To Work with Sketches in Drawings

You can create and edit sketches in drawings, get model sketches in a drawing, and create symbols in a sketch.

Create a Sketch

On the ribbon, click Place Views tab Sketch panel Create Sketch .

1. Click in the graphic window to place the sketch on the sheet, or select a drawing view to associate the sketch to the view.
2. Use commands on the Sketch tab to create the sketch geometry.
3. When finished, right-click and select Finish Sketch.

Edit a Sketch

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

Change Attributes of the Sketch Geometry

You can add sketch geometry to an existing sketch and view or change its line attributes.

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.
4. To suppress sketch formatting overrides and display the sketch with default attributes, toggle Show Format on in the Sketch tab, Format panel.
   Tip: Toggle Show Format off 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.

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. A drawing view cannot display sketches consumed by assembly features.

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 browser, and select Reapply Model Properties from the menu.

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.

1. Place a drawing view of a model containing one or more sketches.
2. In the browser, click to expand the view and display the parts or components in the view.
3. Right-click the part or assembly or any component containing a sketch, and select Get Model Sketches.
4. To include projected and derived sketch geometry, right-click the sketch node in the browser, and select Display Reference.
5. (Optional) Do any of the following to modify the recovered sketch:
   • 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 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.
   • 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.
   • 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.