Setting Draft Properties

You can assign draft properties to a feature in two ways:
  • By defining properties specific to the feature you are creating. These properties are available from a Draft tab included in the feature definition dialog box and are referred to as properties Intrinsic to feature. To see an example, refer to the task describing how to create a Boss.
  • The Draft Properties  command assigns draft properties to an active body of the Functional Features. The command requires the following three parameters:
    • 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.
    • Parting element: this plane, face or surface cuts the part in two and each portion is drafted according to its previously defined direction. From R16 onwards, you can select a sketch. When the sketch is selected, a GSD surface will be automatically built internally.
    • Parting radius:

Because some sub-elements of the part can be molded in different directions, there is no limitation on the number of Draft Properties features you can define in a functional body.

Open the Cutout.CATPart document.



  1. Click the Draft Properties icon .
    Note that it is not possible to set draft properties feature during the definition of a functional feature.
    The Draft Properties dialog box appears.

  2. Select a line or a plane to define the pulling direction.

    To define this type of parameter, we recommend no to use any edge supporting a functional specification.
    A red arrow indicates the pulling direction in the geometry area. By clicking on this arrow, you reverse the direction.

  3. Enter 2deg in the Draft angle field to edit the default angle value.

  4. Parting elements are optional. For the purpose of our scenario, select Extrude.1.

    Contextual commands available from the Parting element field let you create planes. These commands are:

    • Create Plane: for more information, see Creating Planes.

    • XY Plane: the XY plane of the current coordinate system origin (0,0,0) becomes the  parting element.

    • YZ Plane: the YZ plane of the current coordinate system origin (0,0,0) becomes the parting  element.

    • ZX Plane: the ZX plane of the current coordinate system origin (0,0,0) becomes the parting element.

    • Create Join: joins surfaces or curves. See Joining Surfaces or Curves.

    • Create Extrapol: extrapolates surface boundaries or curves. See Extrapolating Surfaces and Extrapolating Curves.

  5. Click OK to confirm the draft properties you defined.

    Draft Properties.X is added to the specification tree in the Solid Functional Set.X node.
    The blue graphics representation is located on the geometrical element used for defining the pulling direction, or the parting element or at the part's origin.

    This representation is associative with the geometry so when the parting element or direction is modified, the representation is updated.
  6. Draft Properties Versus Intrinsic to Feature

    The draft properties apply to all the features of the shellable body provided that these are not assigned the Intrinsic to feature option to define their draft behaviors. If that occurs, what you need to do then is just edit the features.  More precisely, click the Draft tab and change Intrinsic to feature to Draft Properties.x.

    For more information about defining draft properties specific to a feature, refer to the Reference Information.


Selecting Draft Property from another Solid Functional Set (SFS).

You can access the draft property which is defined in another solid functional set. All draft properties are displayed and can be selected for feature definition even though draft properties are defined in different solid functional sets. In our example below, Draft Properties.1 which is defined in the Solid Functional Set.1 can be accessed in Solid Functional Set.2 during the feature definition.


At the selection of Draft properties in the dialog all the draft properties located in the CATPart are displayed in the combo box and it can be selected for the feature definition.


You can replace Draft properties from one solid functional to another solid functional set.

When the feature which has draft properties associated with the definition, is copied and pasted in another document, then link to the draft properties is removed and the draft behavior is set to None.