottom of one line of text and the bottom of the next line of text. Click the arrow to select.
Value	When line spacing is set to Exact or Multiple, specifies the value for line spacing.
% Stretch	Specifies the text width. Enter 100 to display the text as designed, enter 50 to decrease the width of the text by 50%.
Color	Specifies the text color. Click the color button, and then select a color from the Color dialog box. Text color can be set to By Layer.
Justifications	Click Left, Center, or Right Justification, or Top, Middle, or Bottom Justification to apply the justification to the text style.
Rotation	Rotates the text. Select a button to specify the angle of rotation for the text.

In Character Formatting, set font, text size, and emphasis. Attributes can be overridden on individual characters in the text of the object.
Font	Specifies the font for the text style. Click the arrow and select from the list.
Text Height	Sets the height of the text in sheet units (inches or millimeters). Enter the size or click the arrow and select a size from the list.
Emphasis	Click Bold, Italic, or Underline to apply the style to the text.
Italicize Symbols	Click Italic to enable this check box. Uncheck the box to exclude symbols for dimensions and hole/thread notes to be displayed in italic font.

In the Comments box, enter a comment about the definition of a particular style, such as date created, created by, or derived from a particular standard.

Style and Standard Editor - View Annotation Style

Use the View Annotation Style panel to set up defaults for view annotations.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, expand the View Annotations item and select a view annotation style.

View type	Select the type of drawing view and then set the options. Available options depend on the selected view type.
		Selects section views.
		Selects auxiliary views.
		Selects detail views.
Format	Sets format for annotations in the base view when creating section, auxiliary, or detail views.
	Select an annotation format. Available formats are illustrated by images.
	Show Entire Line displays the section line in the base view. Available for section views only.
	Select Definition in Base View (Default - Removed View) to display the auxiliary view definition in the base view when the alignment of the auxiliary view is broken. Select Definition in Base View (Default - Auxiliary View) to display the auxiliary view definition in the base view. Available for auxiliary views only.
Leader Format	Available for detail views only. Line Type selects the line type for the leader line. Draw Terminator draws the arrowhead (terminator) on the detail view annotation leader. Text Orientation sets the orientation and alignment of detail view identifier text on a leader.

Terminator	Extension Line Length sets the length of the leader line for the selected view type. Not available for detail views.
	Terminator selects the default arrowhead (terminator) for the selected view type.
	Size (X) specifies the length of the open or closed arrowheads for the selected view type.
	Height (Y) specifies the height of open or closed arrowheads for the selected view type.
Text Style	Selects an existing text style to use for the annotation text.
	Click the pencil to edit the selected text style. When you save the style, the changes are in effect wherever the style is used
Comments	Enter information about the style, such as date created, created by, or derived from a particular standard.

Style and Standard Editor - Weld Symbol Style

Defines welding symbols available for use in the drawing or template.

The Weld Symbol style is a substyle of the active standard style.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Weld Symbol. If available, click one of the listed styles to view or edit.

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles, Styles in the Active Standard, or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

Set weld symbol attributes in the Weld Style window.

Substyles

Specifies styles required to define a weld symbol. The attributes of the leader, alternate leader, and text styles are defined in their own style; balloons reference those attributes for formatting those objects.
	Some substyles can be edited while defining the parent style. Click the pencil to edit the selected style. When you save the style, the changes are in effect wherever the style is used.
Leader Style	Click the arrow to list leader styles in the active standard. Click the pencil icon to open the leader style for editing.
Text Style	Click the arrow to list text styles in the active standard. Weld symbol text is formatted with this style.

Identification Line

Sets the format for displaying a welding symbol identification line.
Identification Line Default	Click to select the default placement. Select no identification line, identification line above, or identification line below the reference line. May be changed for individual welding symbols. Available for ISO and DIN only.
Offset	Controls the distance between the line and the welding symbol. The resulting offset is calculated using this value and the text height.
Line Type	Sets the line style, such as dashed, dotted, or continuous. Click the arrow to select the line type from the list.

Arrow Side Position

Determines if the weld symbol is on the top or bottom of the reference line.

Symbol Size

Specifies the size of the weld symbol.
Link to Text Height	Select the check box to size the symbol the same as the text height defined in the active standard.
Scale Factor	Clear the Link to Text Height check box to enter a scale factor relative to its default size. Scale factor must be between 0.5 and 2.00.

Symbol Filter

Lists all defined welding, contour, and backing symbols, regardless of active standard. Selecting a symbol or canceling the selection includes or removes it to the selection set in the Welding Symbol dialog box. Symbol list originates in the Welding Symbol dialog box. Click a symbol type to show all defined symbols of that type. Click the check box to include the symbol in the Welding Symbol dialog box selection set or clear the check box to remove it from the list. Click the plus sign to see variations of a symbol and then click the desired variation.
Welding symbols	List originates on the Arrow Side of the Welding Symbol dialog box.
Contour symbols	List originates on the Other Side of the Welding Symbol dialog box.
Backing symbols	List originates on the Other Side of the Welding Symbol dialog box.

Comments

Enter information about the definition of a particular style, such as date created, created by, or derived from a particular standard.

Style and Standard Editor - Weld Bead Style

The Weld Bead Style specifies the attributes for weld annotation objects in drawings, including caterpillars, end fills, and annotations recovered from a weldment model.

The Weld Bead Style is a substyle of the active standard style.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Weld Bead, and then click Weld Bead Recovery. If available, click one of the listed styles to view or edit.

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles, Styles in the Active Standard, or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

In the Weld Bead Style window, specify the attributes for weld bead recover.

