Sketch based features

Sketch Based Feature is a BricsCAD feature that allows you to edit a 2D entity used to create a 3D solid and automatically update the 3D solid.

The EXTRUDE, LOFT, SWEEP, and REVOLVE commands and their options Subtract and Unite create sketch features when the CREATESKETCHFEATURE system variable is ON. The sketch features are available in the Mechanical Browser panel.

Note: An automatic conversion algorithm runs when opening a drawing that contains old sketch features.
If something goes wrong, you must decide whether to continue the conversion.
  • If yes, the algorithm will do its best to convert the features, guessing the geometry of arbitrary features. However, the converted Boolean features (UNITE or SUBTRACT) will not be properly renamed, even though the algorithm treated them as Booleans.
  • If not, it dissolves the old sketch features and keeps only the 3D features.
Important: Sketch features created when the CREATESKETCHFEATURE system variable is ON are not compatible with other CAD programs. When you manually SAVE these drawings, a warning message appears in the Command line and in a Warning balloon at the bottom right side of the drawing: "This drawing contains sketch features that are not compatible with other CAD programs. These features might break if you open the drawing using another CAD program!".

Create a 3D solid

  1. Turn ON the CREATESKETCHFEATURE system variable.
  2. Draw a 2D entity, such as a closed polyline.
  3. Optionally, add parametrics to the Sketch entity.
  4. Launch the EXTRUDE, LOFT, SWEEP, or REVOLVE command to create the 3D Solid features, which are visible in the Mechanical Browser panel.

Sketch features can be copied/pasted into the same or a different drawing. The SKETCHFEATURECOPYMODE system variable will dictate the behavior of the copied sketch features.

When the SKETCHFEATURECOPYMODE system variable is ON, copies of sketch features will be independent of their source (new blocks of the sketches/paths/guide curves/etc. will be created). When it is OFF, copies of sketch features will share their sketches (paths, guide curves, etc.) with their source.

Edit the 3D solid by editing the corresponding sketch entity

A Sketch feature is created from the 2D entity as a block and moved to a new layer: BC_SKETCHES. This layer is turned Off by default.

All Sketch features will be visible in the Mechanical Browser panel.

Method 1

To edit the Sketch feature, right-click the entity in the Mechanical Browser panel and select Edit geometry.

After save the changes for the Sketch feature (BCLOSE command), the 3D solid is automatically updated.

Method 2

To edit the Sketch feature you can also use the BEDIT command that opens the Create or Edit Block Definition dialog box from where you select the Sketch feature to open it in Block Editor.

Method 3
To edit the Sketch feature you can also launch SKETCHEDIT command. Provide the Sketch Based Feature (3D solid) and Sketch names, and after making all changes and pressing the ENTER key, the 3D solid is updated.

To modify a Sketch Based Feature (3D solid), there are two methods:

Method 1

Click the Solid in the Mechanical Browser and adjust the properties in the bottom of the Mechanical Browser panel.

Method 2
Launch the UPDATESKETCH command and specify in the Command line the name of the feature, the name of the parameter, and its new value.

Removing all created sketch entities

Launch the REMOVESKETCHFEATURE or DISSOLVESKETCHFEATURE commands to remove only the sketch features. The REMOVESKETCHFEATURE command does an additional purge after the DISSOLVESKETCHFEATURE command.

Both commands keep the contents of the scene untouched.

Note: You can also dissolve the sketch features of a 3D solid by choosing the Dissolve option from its context menu in the Mechanical Browser panel.

Deleting all features

Launch the DELETESKETCHFEATURE command to delete the sketch features and their corresponding 3D solid.

Note: You can also delete a sketch based feature (3D Solid) by choosing the Delete option from its context menu in the Mechanical Browser panel.