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

1. Select the sheet or drawing view you want to associate to the sketch.
2. On the ribbon, click Place Views tab Sketch panel Create Sketch .
3. Use commands on the Sketch tab to create the sketch geometry.
4. 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.

1. Right-click the sketch in the browser, and then select Edit.
2. Select the sketch geometry in the graphic window.
3. 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.

4. To suppress sketch formatting overrides and display the sketch with default attributes, select Formatting Toggle in the Sketch Properties toolbar.
   Tip: Unselect 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.

1. Select the sketch elements you wish to hide.
2. 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:

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

Get model sketches in a drawing

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

Note: After 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.

1. Open a drawing file or drawing template.
2. On the ribbon, click Manage tab Define panel Symbol .

   If you prefer, right-click the Sketched Symbols folder in the browser and select Define New Symbol.

3. On the Sketch tab, use the commands to create the symbol.
4. 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.
5. 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.
6. 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.

Note: To 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:

1. Add or activate a drawing sheet on which to place the draft sketch.
2. On the ribbon, click Place Views tab Create panel Draft .
3. 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.
4. Use sketch commands to add geometry, text, and dimension as needed.
5. Right-click and select Finish Sketch.