Caterpillar

Sets the defaults for weld caterpillar annotations in the drawing.
Type	Selects the default caterpillar type: Centered or Edge caterpillar. Set the defaults for both types.
Stitch Options	Sets the size for creating intermittent caterpillars. Length sets the default length of one segment in an intermittent caterpillar. Offset sets the default distance between the centers of two adjacent segments of an intermittent caterpillar.
Seam Visibility	Select the check box to set the default for the visibility of the edge on which a weld caterpillar is placed. Clear the check box to hide the edge after placing the caterpillar.
Width	Sets the default width of caterpillar legs. For a partial caterpillar, width is the distance between the endpoint of the leg and the selected edge. For a full caterpillar, width is the distance between the endpoints of the legs.
Angle	Sets the default angle for an imaginary line between the selected edge and the endpoints of the caterpillar legs. The units (deg, rad, grad) are displayed.
Spacing	Sets the default distance between legs in the caterpillar. The units (in, mm, cm, and so on) are displayed.
Arc %	Sets the default radius of the arc relative to the length of the arc chord. The value must be greater than 0° and less than 100°.
Line Weight	Sets the default thickness of the lines in the caterpillar. All line weights defined in the active standard are available. Click the arrow to select a value. If a specific value is not selected, the default By Layer is used, where the line weight is defined by the layer on which the object resides.

End Fills

Sets the defaults for weld end fill annotations in the drawing.
Leg 1/ Leg 2	Sets the default height and width for end fills. Type the value for each leg into the corresponding box. Units are displayed (in, mm, cm, and so on).
Throat Depth	Sets the default throat depth for fillets.
Bevel defined by Throat Depth	If selected, the fillet size is defined by throat depth by default.
Scale	Sets the default scale for the selected hatch pattern. Click the arrow, and then select the scale. Not available if Solid Fill is checked.
Hatch	Selects a default hatch pattern for the fill. Click the arrow, and then select from the available hatches. Not available if Solid Fill is checked.
Color	Selects the default display color for the hatch or solid fill. Click the color button, and then select the color. If no color is selected, By Layer is the default, where the color is defined by the layer on which the object resides.
Solid Fill	Sets solid fill as the default the end fill. Select Solid Fill to fill the end fill. Clear the check mark to use the selected hatch pattern as the default fill for end fills.

Comments

Enter information about the definition of a particular style, such as date created, created by, or derived from a particular standard.

Units

Sets the units for datum target style and feature control frame style.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor, click to expand Datum Target or Feature Control Frame, and then double-click to show the style in the window. Click the Units tab.

Primary Units

Changes the format of the primary units of measure for values in datum target symbols or feature control frames.
Linear	Sets the units of measurement. Click the arrow, and then select from the list. The default is Use Common.
Decimal	For a linear unit other than Use Common, specifies the character to use as a decimal. Click the arrow, and then select from the list.
Unit String	Displays the primary unit type after the value in datum target annotations. Select the box to display the unit type. Clear the check mark to hide the unit type.
Leading Zeros	Shows or suppresses the display of leading zeros in datum target values. Select the box to display leading zeros. Clear the check mark to suppress them.
Trailing zeros	Shows or suppresses the display of trailing zeros in datum target values. Select the box to display trailing zeros, Clear the check mark to suppress them.
Alternate Units	Displays or hides alternate units in datum target symbols. Select the box to display alternate units. Clear the check mark to hide them.
Display Style	Sets the display style for alternate units in datum target symbols. Click the arrow, and then select from the list.

Alternate Units

Changes the format of the secondary units of measure for values in datum target symbols and feature control frames. Not available unless Display Alternate Units is selected in the Primary Units box.
Linear	Sets the units of measurement. Click the arrow and select from the list.
Decimal	Specifies the character to use as a decimal. Click the arrow and select from the list.
Unit String	Displays the alternate unit type after the value in datum target annotations. Select the box to display the unit type. Clear the check mark to hide the unit type.
Leading Zeros	Shows or suppresses the display of leading zeros in datum target values. Select the box to display trailing zeros. Clear the check mark to suppress them.
Trailing zeros	Shows or suppresses the display of trailing zeros in datum target values. Select the box to display trailing zeros. Clear the check mark to suppress them.
Precision	Sets the decimal precision for display of alternate units in datum target annotations. Click the arrow, and then select from the list.

Select Hatch Pattern

Use the Select Hatch Pattern dialog box to select hatch patterns to be available in the drawing.

Access:

Ribbon: Manage tab Styles and Standards panel Styles Editor. In the Style and Standard Editor, click to expand Hatch, and then double-click a hatch style from the list to show the style attributes in the window. From the Pattern list select Other.
On the Hatch/Color Fill dialog box, select Other in the Pattern list.
On the Edit Hatch Pattern dialog box, select Other in the Pattern list.

Loaded Hatch Patterns

Displays a list of hatch patterns loaded in the drawing.

TipBefore you close the Select Hatch Pattern dialog box, select a hatch pattern to set it in the Pattern list of the superior dialog box.

Offered selects hatch patterns to be available in the Pattern list on hatch-related dialog boxes.

TipUse the Offered property to filter out hatch patterns that are not any more needed in the drawing.

Hatch Pattern displays the name of the hatch pattern.

Description displays the description of the hatch pattern.

Load

Loads additional hatch patterns to the drawing.

Opens the Select Hatch Pattern File or Load Hatch Pattern dialog box. You locate a PAT file and select hatch patterns to load.

Export

Displays the Select Hatch Pattern File dialog box. You specify the location and file name for the exported PAT file. All hatch patterns selected in the Loaded Hatch Patterns list are exported to the specified file.

Load Hatch Patterns

Use the Load Hatch Pattern dialog box to locate a PAT file and select hatch patterns to load in the drawing.

