On the ribbon, click Place Views tab Sketch panel Create Sketch to create a 2D sketch. The sketch is added to the drawing sheet or, if a view is selected, is associated with the active view.

Once you create a sketch, the Sketch tab has commands you can use to create custom borders and title blocks, or to develop your own set of sketched symbols.

You can get model sketches in a drawing view by using Get Model Sketches command. After the model sketch is recovered, the sketch attributes do not automatically update with respect to changes in the model sketch. To update the attributes of the recovered sketch, right-click the sketch in the graphic window or in the browser, and select Reapply Model Properties from the menu.

If you translate AutoCAD data to a drawing, the geometry is placed on sketches in the drawing. AutoCAD line styles are maintained.

If you open an AutoCAD DWG or an Autodesk Inventor Drawing File (DWG) , the geometry is placed on sketches in the drawing. AutoCAD line styles are maintained.

Add sketches to drawings

A drawing sketch can contain text and 2D geometry such as lines and arcs. If a drawing view is selected when you activate the Sketch commands, the sketch is associated to the view. If no drawing view is selected, the sketch is associated to the drawing sheet.

If you copy a sheet or a drawing view, the associated sketches move with it. You cannot copy or move a sketch independently of its associated sheet or view.

A sketch cannot be copied, but you can copy the geometry in a sketch, and paste it in another drawing.

Tips for sketching in a drawing

Drawing sketches are associated with the active view or sheet.
In the Drawing Resources folder of the browser, right-click, and select options to develop sketched symbols, title blocks, or custom borders. Use sketch commands to create geometry.
On the ribbon, use View tab Navigate panel Zoom to zoom in on the area where you are working.
On the ribbon, click Tools tabOptions panel Document Settings. Select Sketch and set the grid to the optimal spacing to line up the sketch elements quickly.
On the ribbon, click Tools tabOptions panel Application Options. Select Sketch and check the Snap to Grid setting to more easily place sketch elements.
On the Quick Access toolbar, activate the Select commands to select a group of sketch elements, click in the graphics window, and then drag a box around the elements.
Use the dimension commands to set the size of sketched geometry or to add dimensions between the geometry in a sketch and elements in the underlying drawing view.
NoteWhen you use dimensions to set the size of elements in a title block or border, the dimensions are hidden when you finish editing.
Use Sketch Properties to change the color, line type, and line weight, or to suppress sketch formatting overrides and display the sketch with the default attributes.

Create sketched symbols

The drawing templates contain a Sketched Symbols heading in the Drawing Resources section of the browser so that you can create and save sketches for reuse. Sketched symbols can contain 2D geometry, bitmap images, static text, prompted text boxes, or properties fields that update automatically.

To make the sketched symbols available in new drawings, save them in a template that you use to create drawings.

TipTo copy a sketched symbol to another drawing, right-click a sketched symbol and choose Copy from the menu. Open the destination drawing, right-click the Sketched Symbols entry and choose Paste.

Create title blocks

The templates provided with Autodesk Inventor contain one or more standard title block formats that you can modify and use. You can also sketch custom title blocks, and save them as drawing resources. Title blocks can contain 2D geometry, bitmap images, static text, prompted text boxes, or properties fields that update automatically.

To use the custom title blocks in all your new drawings, save them in a template that you use to create drawings.

TipTo copy a title block format to another drawing, right-click a title block format, and choose Copy from the menu. Open the destination drawing, right-click the Title Blocks entry, and choose Paste.

Create custom borders

The templates provided with Autodesk Inventor contain a default border. You can modify the border or sketch custom borders and save them as drawing resources.

Custom borders can contain 2D geometry, bitmap images, static text, prompted text boxes, or properties fields that update automatically. To use a custom border in new drawings, save it in a template that you use to create drawings.

All drawing borders have four points at the sheet corners that cannot be deleted. These points move when the sheet is resized. If you constrain the custom border geometry to these points, it adapts to any sheet size.

TipTo copy a drawing border format to another drawing, right-click a border format in the browser of the source drawing, and then choose Copy. Open the destination drawing, right-click the Borders entry in the browser, and then choose Paste.

Translate DWG data

When you translate 2D data from a DWG file to an Autodesk Inventor drawing, the geometry is placed on one or more sketches in the drawing. Dimensions are placed on the drawing sheet.

