Creating Advanced Drafts  

The Advanced Draft command lets you draft basic parts or parts with reflect lines but it also lets you specify two different angle values for drafting  complex parts. 

This task shows you how to draft two faces with reflect lines, and this by specifying two different angle values and by using both modes available.
We recommend the use of this command to users already familiar with draft capabilities.

Open the Draft4.CATPart document.

  1. Select View > Toolbars > Advanced Dress-Up Features to access the Advanced Dress-Up toolbar.

  2. Click Advanced Draft .
    The Draft Definition (Advanced) dialog box is displayed and you can see a default pulling direction (xy plane) in the geometry.

  1. Specify that you wish to draft two faces with reflect lines by clicking both icons as shown:
    Note that two modes are available :

    • Independent: you need to specify two angle values.

    • Driving/Driven: the angle value you specify for one face affects the angle value of the second face.
If you have a Cast and Forged Part Optimizer license, the Fitted option is also available. This option lets you perform a draft operation on two opposite sides of the part while adjusting the resulting faces on the parting element you chose.
  For the purposes of our scenario, ensure that the Independent option is on.

The icon available after the Faces to draft field lets you edit the list of the faces to be drafted. For more information about that capability, refer to Editing a List of Elements.

Neutral Element

  1. In the Neutral Element frame, click No Selection and select the fillet as shown. 
 

Pulling Direction

Contextual commands creating the reference elements you need are available from the Selection field:

  • Create Line: For more information, see Creating Lines.
  • Create Plane: see Creating Planes.
  • X Axis: the X axis of the current coordinate system origin (0,0,0) becomes the direction.
  • Y Axis: the Y axis of the current coordinate system origin (0,0,0) becomes the direction.
  • Z Axis: the Z axis of the current coordinate system origin (0,0,0) becomes the direction.

If you create any of these elements, the application then displays the corresponding icon next to the Selection field. Clicking this icon enables you to edit the element.

  1. In the Pulling Direction frame, click Pulling Direction in the Selection field and select the part's bottom face to specify a new pulling direction.

  2. Enter 10 as the angle value.

Parting Element

  1. Click the Parting Element tab to define the parting element.

  2. Check the Use parting element option and select the green surface as the parting element.
    The Parting Line Adjustment option adjusts the smoothness of the transition zone on the draft surface. A transition zone occurs when a neutral element that was driving becomes driven, or vice versa. A zero parting line adjustment would yield a sharp edge on the draft surface. Usually, the default value (0.1mm) proves to be efficient most of the time. For more information, refer to More about the Parting Line Adjustment Option.

  3. Click the 2nd Side tab to define the second face to be drafted.

  4. In the Neutral Element frame, click No Selection from the combo list and select the second fillet.

    Both faces to be drafted are now selected. The application displays the reflect line in pink.

  5. Enter 6 as the angle value.

  6. Click OK to confirm.
    Both faces are drafted using a distinct angle value, as specified.
  Due to the use of the angle values you have set, this operation results in a "step" where both drafted faces meet. To avoid such a result, you can use the Driving/Driven option as explained hereafter.

Using the Driving/Driven Option

  1. Double-click Draft.1 in the specification tree to edit it.
    The Advanced Draft dialog box appears.

  2. Set the Driving/Driven option. You can note that the Driving side option is checked, meaning that the angle value you specified for the first face you selected (10 degrees) is the driving value.

  3. If you click the 2nd Side tab, you can notice that the angle value field is no longer available.
    In concrete terms, the application will compute the value for the second face so as to avoid the "step effect".

  4. Click OK to confirm the operation.
    The application has adjusted the second drafted face.
  • If you prefer to set the angle value you specified for the second face you selected (6 degrees) as the driving value, just click the 2nd Side tab and check Driving side.
  • Sometimes, some resulting faces of the "Driven draft" are not apt for being removed from molds. In this case, we recommend you to check this using the Draft Analysis capability.

More about the Parting Line Adjustment Option

You will use the Parting Line Adjustment option to ensure that later on you will be able to apply machining techniques onto the part. To illustrate that option, let's consider the part we used in the scenario.

  1. Set the Fitted option.
    This option lets you perform a draft operation on two opposite sides of the part while adjusting the resulting faces on the parting element you chose.

  2. Keep 0.1mm as the parting line adjustment value, and enter 17 degrees to change the draft angle value you previously set to the draft.
    This excessive value does not reflect angle values designers usually use, but this lets us quickly see what happens next. You obtain a draft which is not satisfactory. As indicated by the arrow, the curvature radius would invalid any machining process because it is too small:

  3. If you click Top View from the View toolbar, the curvature radius causing trouble for being too small, becomes more visible, as pointed to by the arrow:

  4. Now, changing the parting line adjustment value to 0.7 mm would add material up to the curve pointed to by the arrow. Consequently, the curvature radius would be more acceptable.

  5. Changing the parting line adjustment value to 0.9mm would let you obtain an even larger curvature radius:

     

    Concretely speaking, when setting the parting line adjustment parameter, you define a length value that sets a maximum thickness to be added to the draft to enlarge the wrong curvature radius. As illustrated in the case just above, that length is represented by L. The chosen value is 0.9mm, which means that L might be 0.9mm or even a little bit less.
    Considering the rest of the curvatures of the draft feature, depending on the part shape, that thickness will most often be thinner, but will never exceed the value you entered.

    Methodology

    This option thus adds material to the part. If then you decide to use it, you should keep in mind that you need to enter reasonable values not to add too much material prior to machining processes. Usually, 0.1mm set as the default value provided by the application, proves to be efficient most of the time.

    Concerning draft angle values, again make sure the value you enter does not add too much material. In the worst cases, this would prevent you from removing parts from molds.

    In other words, a successful draft operation requires a fine tuning between the draft angle value you set and the parting line adjustment you may perform. The challenge being to add the minimum material to the part.

    Useful Tools

    Remember that you can always check curvatures by performing Surface Curvature Analyses and draft validity by using the Draft Analysis capability.