Access:

In the Select Hatch Pattern dialog box, click Load.

Hatch Pattern Definition File

Specifies the PAT file with patterns to load.

Select a PAT file from the list or click Browse to locate a PAT file.

Available Hatch Patterns

Displays hatch patterns available in the specified PAT file.

Select hatch patterns to load, and then click OK to close the dialog box.

Select Line Type (LIN file)

Loaded Line Types	Displays list of line types and their attributes loaded in the current drawing.
Load	Displays the Load Line Types dialog box, in which you can load selected line types (LIN file) into the drawing and add them to the list of line types.

Load Line Type (LIN file)

Line Type Definition File	Displays the location of the .lin file. Click Browse to locate and load a .lin file.
Available Line Types	Displays the available line types associated with the selected line type. Select the line type to add or SHIFT-select to load multiple line types, and then click OK.

Dimension styles in drawings

A dimension style is a named group of dimension settings. When you apply a style to an object, the setting determines the format of that object.

The Dimension style uses the Text style as a substyle to format dimension text. You can specify individual text attributes (bold, underline, and so on) when you create or modify a dimension style. Changes to dimension text style update the Text style.

You can also specify a text style for the tolerance portion of the dimension on the Text page. If no specific text style is specified for the tolerance, the text style is used.

Dual dimension units in drawing annotations

You can display the dimension values in both primary and alternate units in the following types of drawing annotations:

Dimensions
Hole Notes
Chamfer Notes

The dual units display is set on the Alternate Units tab of the dimension style for dimensions and all note types.

NoteIf a dual unit format is selected, precision and tolerance values also display in the dual format.

TipDual dimension values can be displayed also in hole tables. Add the Alternate Units column to the table by using the Column Chooser dialog box.

Overriding dimension styles

You can modify individual dimensions for special annotation purposes.

To override dimension style settings, right-click a dimension, and then choose Options, Precision, Tolerance, or Text. Overrides always supersede the equivalent setting in the dimension style.

NoteIf you apply a dimension style to a dimension, any overrides on that dimension are removed.

Reusing customized dimension styles

When you customize the dimension style in a drawing, the changes are saved in that drawing. To make customized styles available in all new drawing files, save the changes in the style library. The style is available to all documents that use the style library.

You may not be able to save changes to the style library if it is locked to prevent unauthorized changes.

Procedures

Set dimension styles

The dimension styles control the drawing dimension format. The active standard provides a set of default styles, among them dimensions. You can add or edit dimension styles to control measurement units, precision, line and arrowhead styles, text styles, tolerance format, and many other attributes of dimensions. Changes to the default styles associated with the active standard affect only the current document.

NoteMany legacy documents have styles defined in the template used to create a drawing. You can continue to use those styles. If there are styles you do not intend to use, use Manage tab

Styles and Standards panel

Purge to deleted unused styles.

Apply a dimension style

When you place a dimension in a drawing, it assumes the formatting of the default dimension style. You can apply a different dimension style to individual dimensions.

On the Annotate tab, Format panel, click the arrow on the Style box, and then select a dimension style to make it active. All dimensions use the formatting of the selected dimension.

To change dimension styles, click the Style box, and then select a different dimension style.

Create a dimension style

Autodesk Inventor LT provides several dimension styles for each drafting standard. You can use the preset styles to create your own styles.

Select Manage tab Styles and Standards panel Styles Editor to open the Style and Standard Editor.
In the editor browser, click Dimension to show the available styles.
Right-click a style name, and then choose New Style. Enter a style name.
In the Dimension Style window, the values of the existing style are shown. Select each tab and set the attributes for the new style.
Click Save to save the new style, and then click Done to close the dialog box.

The new style is available only in the current document, unless you right-click the new style name in the editor browser, and then select Save to Style Library. You may not be able to save changes to the style library if it is locked to prevent unauthorized changes.

Create new dimension style from selected dimensions

You can use the formatting of existing dimensions to create a dimension style.

Select one or more dimensions in a drawing. If the dimensions have different formatting, the first dimension selected is used to create the style.
Right-click, and then select New Dimension Style from the menu.
Click OK to save the new style. It is cached in memory.
Click Manage tab Styles and Standards panel Styles Editor. Click to expand the Dimension style. Notice that the new standard is listed. The default name is same as the active dimension style incremented by a number. Right-click, and then select Rename Cached Style. Enter a style name and click OK.
Click Save to saved edits to the style name.

Modify an existing dimension style

You can modify existing dimension styles or the dimension styles that you create. The modified styles are saved in the current document.

Click Manage tab Styles and Standards panel Styles Editor to open the Style and Standard Editor.
Select the style to modify.
Select the appropriate tab and change the attributes for the style.
Click Save to save the new style, and then click Done to close the dialog box.

Display primary and alternate units in drawings

Drawing dimensions and notes display values in the primary measurement units specified in the dimension style or in the part file. If appropriate, set dimensions and notes to display dimension values also in alternate units.

Dimensions and notes can display values both in primary and in alternate measurement units. You select the display options to control the appearance of dual dimensions.

Display or hide alternate units

Open a drawing.
Click Manage tab Styles and Standards panel Styles Editor.
Expand the Dimension styles list and click the dimension style to edit.
On Alternate Units tab, specify the setting for alternate units: Specify the measurement units, dimension formatting, and display. Then select each type of annotation (Dimensions, Hole Notes, Chamfer Notes, Bend Notes, and Punch Notes) and specify the appearance of the dual format.
TipTo hide the alternate units for the selected type of annotation, select the Primary Units Only option.
Click Save to save the change, and Done to close the dialog box.

NoteIf a dual unit format is selected, precision and tolerance values are also displayed in the dual format.