To place dimensions attached to the geometry on the sketches, select Promote Dimensions to Sketch in the Import Destination dialog box when opening an AutoCAD file. AutoCAD line styles are maintained.

Blocks in the DWG file are translated to sketched symbols. You can also translate selected data in a DWG file to Autodesk Inventor title blocks and borders.

NoteWhen using the Drawing Resource Transfer Wizard to copy drawing resources such as borders and title blocks from a source to one or more target drawings, prompted entries may not transfer correctly if they do not match exactly in the source and target files.

Procedures

Add a sketch to a drawing

On the Sketch tab, use the commands to add sketched elements to a drawing. Drawing sketches are associated with the drawing sheet, but if a drawing view is selected, the sketch is associated with the view.

Create a sketch

Select the sheet or drawing view you want to associate to the sketch.
On the ribbon, click Place Views tab Sketch panel Create Sketch.
Use commands on the Sketch tab to create the sketch geometry.
When finished, right-click and select Finish Sketch.

Show Me how to create a constrained sketch and rotate a view with sketch

Edit a sketch

To add sketch geometry to an existing sketch, right-click a sketch in the browser, and then select Edit.

Change attributes of the sketch geometry

You can view or change line attributes for new or edited sketch geometry.

Right-click the sketch in the browser, and then select Edit.
Select the sketch geometry in the graphic window.
Use Sketch Properties to change the color, line type, or line weight of the selected sketch geometry.
Tip: On the ribbon, click Sketch tab Format panel Sketch Properties to display the Sketch Properties toolbar.
To suppress sketch formatting overrides and display the sketch with default attributes, select Formatting Toggle in the Sketch Properties toolbar.
TipUnselect Formatting Toggle to show user formatting again.

Hide individual elements in a drawing sketch

You can hide one or more sketch elements in a drawing sketch without making the entire sketch invisible by setting the Sketch Only attribute.

Select the sketch elements you wish to hide.
On the ribbon, click Sketch tabFormat panel Sketch Only to turn on the attribute.

Geometry with the Sketch Only attribute set is hidden when you exit from sketch mode and is no longer visible on the face of the drawing.

If you wish to restore the visibility of the hidden sketch elements:

Right-click the sketch in the browser, and then select Edit. The hidden elements are visible in the sketch.
Select the sketch geometry you wish to unhide.
On the ribbon, click Sketch tabFormat panelSketch Only to turn off the attribute.

Get model sketches in a drawing

Expand the drawing view in the browser.
Right-click the model (assembly or part) node, and select Get Model Sketches from the menu.
To include projected and derived sketch geometry, right-click the sketch node in the browser, and select Display Reference.

NoteAfter the model sketch is recovered, the sketch attributes do not automatically update with respect to changes in the model sketch. To update the recovered sketch, right-click the sketch in the graphic window or in the browser, and select Reapply Model Properties from the menu.

Tips:

To make the sketch invisible, right-click the sketch node in the browser and unselect the Visibility option. To reset the sketch visibility, right-click the sketch node in the browser and select the Visibility option. Changes to visibility retain object property changes.
To hide all sketch texts, right-click the sketch node in the browser and unselect Display Text. When you unselect the Display Text option, all sketch texts and property changes are discarded.
To hide all the reference geometries, right-click the sketch node in the browser and unselect Display Reference. When you unselect the Display Reference option, all sketch reference geometries and property changes are discarded.
To make a sketch text invisible, right-click the sketch text in the graphic window, and unselect the Visibility option. To reset the text visibility, exclude and include the sketch (which resets all properties), or uncheck and recheck the Display Text.
To make a reference geometry invisible, right-click the reference geometry in the graphic window and unselect the Visibility option. To reset the reference geometry visibility, exclude and include the sketch (which resets all properties), or uncheck and recheck Display Reference, or use Show Hidden Edges context menu.
When reference edges are invisible, edge visibility can be reset using the Show Hidden Edges option in the Drawing View, and selecting the edges to get them displayed again.
To display the model sketch with default attributes, open the source model file, select Formatting Toggle in the Sketch Properties toolbar, and then Reapply Model Properties in the drawing.
For a view of a sheet metal part, only the model sketches in one of the models (folded model or flat pattern model) can be recovered.
To override the properties for recovered model sketch geometries or texts, select one or multiple objects in the graphic window, right-click, and choose Properties or Color from the menu.

