Creating a Sketch

Creating a sketch is often the first step in creating a solid body. Sketches are associated with planar surfaces, which are known as sketch planes.

To create a sketch:

  1. Identify the planar surface on which to create the sketch. This planar surface can be one of the default sketch planes, a previously created transform sketch plane, or the surface of an existing body.

    See Sketch Planes.

  2. Activate the sketch tool on the chosen surface. The method that you use depends on the type of surface:
    • For a default sketch plane, or a transform sketch plane, right-click the corresponding feature node in the feature tree, or the actual feature in Graphics window and choose Create Sketch.
    • For the face of an existing body, right-click the face in the Graphics window and choose Create Sketch > On Face.
    • To place the sketch at the face center on an existing body, right-click the face in the Graphics window and choose Create Sketch > At Face Center.
    The Sketch panel appears in the left-hand side of the window. The Sketch panel contains the Create Sketch Entities and Display Options boxes. A sketch grid with the local X and Y axes appears within the Graphics window.

  3. Use the tools in the Display Options box to control the appearance of the sketch environment in the Graphics window. See Sketch Display Options.
    To make the 3D-CAD View scene normal to the sketch plane, click (View Normal to Sketch Plane).
    If you subsequently rotate or move the scene while in sketch mode, you can return to the normal view by clicking (View Normal to Sketch Plane).
  4. Use the tools in the Create Sketch Entities box to create the sketch. See Sketch Entity Reference.
    As you draw sketch in 3D-CAD, the color of the entities change depending on their state. Active entities are colored in purple.

    When you click to finalize an entity, the color changes to blue. If your CAD model has multiple 2D or 3D sketches, active sketch primitives are in blue color and the remaning background sketches appear in dark rose.
    3D-CAD applies some constraints interactively as you sketch. For example, lines that you draw in the vertical direction appear in red and snap to this direction. When you click to draw the line in this position, a vertical constrain is added automatically.

    Similarly, when you draw in the horizontal direction, the entity is displayed in yellow and a horizontal constraint is added.

    Other interactive constraints include tangent, parallel, coincident, and perpendicular.

  5. Add further constraints that fix the position of sketch entities relative to each other, and to specific locations. See Constraining a Sketch.
    Some constraints require that you select multiple sketch entities before they appear in the context menu.
    For a full list of constrain types, see Constraint Types.
  6. Dimension the sketch using constant sizes or parametric expressions. See Dimensioning Sketches.


  7. If a sketch entity is overlapping with or hidden by another object, use the depth selector to cycle through the entities and select the desired one. See Selecting Hidden and Obscured Entities in a Sketch.
  8. When the sketch is complete, click OK in the Sketch panel.
    A Sketch node is added to the feature tree. You can edit and duplicate existing sketches using the Sketch node.
To edit an existing sketch:

  1. Right-click the corresponding sketch node and select Edit.
    This action automatically rolls back the 3D-CAD model to the selected sketch and activates Sketch Mode.
  2. Modify your sketch using the tools available in the Sketch panel. You can create, edit, and delete sketch entities.
  3. Click Apply to confirm the changes and exit the sketch.

If the changes cause any feature in the model to fail to rebuild properly, the feature state of affected features changes. To resolve the issue, update the model, or edit the affected features.

To duplicate a sketch:

  1. Right-click a Sketch node and select Duplicate.

    An identical sketch feature is added to the feature tree. When you carry out this operation on a Face Sketch, an ordinary sketch feature is created. Duplicating a sketch feature also retains any design parameters that are associated with that sketch. Editing the design parameter affects both the original sketch and the duplicate sketch.