Use part units or primary units from the style

Open a drawing.
Click Manage tab Styles and Standards panel Styles Editor.
Expand the Dimension styles list and click the dimension style to edit.
On Notes and Leaders tab, select Hole Note, Bend Note, or Punch Note Setting.
NoteThe change applies only to the selected type of drawing annotation.
Select Part Units to display values in units specified in the part file. Clear the Parts Units check box to use units specified on the Units tab of the dimension style.
Click Save to save the change, and Done to close the dialog box.

NoteThe Part Units option overrides the setting for primary units on the Units tab. Secondary units always respect the unit setting on the Alternate Units tab.

View tap drill diameters

To see the tapped drill diameter display in a drawing, add the Tap Drill value to the Edit Window in the Styles Editor dialog box.

Note: A thread type must be specified.

Click Manage tab Styles and Standards panel Styles Editor.
Activate the dimension you want to use.
Click Notes and Leaders tab.
Click the Thread Type down-arrow, and select a type from the list.
In Options list, cancel the selection of Use Default.
Click Tap Drill Diameter Value to add tap drill syntax to the Edit Window.
Click Done and save the changes.
NoteFollow these steps for every Thread type and Hole type you want to display the tapped drill diameter.

References

Style and Standard Editor - Dimension Style

Sets the format of dimension styles used in drawings.

The dimension style is a substyle of the standard, but format may be defined regardless of the active standard style. The dimension style references text and leader styles as substyles for formatting.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Dimension in the browser. Click one of the listed styles to view or edit. You can also expand Dimension in the browser, and then click one of the styles.

For the current document, you can click:

Back to return to the previously edited style. You are prompted to save the previous edits.
New to create new styles. Select the Add to Standard check box to add to the available styles list in the active standard style.
Save to save changes to an existing style in the current document.
Reset to return style values to the saved values.
Filter to show Local Styles, Styles in the Active Standard, or All Styles in the browser.
Import to use the Import Style Definition dialog box to import a style exported from another document.

On the Manage tab, Styles and Standards panel, you can also use these commands:

Click Update to refresh the style list in the browser pane to include new or changed styles in the library.
Click Save to save changed styles to the style library, which replaces the style library version with the new values.
Click Purge to delete unused styles from the document.

In the Dimension Style window, click a tab to show attributes.

Units

The Units tab sets dimension attributes for units, linear and angular format and precision, and display preferences.

The Units box sets the units of measurement for the dimension style.
Linear	Click the arrow to set linear units.
Decimal Marker	Click the arrow to specify either a period or comma as the decimal character.

The Linear and Display boxes specify dimension format, precision, and display preferences.
Format	Sets fractional or decimal format for all primary linear dimensions. Click the arrow and select from the list.
Precision	Sets the precision for primary linear dimensions.
Unit String	Select the check box to show primary units in drawing dimensions.
Included Zeros	Select the check box to display a zero before fractional inch values less than one. For example, 1’ - 0 1/2”.
Leading/Trailing Zeros	Select the check box to show leading and trailing zeroes for primary linear dimensions according to the precision setting.

The Angular and Angular Display boxes specify dimension format, precision, and display preferences.
Format	Sets format for all angular dimensions to either decimal degrees or degrees, arc minutes, or arc seconds. Click the arrow and select from the list.
Precision	Sets the precision for angular dimensions. Click the arrow and select the number of decimal places to display.
Leading/Trailing Zeros	Select the check box to show leading and trailing zeroes according to the precision setting.

In Comments, enter information about the definition of a particular style, such as date created, created by, or derived from a particular standard.

Alternate Units

The Alternate Units tab sets the alternate unit attributes for the dimension style.

The Alternate Units box sets the alternate units of measurement for the dimension style.
Linear	Click the arrow to set linear units.
Decimal Marker	Click the arrow to specify either a period or comma as the decimal character.

The Linear box specifies the dimension formatting.
Format	Sets fractional or decimal format for all non-angular dimensions. Click the arrow and select from the list.
Precision	Sets the precision for linear dimensions. Click the arrow and select the number of decimal places to display.
Fractional Text Scale	Sets the scale of numbers in a fractional format.

The Display box specifies the display preferences.
Unit String	Select the check box to show units in drawing dimensions.
Included Zeros	Select the check box to display a zero before fractional inch values less than one. For example, 1’ - 0 1/2”.
Leading/Trailing Zeros	Select the check box to show leading and trailing zeroes according to the precision setting.

The Dual Format box specifies the display format for dual dimensions.
	Selects an annotation type to change its dual format.
	Selects the format to display the primary and alternate dimensions. TipSelect the last option on the image to display only primary units.

Display

The Display tab sets attributes for extensions, terminators, dimension line visibility, break line symbol, and positioning.

The Line box sets the line type, line weight, and color.
Type	Sets the line type for the selected dimension style. Click the arrow and select a specific line type or select By Layer to use the value specified by the layer style.
Weight	Sets the line weight for the dimension style. Specify a line weight by selecting from the list, entering a value, or selecting By Layer to use the layer line weight value.
Color	Sets the line color for the selected dimension style. Click the color box and select a color from the palette or select By Layer to use the layer color value.

The Terminator box sets the arrowhead type and size for the dimension style dimension lines. It does not set the arrowhead type for leader text or for hole notes. Arrowhead type for leader text or hole notes is set by the leader substyle on the Holes/Leaders tab.

Terminator

Click the arrow to select the preferred terminator.

Size (X) and Height (Y)

Sets the size of the terminator.

Size (X) specifies the length of the open or closed arrowheads, datum terminators, or the diameter of circular terminators.
Height (Y) specifies the height of open or closed arrowheads.