Create a symbol in a sketch

The browser for each drawing or drawing template contains a Sketched Symbols folder in the Drawing Resources folder. When you create custom symbols, they are added to Sketched Symbols available to use in the drawing.

A sketched symbol can contain geometry, text, or imported bitmap images.

Open a drawing file or drawing template.
On the ribbon, click Manage tabDefine panel Symbol.
If you prefer, right-click the Sketched Symbols folder in the browser and select Define New Symbol.
On the Sketch tab, use the commands to create the symbol.
To add an insert point to the sketch,
- Click a point in the sketch to select it.
- On the ribbon, click Sketch tab Format panel Set Insertion Point Grip. A sketched symbol can have only one insert point.
To add connection points to the sketch,
- Click a point in the sketch to select it.
- On the ribbon, click Sketch tab Format panel Connection Point Grip.
- Add as many connection points as needed.
Right-click and select Save Sketched Symbol. Enter the new symbol name in the dialog box. The symbol is added to the Sketched Symbols folder in the browser.

NoteTo make sketched symbols available to all new drawings, add them to the template you use to create drawings.

Create a draft sketch

A draft sketch is a special drawing view that contains no representation of a model. When you open an AutoCAD file as an Autodesk Inventor drawing, a new file is created with a sheet that contains a draft sketch. Geometry from the AutoCAD file is placed in the draft sketch.

You can scale a draft sketch and give it a label. If you later copy data from a draft sketch to another sketch, the copied geometry is shown with a 1:1 scale in the sketch.

You can add a draft sketch even if you do not have AutoCAD data:

Add or activate a drawing sheet on which to place the draft sketch.
On the ribbon, click Place Views tabCreate panel Draft.
In the Draft View dialog box, enter a label and scale for the draft view. Select check boxes to show the label and scale on the draft view.
Use sketch commands to add geometry, text, and dimension as needed.
Right-click and select Finish Sketch.

Show model sketches in drawing views

You can show unconsumed and consumed sketches from a model in a drawing view of the model. You cannot edit a model sketch in the drawing.

Only sketches that are parallel to the view can be displayed.

Place a drawing view of a model containing one or more sketches.
In the browser, click to expand the view and display the components in the view.
Right-click the assembly or any component containing a sketch, and select Get Model Sketches.

NoteSketches consumed by assembly features cannot be displayed in a drawing view.

Add hatch/color fill to drawing sketches

Click Fill/Hatch Sketch Region to hatch or color fill an enclosed boundary in a drawing sketch.

On the ribbon, click Place Views tab Sketch panel Create Sketch to create a drawing sketch or double-click an existing sketch in the browser to make it active.
Use the sketch commands to create a sketch that forms a closed loop.
On the ribbon, click Sketch tabDraw panel Fill/Hatch Region.
In the graphics window, select the sketch loop you want to fill or hatch.
In the Hatch/Color Fill dialog box, select options, and then click OK.
- To add hatching, switch Hatch on. Hatch style assigned to the Sketch Hatch object in Objects Defaults is applied on the hatch fill.
  If appropriate, change the hatch attributes: Select another hatch patterns, edit the hatch angle, scale or shift, or change the Line Weight. Select Double to add a copy of the specified hatch pattern perpendicular to the first hatch pattern. All edits are kept as object overrides.
  TipTo use a hatch pattern that is not available in the Pattern list, select Other in Pattern. Then set the hatch pattern as Offered or load the hatch pattern from a PAT file using the Select Hatch Pattern dialog box.
- To add a color fill, switch Color Fill on. Then select a color in the Color dialog box and click OK.
Right-click, and then select Done. Right-click again, and then select Finish Sketch to close the sketch.

Show Me how to create and edit a sketch hatch fill

Show Me how to shift the sketch hatch fill pattern

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

Edit or delete the hatch/color fill

When you edit attributes of a hatch fill, all edits are kept as object overrides.

