About Dimensions from Part Design Features

The following dimensions can be generated:

• Some or all hole dimensions from a hole parameter (except if these parameters cannot be associated with an existing geometrical element to generate dimensions: diameter of a tapered hole out of the part, depth for a blind hole setting a through hole).
• Pad/Pocket length: if two limits are defined, two dimensions are generated between the sketch plane and each limiting face, and sketch constraints.
• Multi-Pad/Multi-Pocket lengths, and sketch constraints.
• Shaft/Groove distance constraints that are parallel or perpendicular to the shaft/groove axis direction, distance between the shaft/groove axis and point, or straight line or circle (arc or complete) as a half dimension diameter if the shaft/groove is not complete (value of the single angle or total of the 2 less than 360 degrees, as regular diameter if the shaft/groove is complete, angle, and sketch constraints.
• Chamfer features; dimensions are generated according to the Part Design chamfer feature definition: for a chamfer with a length x length definition, the dimension format is distance x distance, whereas for a chamfer with a length x angle definition, the dimension format is distance x angle dimension. However, if the tolerances are applied to chamfer parameters, only the tolerance applied to the first parameter is generated. Chamfer dimensions cannot be edited, but they can be modified through the Dimension Properties and the Edit Properties command.

  The Chamfer Dimension command is available for the following geometry selection:

  • A single face of a chamfer part design feature.
  • A conical face.
  • Two adjacent nonparallel and nonperpendicular planar faces. Further, the first selected face shares an edge with a third planar face, and this edge is parallel to the edge shared by the two selected faces.
  • Three faces of the following types:
    • Plane/plane/plane
    • Plane/cone/cone
    • Plane/cone/cylinder
    • Cylinder/cone/cylinder, provided that cone-cone, cone-cylinder, and cylinder-cylinder geometries are coaxial.

• Thread features; thread diameter, depth, and pitch parameter dimensions can be generated. Dimension generation automatically generates a thread symbolic representation.

  Important: Any tolerance attached to the pitch or diameter parameter is not generated. Generating a pitch parameter dimension requires the generation of the corresponding thread diameter parameter dimension. If the thread is not a metric one, the prefix is a diameter symbol instead of the letter M. You can select User Feature and explore them to find Part Design features permitted in generative command. The command recursively searches each compatible internal Part Design features (in the same way User Feature containing other User Features) to show parameters (if nothing could be analyzed by the generative command, no parameter is displayed). Moreover, you can immediately select all of them in the generative command list as if User Feature does not exist. Only published parameters (during User Feature creation) are seen in the list and corresponding dimensions could be created.

Important: A dimension is only linked with a sketch parameter when the dimension is based on the 3D geometrical elements generated from parametrized sketch elements. Dimensions are associated with the design of a part, including the Mean Dimension behavior. When parameter tolerances are defined, they are specified to the dimension tolerances. Modifying the dimension tolerances modifies the parameter tolerances and vice versa. A generated dimension is always created in an annotation plane parallel to the related feature internal parameter plane and this annotation plane is not necessarily the active annotation plane: If an annotation plane parallel to the feature internal parameter plane already exists, the dimension is created in this annotation plane, Otherwise a new annotation plane is created parallel to the feature internal parameter plane.