The Display settings control preferences for the appearance of dimensions. Letters on the image indicate the display attribute.
Dimension Line Visibility	Sets the dimension line visibility when arrowheads are outside the dimension extension lines. Click the arrow to turn dimension lines visibility On or Off whenever the dimension arrowheads are outside the extension lines.
Break Symbol	Click the arrow to turn break symbol visibility On or Off for dimensions used on broken views.
Extension (A)	Sets the distance the extension line is drawn past the dimension line.
Origin Offset (B)	Sets the distance from an edge or point to the endpoint of the extension line that is displayed as you place a dimension.
Gap (C)	Sets the gap distance between the dimension text and the dimension lines.
Spacing (D)	Sets the distance between the parallel dimension lines displayed as you place dimensions.
Part Offset (E)	Sets the distance from the referenced part edge to a parallel dimension line. This option is only used when edges are parallel to the dimension lines.

Text

The Text tab specifies a text style, text and angle dimension orientation, tolerance text height, and a prefix and suffix.
	Click the pencil next to the substyle list to edit the selected style. When you save the style, the changes are in effect wherever the style is used. If you changed the referencing style, save changes before you can edit the substyle.

The Primary Text Style selects an existing text style to use for the dimension text. The text is a substyle that uses font, justification, and color defined in the text style. Click the arrow to select a style.

The Tolerance Text Style selects the text style for tolerances. The default is the same as the primary text style.
	Justification sets the vertical justification of the dimension tolerances with respect to the dimension value text. Click an image to specify Top, Middle, or Bottom justification for tolerances relative to the dimension value.
	Size sets the size of the tolerance value text independently of the text style. Click the arrow to select a predefined size or enter a new size in the box for tolerance text.

Orientation specifies how the dimension text is positioned relative to the geometry. Click an arrow to make the selection. The Tool Tip identifies the orientation type.
Linear	Specifies text alignment for linear dimensions.
	Horizontal specifies parallel to the dimension line or inline.
	Aligned specifies inline horizontal, inline aligned or parallel.
	Vertical specifies inline horizontal, inline vertical, parallel, or parallel-horizontal.
	Text position relative to the landing line may be All Above Landing Line or First Above Landing Line.
Diameter	Specifies text alignment for diameter dimensions.
	Internal Dimension specifies inline horizontal, inline aligned, or parallel placement of the text.
	External dimension text may be Horizontal or Aligned.
	Text position relative to the landing line may be First Line Centered, All Above Landing Line, First Above Landing Line, JIS Alignment/Format, or All Above Landing Underlined.
Radial	Specifies text alignment for radial dimensions.
	Dimension text may be Horizontal or Aligned.
	Text position relative to the landing line may be First Line Centered, All Above Landing Line, First Above Landing Line, JIS Alignment/Format, or All Above Landing Underlined.

The Angle Dimensions box specifies the angle dimension orientation and the modifier. The preview image updates with your selection.
	Orientation sets inline horizontal, inline aligned, parallel - aligned or parallel - horizontal.
	Modifier sets no modifier, above for horizontal, outside dimension line, or outside for angles between 30° and 210°.

The Prefix/Suffix box specifies text and the appropriate symbol.
	Prefix and Suffix specifies the appropriate text.
	Symbol selects a defined symbol from the list. The selected symbol is inserted into the last selected Prefix or Suffix text box.
	Prefix/Suffix order orients the prefix and suffix text relative to the primary or alternate unit text. Select the above/below or inline.

Tolerance

The Tolerance tab sets tolerance format for the dimension style.

The Method box specifies the tolerance method. Click the arrow to make a selection.
Upper	Sets the value for the upper tolerance. Enter a sign of operation before the value.
Lower	Sets the value for the lower tolerance. Enter a sign of operation before the value.

The Display Options box specifies how to display or suppress leading and trailing zeros and the method for displaying basic dimensions.
	Zero tolerance is used when a linear tolerance value is true zero. Selects how zero values are displayed in tolerances. Choose Full Display, No Trailing Zeros, No Trailing Zeros - No Sign, or Suppress Display
	Zero arc minutes/seconds is used when the arc minutes or arc seconds are true zero for primary units and tolerance units. Choose to show zero values for arc minutes and arc seconds for arcs or hide zero values for arc minutes and arc seconds.
	Basic dimension display shows prefix/suffix inside or prefix/suffix outside the Basic dimension bounding box.

The Primary Units box specifies precision, and display preferences for primary unit tolerances.
Linear Precision	Sets the precision for linear dimension tolerances. Click the arrow and select the number of decimal places to display.
Angular Precision	Sets the precision for angular dimension tolerances. Click the arrow and select the number of decimal places to display.
Included Zeros	Select the check box to display a zero before fractional inch values less than one. For example, 1’ - 0 1/2”.
Leading/Trailing Zeros	Select the check box to show leading and trailing zeroes on tolerance values according to the precision setting.

The Alternate Units box specifies precision, and display preferences for alternate unit tolerances.
Precision	Sets the precision for alternate unit tolerance. Click the arrow and select the number of decimal places to display.
Leading/Trailing zero	Select the check box to show leading and trailing zeroes in alternate unit tolerances according to the precision setting.

Options

The Options tab sets preferences for arrowhead placement, extension line visibility, radius, horizontal, and angular dimensions, and leaders and origins of ordinate dimensions.

