Creating a Draft

You can create draft by selecting a neutral element. Drafts are defined on molded 3D shapes 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.

Before you begin: Create a 3D shape containing a volume.
Related Topics
Creating Volumes

  1. Click Draft Angle from the Volume drafts sub-toolbar.

    The Draft Definition dialog box is displayed and an arrow appears on a plane, indicating the default pulling direction. This dialog box displays the constant angle draft option as activated. If you click the icon to the right, you then access the command for creating variable angle drafts.

  2. Select the Selection by neutral face check box to determine the selection mode.

  3. Select the upper face as the neutral element. This selection allows the application to detect the face to be drafted.

    The neutral curve is displayed in pink. The faces to be drafted are in dark red. The Support field is filled with the volume owning the selected face.

  4. Set the Propagation option:


    • None: there is no propagation
    • Smooth: the application integrates the faces propagated in tangency onto the neutral face to define the neutral element.

  5. Define the Pulling Direction:

    By default, it is normal to the neutral face and is displayed on top of the 3D shape. The Controlled by reference option is now activated, meaning that whenever you will edit the element defining the pulling direction, you will modify the draft accordingly. Note that when using the other selection mode (explicit selection), the selected objects are displayed in dark pink.

  6. The default angle value is 5 degrees. Enter 7 degrees as the new angle value.

    The application displays the new angle value in the geometry.

  7. Click Preview to see the draft to be created.

    It appears in light blue:

  8. Click OK to confirm the operation.

    The element (identified as Draft.xxx) is added to the specification tree.

    For more information, refer to Part Design User's Guide : Creating Basic Drafts or Creating Drafts with Parting Elements.