New Sketch to Reference Geometry

You can add a sketch to the reference geometry of part which has been added to an assembly model. If the part is not a part of an assembly, this function does not exist in the context-sensitive menu.

In Context-sensitive Menu

  1. Open the assembly model in the working window.
  2. Edit a part or create a new part.
  3. Select the context-sensitive function New Sketch > To Ref. Geometry... > Face / Line / Plane by 3 Points.
  4. Select a face, line or three points according to what you selected in the previous step.
  5. Draw a sketch or read an existing sketch from the sketch library.
  6. Accept the sketch by selecting the context-sensitive function OK or cancel it by selecting the context-sensitive function Exit.

Fixing a New Part Automatically to Reference Geometry

Geometric constraints are automatically created for a new part when you add a new sketch to reference geometry, for example to a face or a line in the assembly, as the first phase of creating a new part.

To Face added is created the following constraints.

  • A Coincident constraint between the Z axis of the part's origin, corresponding with the part's XY plane, and the selected planar face.
  • A Coincident constraint between the part's origin and the origin of the sketching coordinate system of the selected planar face.
  • A Coincident constraint between the X axis of the part's origin, corresponding with the part's YZ plane, and the direction point of the X axis of the sketching coordinate system of the selected planar face.

Added to a Straight Line, the following constraints are created:

  • A Coincident constraint between the part's origin and the selected line.
  • A Coincident constraint between the Z axis of the part's origin and the selected line.

Added to a Circle or an Arc, the following constraints are created:

  • A Coincident constraint between the part's origin and the selected line.
  • A Tangential constraint between the Z axis of the part's origin and the selected line.