Creating a Draft

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.

This task shows you how to create a basic draft by selecting the neutral element.
Open the VolumeDraft1.CATPart document.

  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. Check Selection by neutral face 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 part. The pulling direction is displayed near the draft area to make it visible. As per the inputs given for creating a draft, the pulling direction arrow is located around the below elements in the given priority order:
    • Face as a neutral element
    • Neutral curve
    •  Face or surface as a pulling direction
    •  Faces to draft
    •  Elements like axis, line, or plane as pulling direction
    • Origin of a 3D part
         		  
      You can dock the pulling direction arrow on the top right corner of the window. To do so, right-click the pulling direction arrow and select Display indicator frozen on the screen.
    The same pulling direction that you specified for creating the previous draft is used for the next draft. This pulling direction based on the previously created draft appears only when you define it explicitly in the previous draft and not applied automatically due to the selection of the neutral element.      		  
    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. 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 further information about drafts, refer to Creating Basic Drafts and Creating Drafts with Parting Elements in Part Design documentation.