Arrowhead Placement	When creating dimensions, specifies inside or outside placement for linear, angular, diameter, and radial dimensions.
Hide Extension Lines	Select the check boxes to specify to hide linear or angular extension lines.
Radius Dimensions	Select a check box to specify no leader or leader from center and no jogged leader or a jogged leader.
Diameter Dimensions	Shows or hides the diameter symbol when a diametric dimension is placed on a geometric circle. Specifies no leader or a leader from the center of a circle. Specifies a single or dual dimension line.
Angular Dimensions	Specifies whether to use a quadrant or ignore a quadrant when placing text for angular dimensions. For a quadrant, the angular dimension changes to match the destination quadrant. The angular extension lines change to show which quadrant the angle is measuring. When not using the quadrant, the angular dimension text remains constant, matching the original angle when it was placed.
Ordinate Dimension Leaders	Jogging specifies broken or straight leaders. Alignment Select the check box to use continuous running leaders. Clear the check box to select aligned leaders or non-aligned leaders.
Ordinate Dimension Origins	Displays or hides the direction arrow. Displays positive dimensions in both directions. Select the origin indicator check box to use the origin indicator. Select the Hide Origin Indicator check box to hide the origin symbol or clear the check box to display it. Origin Selects an origin mark for the Countinous Running ordinate dimension sets. NoteWhen you change the origin mark in the style, all existing By Style origin marks in the drawing respect the new setting.

Notes and Leaders

The Notes and Leaders tab formats hole and thread notes, revision tags, hole tags, leader text objects, and chamfer notes.

Unless indicated otherwise, all values are linked to the note. Changes to the values affect notes associated with the modified style.

Selects the note type to edit its settings. Available options depend on the selected note type.

Hole type

Selects the hole type. Click the arrow, and then select the hole type from the list. Available for hole note only.

NoteSet the attributes for each hole type that are in the drawing.

Edit window

Sets up the content of the notes. In Values and Symbols, click a value or symbol to add the corresponding property to the note text. Click the arrow next to the Insert Symbol command to select and insert a symbol.

You can use a combination of text, inserted symbols, and variables to configure the annotation text of the note. For example:

C <DIST1> X <DIST2> would result in C 10 X 10

Options

Use Default sets hole note formatting to the default. Check the box to use defaults. Remove the check mark to change the formatting. Not available for chamfer notes.

Tap Drill indicates that the current format selected (from the combination of Hole type and Thread type) is used when the Tap Drill option is turned on for edited hole notes. Select a hole note, right-click, and select Edit Hole Note. Then select the Tap Drill option on the Hole Note edit dialog box. Not available for chamfer notes.

Part Units sets the note to use the measurement units of the model. Check the box to use model units. Remove the check mark to use the measurement units specified by the dimension style. Not available for chamfer notes.

Precision/Tolerance Settings opens the Precision and Tolerance dialog box so you can add tolerance information to values included in notes.

Apply to All applies all selected settings in the Options box to all hole and thread types, including all settings in the Precision and Tolerance dialog box. Not available for chamfer notes.

Values and Symbols
	Hole notes: Adds values and symbols to hole notes. Click a value or symbol to add it to the hole note. To remove, place the cursor after the value or symbol in the Edit Window and backspace.
		Selects a symbol from the list to adds it to the hole note.
	Icon	Formula	Name	Origin / Column in Threads.xls
		<HDIA>	Hole Diameter Value	Size
		<HDPT>	Hole Depth Value	Model
		<CBDIA>	Counterbore/Spotface Value	Model
		<CBDPT>	Counterbore/Spotface Depth Value	Model
		<CSDIA>	Countersink Diameter Value	Model
		<CSANG>	Countersink Angle Value	Model
		<CSDPT>	Countersink Depth Value	Model
		<QTYNOTE>	Quantity Note adds text to indicate quantity. Not displayed if the hole note is used inside a hole table or if the quantity is less than two.	Format defined by
		<THRP>	Thread Designation Value	Thread Designation
		<THDCD>	Custom Designation Value	Custom Thread Designation
		<THDPT>	Thread Pitch Value	Pitch Dia
		<THRC>	Thread Class Value	Class
		<THRD>	Thread Depth Value	Model
		<TDDIA>	Tap Drill Diameter Value	Tap Drill
		<FST>	Fastener Type Value	Model (Clearance holes only)
		<FSZ>	Fastener Size Value	Model (Clearance holes only)
		<FIT>	Fastener Fit Value	Model (Clearance holes only)

	Chamfer notes: Adds values and symbols to chamfer notes.
		Inserts the Distance1 variable (<DIST1>) in the text window.
		Inserts the Distance2 variable (<DIST2>) in the text window.
		Inserts the Angle variable (<ANGL>) in the text window. The calculated angle is always the acute angle between the selected chamfer edge and the reference edge (less than 90 degrees).
		Selects a symbol from the list to add to the chamfer note.

General settings

Unlike other options, general settings are a single setting for each hole note or leader object.

Edit Quantity Note opens the Quantity Note dialog box. Allows custom configuration of the quantity note display in the context of a hole note (represented by the Quantity Note symbol).

Leader style sets a specific leader for hole notes and leader text.

Edit opens the Leader Style so that attributes can be modified. For more information about the leader style, see Style and Standard Editor - Leader Style.

Justify text to leader overrides the text style justification settings and automatically justify toward the leader. Clear the check box to retain the text style.

Leader orientation specifies whether leader text is aligned to the leader or horizontal to the line. Click the arrow to select horizontal or aligned.

Leader text alignment controls how text displays relative to the leader landing line and sets underlining for multi-line text. Click arrow to select first line centered, all above landing line, first above landing line, JIS alignment/format, vertical extension, or all above landing underlined.

Thread Note Settings

Select the Custom Designation check box to apply the custom thread designation field from the Thread.xls spreadsheet instead of the default note (thread designation and class).