To edit a sketch with hatch/color fill, double-click the sketch in the browser.
On the ribbon, click Sketch tabDraw panel Fill/Hatch Region.
In the graphics window, select the sketch with the hatch/color fill.
In the Hatch/Color Fill dialog box, change options, and then click OK.
- Change the hatch attributes: Select another hatch patterns, edit the hatch angle, scale or shift, change the Line Weight, or select Double to create a crosshatch.
- To use a hatch pattern that is not available in the Pattern list, select Other in Pattern. Then set the hatch pattern as Offered or load the hatch pattern from a PAT file using the Select Hatch Pattern dialog box.
- Change the color of the color fill in the Color dialog box.
- To switch between hatch and color fill, switch Hatch or Color Fill on.
- To delete the hatch or color fill, switch off both Hatch and Color Fill.
Right-click, and then select Done. Right-click again, and then select Finish Sketch to close the sketch.

References

Hatch/Color Fill

Adds hatch or color fill to an enclosed boundary in a drawing sketch.

Access:

In an active drawing sketch, click Sketch tabDraw panel Fill/Hatch Region.

And then select a closed sketch profile in the graphic window

	Hatch switches the hatch fill on. Enables the Hatch options
	Color Fill switches the color fill on. Enables the Color option.
Pattern	Selects the hatch pattern to use. Select Other to add a hatch pattern to the Pattern list. Then add the hatch pattern 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.
Thumbnail	Displays a preview of the hatch pattern definition.
Line Weight	Sets the hatch line weight.
Double	Creates a copy of the specified hatch pattern perpendicular to the first hatch pattern.
Color	Sets the color of the fill for the selected sketched profile. Click to open the Color dialog box and select the color.

Show Me how to shift the sketch hatch-fill pattern

Part, Feature, or Edge properties

Changes the line type, line weight, and color for selected edge, feature or part to the value specified in the style or for the current document, overrides values set in the style.

Manages properties for view edges, symbols, feature and component selection priorities, trails, user-defined symbols, and sketch geometry.

NoteYou can load and use line types from AutoCAD *.lin files as the line type for an edge property.

Access:

Right-click on the edge of an object, and then select Properties from the menu.

By Layer	Available only when the Select command on the Quick Access toolbar is set to either Feature Priority or Part Priority. Select the check box to show properties specified as By Layer. Clear the check box to set Line Type, Line Weight, or Color independently.
Line Type	Specifies how a line or type of curve is displayed. Set to By Layer to inherit the line type specified for the layer. NoteTo load an AutoCAD .lin file, select Other from the bottom of the Line Type list. For more information, see Select Line Type (LIN file).
Line Weight	Specifies the thickness of the line type. Set to By Layer to inherit the line weight specified for the layer.
Scale	Available only in a drawing sketch. Changes the scale of the selected line type. Enter scale size in the text box.
Color	Sets the line color for the line type. Set to By Layer to inherit the color specified for the layer.

Format Text

Use the Format Text dialog box to set the attributes for a drawing or sketch text.

Access:

Ribbon: Sketch tab

Draw panel

Text

Style

Specifies the text style to apply to the text. Click the arrow and select from the list of available text styles.

Text attributes

Specifies the paragraph attributes for selected text.

	Justification positions the text within the text box. Left, Center, or Right Justifications position the text relative to sides of the text box. Top, Middle, or Bottom Justifications position the text relative to the top and bottom of the text box.
	Base Line Justification is available when Single Line Text is selected and when creating sketch text.
	Text box allows constraining and dimensioning to text. Available only for sketch text.
	Fit text sizes the text to fit the designated space, such as a text box. Available only for sketch text.
	% Stretch specifies the text width. Enter 100 to display the text as designed, enter 50 to decrease the width of the text by 50%.
	Single line text removes all line breaks from multiline text. Available only for sketch text.
	Spacing sets the line spacing to Single, Double, 1.5 Lines, Multiple, or Exactly.
	Value specifies the value for line spacing, when you set line spacing to Exactly or Multiple.

Font attributes

Specifies the font attributes for the text.

