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 or balloon 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 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 Balloon object to MyBalloonLayer. The result is that all balloons created using MyStandard, with the layer set to By Standard, updated to use MyBalloonLayer.

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 the CAD administrator has locked it 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 of the current project (click From Library).
  TipChange the Default Hatch Pattern to correspond to the hatch pattern 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 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 layer.

In a Drawing file (Autodesk Inventor 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 material names from the material library of the current project.
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 Bend Note Bend Table Bend Tag Border Text Chamfer Note Configuration Table General Table Leader text Punch Note 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
Bend Note	DEFAULT
Bend Table	Table_DEFAULT
Bend Tag	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
Punch Note	DEFAULT
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 assembly configuration tables, spot-weld tables, 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.

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