Quantity Note

Creates text to describe quantity in hole notes. Quantity note is not displayed if the hole note is used in the context of a hole table or if the quantity is less than two.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor

. In the Style and Standard Editor dialog box, click Dimension style. Click one of the listed styles and then click the Notes/Leader tab. Click Edit Quantity Note.

If desired, right-click a hole note and select Edit Hole Note or double-click a hole note. In the Edit Hole Note dialog box, click Edit Quantity Note.

Text box	Contents are inserted into a hole note where the <QTYNOTE> variable is positioned. Text is one line only.
Quantity Value	Inserts the <QTY> variable to represent the quantity of holes identified by the hole note.
Symbols List	Click the arrow to insert a symbol selected from the list.
Number of holes	Specifies the value of the <QTY> variable. Number of holes in pattern/feature shows the number of holes in the pattern or feature. Number of like holes in view (normal) shows the number of similar holes normal to a specific view. Holes are "like" if they are the same hole type (blind counterbore are not like through counterbore), hole parameters are equal, and the hole axis is normal to the view.

Precision and Tolerance

Sets the precision and tolerance attributes for hole or chamfer notes.

Access:

Ribbon: Manage tab

Styles and Standards panel

Styles Editor. In the Style and Standard Editor, click to expand the Dimension style in the browser. In the Dimension Style window, click the Notes and Leaders tab, and then click Precision and Tolerance. Click More to expand the dialog box.

To override precision and tolerance parameters for an existing hole or chamfer note, right-click the note and then select Edit Hole Note or Edit Chamfer Note. In the dialog box, click Precision/Tolerance Settings. Click More to expand the dialog box.

Options depend on which note type is selected on the Units tab of the Dimension style dialog box.

Hole notes

Use Global Precision	Sets parameter precision to the precision defined by the Precision setting on the Units tab of the active dimension style. When selected, individual parameters in the Precision column are not available. Clear the check box to edit individual precision controls. Has no effect on settings in the Tolerances column.
Use Part Tolerance	Uses format and tolerance information from the model. When selected, individual tolerance values in the Tolerances columns are not available, except tolerance controls for Countersunk Depth and Tap Drill Diameter. In part modeling, if a limits tolerance is specified for a hole parameter, the Tolerance and Precision dialog box settings are disregarded. The precision of the displayed parameter reflects the setting in part modeling.
Show All Parameters	Displays all hole parameter rows, regardless of the selected hole or thread type. Overrides the default setting, which shows only parameters relevant to the selected hole or thread type.
Unit Precision	Primary sets precision for hole diameter. Click the arrow to select a precision setting from the list. Not available if Use Global Precision is selected. Alternate sets precision for hole diameter in alternate units. Click the arrow to select a precision setting from the list. Not available if Use Global Precision is selected. If Linear Format on the Units tab of the Dimension style is set to Fractional, precision settings are shown as fractions. Decimal precisions correspond to fractional values, such as 1/8 is shown as .125. Format is also represented on Tolerances. An exception for hole notes is countersunk angle (always shown as decimal, unless the Angular Format on the Units tab of the Dimension style is set to Deg_Min_Sec).
Tolerances	Sets the tolerance values for the selected hole type. Check the box next to a symbol representing the hole parameter to set precision and tolerance values. Upper Sets the value for the upper tolerance. Enter the upper tolerance value. Lower Sets the value for the lower tolerance. Enter the lower tolerance value with a negative sign of operation. Not available if the selected method does not support a tolerance range. Method Sets the tolerance method. Click the arrow, and then select from the list. Precision, Precision (Alt)Sets the number of decimal places to display in the hole note. Values are truncated and rounded to the specified precision. Click the arrow, and then select from the list.

Chamfer notes

Use Global Precision

Sets parameter precision to the precision defined by the Precision setting on the Units tab of the active dimension style. When selected, individual parameters in the Precision column are not available. Clear the check box to edit individual precision controls.

Has no effect on settings in the Tolerances column.

Unit Precision

Primary sets precision for each chamfer parameter. Click the arrow to select a precision setting from the list. Not available if Use Global Precision is selected.

Alternate sets precision for chamfer distance values in alternate units. Click the arrow to select a precision setting from the list. Not available if Use Global Precision is selected.

If Linear Format on the Units tab of the Dimension style is set to Fractional, precision settings are shown as fractions. Decimal precisions correspond to fractional values, such as 1/8 is shown as .125. Format is also represented on Tolerances.

Tolerances

Sets the tolerance values for the selected parameter type. Check the box next to a symbol representing the parameter to set precision and tolerance values.

Upper Sets the value for the upper tolerance. Enter the upper tolerance value.

Lower Sets the value for the lower tolerance. Enter the lower tolerance value with a negative sign of operation. Not available if the selected method does not support a tolerance range.

Method Sets the tolerance method. Click the arrow, and then select from the list.

Precision, Precision (Alt) Sets the number of decimal places to display in the chamfer note. Values are truncated and rounded to the specified precision. Click the arrow, and then select from the list.

Lighting Styles

You can create lighting styles and use them to change the lighting effects. Lighting styles interact with appearances to control the visual display of a model.

The lighting settings including the active lighting style are stored in the model file.

Lighting Methods

There are two types of lighting methods. Scene lighting is used in the modeling environment and Studio lighting is used for the rendering environment. Scene lighting can be used for rendering by selecting

Standard Lights

Standard lighting consists of four lights, each of which can be on or off.

