Creating a Variable Draft Angle

  Drafts are defined on molded parts to make them easier to remove from molds.
There are two ways of determining the objects to draft: either by explicitly selecting the object or by selecting the neutral element, which makes the application detect the appropriate faces to use.
Sometimes, you cannot draft faces by using a constant angle value. This task shows you another way of drafting: by using different angle values.
Open the Draft1.CATPart document.

  1. Click Draft Variable Angle from the Volumes drafts sub-toolbar.

    As an alternative, you can click Draft Angle , then click Variable available in the dialog box. For more information, see Creating a Draft.
    The Draft Definition dialog box appears, displaying the variable angle draft option as activated. If you click the icon to the left, you then access the command for performing basic drafts.

  2. Select the Face to draft.

    Multi-selecting faces that are not continuous in tangency is not allowed.

  3. Select the upper face as the Neutral Element.

    An arrow appears on the part, indicating the default pulling direction. The application detects two vertices and displays two identical angle values.
    The Support field is filled with the volume owning the selected face.

  4. Increase the Angle value: only one value is modified accordingly in the geometry.

  5. To edit the other angle value, select the value in the geometry and increase it in the dialog box. For instance, enter 7.

    Alternatively, double-click this value to display the Parameter Definition dialog box, then edit the value.

  6. Click Preview to see the draft to be created:

  7. Click the Points field to add a point.

  8. Click a point on the edge.

  9. Enter a new angle value for this point: for example, enter 17.

  10. Click OK to confirm the operation.

    The element (identified as Draft.xxx) is added to the specification tree.
    For further information about drafts, refer to Creating Basic Drafts and Creating Drafts with Parting Elements in Part Design documentation.