About Creating Draft Features

Drafts are defined on molded parts to make them easier to remove from molds. This section describes the various options used to create a draft.

The characteristic elements are:

• pulling direction: this direction corresponds to the reference from which the draft faces are defined.
• draft angle : this is the angle that the draft faces make with the pulling direction. The angle defined applies to all selected faces (several draft angle values cannot be created in one draft feature).
• parting element : this plane, face or surface cuts the part in two and each portion is drafted according to its previously defined direction. For an example, see Creating Drafts with Parting Elements.
• neutral element : this element defines a neutral curve on which the drafted face will lie. This element will remain the same during the draft. The neutral element and parting element may be the same element, as shown in Creating Drafts with Parting Elements.

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 section describes the operating mode to draft several faces using a pulling direction normal to the neutral element. It helps to facilitate your design.

If you need to draft , keep in mind the following operating mode that will facilitate your design:

• Click and first select the neutral element of your choice. The pulling direction that appears is then normal to the neutral element. Select the face that you want to draft and click OK to create your first draft.
• Now, to create the other drafts in the same 3D shape, note that by default the application uses the same pulling direction as the one specified for creating your first draft. As designers usually use a unique pulling direction, you do not need to redefine your pulling direction.

You can use the Deactivate and Extract Geometry commands to solve difficult drafting operations.

If you perform a difficult draft operation, for example resulting in twisted faces, you can use the Deactivate and Extract Geometry commands to solve your difficulties.

The Extract commands capability lets you generate separate elements from the initial geometry, without deleting the geometry.

When the application informs you via an error message window that your operation cannot be properly performed, closing the window displays a new dialog box providing you with a solution: you can deactivate the feature and extract its geometry.

After clicking Yes to confirm these operations, the feature appears as deactivated in the specification tree. A node Extracted Geometry (Feature.1) is displayed in the tree too.