Font	Specifies the text font. Click the arrow and select from the list of available fonts.
Font Size	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. TipEdit the standard settings to customize the list of pre-defined font sizes. Open the Style and Standard Editor and click the current standard. Then add or remove font sizes in the Preset Values list on the General tab.
Style	Sets the style. Click Bold, Italic, or Underline to apply the style to the text.
Stack	Stack strings in drawing texts to create diagonal or horizontal stacked fractions, and superscript or subscript strings. The option is available only if a string in a correct stacking format is selected in the edit field. Examples of correct stacking format: 1#2 stacks as a diagonal fraction. 1/2 stacks as a horizontal fraction. 1^2 stacks as a tolerance (1 over 2). TipTo edit properties of stacked text, select a stacked text in the edit field, right-click, and select Properties.
Color	Specifies the text color. Click the Color command, and then select a color from the Color dialog box. In the Color dialog box, select the By Layer check box to set the color specified by the text layer. Clear the check box to select a color. The color command shows the selected color or layer color.
Rotation Angle	Sets the angle of the text. Rotates the text around the insertion point. For example, if text is top and left-justified, the text rotates around the top left corner. Click the arrow to select the rotation orientation or enter the angle of rotation in the edit box. For drawing notes, you can rotate to any angle. Enter the angle or click the arrow to select predefined angles or a recently used angle. NoteThe Rotation Angle option is not available in a part file. Use the Rotate command, or create a new UCS to orient the text.

Model, Drawing, and Custom Properties

When retrieving model properties, the model source depends on the sketch type:

Sheet or Draft View sketch	Top-level model of the first view on the sheet. If the first base view on the sheet is deleted, the next base view on the sheet becomes the data source for properties.
View sketch	Top-level model of the view.

NoteWhen the drawing update status is deferred or the referenced model document is unresolved, model-based text property values do not update.

Type	Specifies property types from the drawing, the source model, and the custom property source file (for external and model custom properties) specified on the Drawings tab of the Document Settings dialog box. Available when creating or editing sketch text (in Sheet, View, or Draft View sketches), symbol text, title block and border text. Note Each external property set defined in either the drawing or the model file has an entry with that property set name in the list. If the source model contains at least one custom property, the Custom Properties - Model property type is available. In sheet metal drawings, select the Sheet Metal Properties type to add the Flat Pattern Extents Area, Width, or Length in text. Select the Physical Properties - Model property type to add the model Mass, Density, Volume, and Area in the text. If the displayed value of a physical property is N/A, physical properties of the model are out of date. To update the model, open the model file and choose Manage tab Update panel Update Mass. All values of physical properties are displayed with the unit string.
Property	Specifies a property associated with the selected Type. Available when creating or editing all drawing text, including text properties in notes, leader text, sketch text, symbol text, title block, and border text.
Precision	Specifies the precision for numerical properties displayed in the text. Select the desired precision from the list.
	Add Text Parameter inserts the parameter selected in Type and Property to the text. Available when creating or editing drawing text, including sketch text, symbol text, note text, leader text, title block, and border text. Not available for Prompted Entry type.

Parameters

Selects a named parameter and inserts its value into the text at the insertion point. Parameter options are available only when adding or editing text in general drawing notes and dimension text.

NotePart text does not use parameter settings.

Component	Specifies the model file that contains the parameter. If the drawing contains views of more than one model, click the arrow, and select the file from the list. If the drawing contains derived parts, the donor parts are also included in this list.
Source	Selects the type of parameter to show in the Parameter list. Click the arrow and select from the list. Model Parameters lists the named parameters automatically added to the model when you add dimensions or features. User Parameters lists the user parameters added to the model.
Parameter	Specifies the parameter to insert into the text. Click the arrow and select from the list. The parameters in the list change, depending on the Source you selected.
Precision	Specifies the precision for numerical parameters displayed in the text. Select the desired precision from the list.
	Add Parameter adds the selected parameter from the selected component to the text.

Symbol

Inserts a symbol into the text at the insertion point. Click the arrow and select the symbol from the palette. The top three symbols are diameter, degree and plus-minus, and they use the active font. All other symbols use the AIGDT font. In drawings, the available symbols are determined by the active drafting standard.

At the bottom of the symbol list, the Windows Character Map command accesses characters not available as standard keyboard characters. In the Character Map, click a character, and then click Select and then click Copy. In the Format Text pane, right-click and select Paste.

Zoom commands

Zooms in or out on the text and symbols in the edit box. Click the up arrow to zoom in, click the down arrow to zoom out.

Comments

Comments1

andrewcarlileThu May 17, 2012 3:30 pmWhat about points in a drawing sketch? How can i get those to show up?

Inventor

Community Scoring

Tag Tags0

Page statistics

Sketches in drawings

Table of contents

Comments1