Standard lights are directional lights. Their position can be edited in relation to the model. Two position sliders adjust the light direction:

Horizontal (azimuth): Zero at the eye, -90 at left, +90 at right, and +-180 from behind, shining toward the camera
Vertical (altitude): zero at the eye, +90 coming from directly above, -90 coming from directly below

The lighting results differ based on the light Relative movement setting:

Camera space lights are fixed to the view camera or what is commonly referred to as screen space or your eye position. As the camera and lights move through the scene, the shadows update in real time. Light position settings are relative to the screen.
ViewCube space lights are positioned relative to the ViewCube Front face. This method allows you to rotate the model and have the shadows stay relative to the model without regard for camera position.

Shadows

The active lighting style sets the direction and appearance of shadows.

To display shadows, select All Shadows from the Shadows list on the View tabAppearance panel.

Inventor Studio light settings differences

In Inventor Studio, the major differences from above are:

A lighting style consists of an unlimited number of lights (however, only a limited number (8) are currently represented on screen).
Lights are positioned in world space - that is, their position is constant relative to model objects in the scene, even when the camera moves.
Lights can be:
- Directional: infinitely far away, with light coming in parallel rays from a given direction (like the sun).
- Point: at a defined position in world space, radiating in all directions equally.
- Spot: at a defined position in world space, pointing in a given direction, with output strongest along the direction they point, falling off over a given angle.
- Ambient light in the scene can be defined in more complex ways for offline rendering.
Each light can have a different shadow density, softness, and effect in the scene.

NoteWhen rendering with “Current lighting” as the selected lighting style, the model environment Standard lighting is used.

See Inventor Studio documentation for details.

Procedures

Managing lighting styles

On the ribbon, click Manage tab Styles and Standards panel Styles Editor.
In the Style and Standard Editor, expand Lighting to display available lighting styles.
To edit a lighting style, click the style, and change its settings on the Lighting Style panel. See the Style and Standard Editor - Lighting Style reference for more information.
TipTo preview the edits immediately, activate the edited lighting style, and display shadows.
To create a lighting style, select an existing lighting style to use as a template, click New, and enter the style name. Then edit settings of the new lighting style.
Click Save to save changes to the current document.
Click Done to close the Style and Standard Editor.

How to edit a lighting style

Add IBL Environments for lighting styles

Producing IBL environments for Inventor requires a level of photographic skill, used to product HDR images, and image editing technique. You can obtain and use additional IBL Environments with Inventor lighting styles.

Obtain additional IBL Environments

To go to the Autodesk Exchange App Store, near the right end of the title bar, click .
Locate, purchase, and download your new IBL environment.
Install the new IBL environment per the instructions.
NoteThe installation process locates the new environment with the installed environments. They are immediately accessible for use in an Inventor Lighting Style.

To use the new IBL Environment you must do either of the following:

Modify an existing lighting style

On the Manage tab Styles and Standards panel click Styles Editor.
Select an IBL lighting style where you want to use the new IBL environment.
In the Image Based Lighting section, change the Source by selecting the new IBL environment from the dropdown list.
Click Save.
In the View tab Appearance panel, select the modified Lighting Style.

Add a new Lighting Style

On the Manage tab Styles and Standards panel click Styles Editor.
Right-click an IBL Lighting style and click New Style.
In the New Local Style dialog box, change the name to indicate the new IBL environment.
In the Image Based Lighting section, change the Source by selecting the new IBL environment from the dropdown list.
Click Save.
NoteTo make the style available to all it must be saved to the Style library.
Optional: In the Style browser, right-click the new lighting style and click Save to Style Library.
In the View tab Appearance panel, select the new Lighting Style.

References

Style and Standard Editor - Lighting Style

Access:

Click Manage tab Styles and Standards panel Styles Editor

In the Style and Standard Editor, expand Lighting, and click a lighting style to edit.

TipSee the Style and Standard Editor reference for description of the general options.

Standard Lights

Light
Switches lights on and off, and selects lights to edit.
	Click to switch a light on or off.
	Click to select a light.

Settings (Light #)
Edits properties of the selected light.
	Move the vertical and horizontal sliders to specify the position of the selected light.
Color	Click the color pad to change the color of the light source.
Brightness	Use the slider to increase or decrease the intensity of the selected light source.
Relative Movement	Associates the selected light with the view camera. The behavior is like walking around in a room while using a video camera with its light on.
Relative Movement	Associates the selected light with the ViewCube. The scene provides the lighting and the lights do not move with the camera. When the ViewCube is redefined, the lighting direction is updated to represent the new position.
	TipThe Move with Camera and Fixed to ViewCube options enable you to mix the two settings within a single lighting style.

All Standard Lights
Sets all standard lights in the style. The values are applied equally for each light.
Brightness	Sets the intensity of all the directed light sources. Use the slider to increase or decrease the intensity.
Ambience	Sets the level of ambient light in the scene, controlling the level of contrast between the lighted and unlighted areas of a face. Move the slider left to increase the contrast; move it right to decrease the contrast.

Shadow Settings

Shadow Direction	Select a lighting direction to determine how the shadows look in the scene.
Density	Sets the light to dark ratio for Object and Ground shadows. Positive values make the shadow darker and negative lightens the shadow.
Softness	Sets the amount of blending between the shadowed and non-shadowed areas of the scene. Move the slider to the left to harden the shadow, reducing the softness, providing a more distinct line between shaded and non-shaded areas. Move the slider to the right to increase the softness and reduce the distinction between the areas.
Ambient Shadows	Sets the ambient shadow intensity. Ambient shadows have to do with the amount of light that is scattered into areas within or between parts, providing more realistic scene lighting. Negative values darken the ambient shadows, positive values lighten the ambient shadows.

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Table of contents

Styles and Style Libraries

Topics in this section

Manage styles in documents

Style Libraries

Transition legacy documents to a style library

Style Library Manager

Styles in drawings

Dimension styles in drawings

Lighting Styles

How to edit a lighting style