Creating a Mating Flange

This command is only available with the Automotive Body in White Templates product.

This task shows how to create a mating flange, in order to add a shape to a part.
This shape is a surface and can be used as a contact zone with another part in an assembly purpose.

1. Click Mating Flange .

   The Mating Flange Definition dialog box is displayed.

2. Select the Base surface.
   It can have several faces and internal sharp edges.

3. Select a Reference element to position the mating flange on the base surface.

   It can be: a plane or a surface. The reference location is computed as an intersection with the base surface. a curve (as in our scenario): the curve can be either a 3D curve or a planar curve and must have a projection on the base surface along the reference direction. We advise you not to use the intersection or projection curve but rather the input surface or curve.

4. Select a Reference direction. The reference location is a curve computed as a projection along the direction.

   	To select a default reference direction, right-click in the field and choose the Default Selection contextual item. Conversely, to clear the selection, right-click in the field and choose the Clear Selection contextual item. If a direction is selected, both Default Selection and Clear Selection items are available from the contextual menu. If a plane or a surface is selected as a Reference element then Reference direction field will be disabled, as reference location is computed as an intersection of that plane with base surface. In this case OK and Preview are available.
   	The intersection or the projection curve must be long enough to join the base surface boundaries.
   The mating flange reference location feature is created in hidden mode and is temporarily shown during edition.

5. Define the mating flange parameters by clicking the value to edit in the dialog box or by clicking the manipulators in the 3D geometry.

   Width Margin Wrap

6. Click Preview.

7. Define the thickness:

   Default thickness: is generally the part thickness and is used as the default offset value. You can define its value either by entering a value in the field or using the manipulators in the 3D geometry. Local thickness: enables you to define multiple thickness values. They replace the default value and can be positive, negative, or null. Select a sub-part of the reference curve and define its value either by entering a value in the field or using the manipulators in the 3D geometry. This thickness value applies to all surfaces on which the curve lies as well as connex surfaces that are tangent continuous. You can select several sub-parts, each one having its own local thickness. For each value, a corresponding 3D dimension is created in the 3D geometry and can be edited by double-clicking it. In case no local value is defined, the Local thickness field is grayed out. Otherwise, the corresponding sub-part and the 3D dimension are highlighted in the 3D geometry. If you select the highlighted sub-part, the local value is deleted and the default thickness value is used.

   The thickness that is aggregated under the mating flange feature is the default thickness.

8. Click OK to create the mating flange.

   The new shape (identified as Mating Flange.xxx) is added to the specification tree. Its reference location is aggregated under the Mating Flange feature and can be used as an input for a further operation.

   Check No trim if you do not want the base surface to be modified. Check Trim to trim the base surface with the mating flange. Check Trim and Split to trim the base surface with the mating flange and create an additional feature that corresponds to the base surface split by the reference element. The Split feature is aggregated under the Mating Flange feature. Click Reverse Direction to inverse the thickness direction, according to the orientation of the reference element. As as consequence, the mating shape is displayed on the other side of the base surface. Click Flip Flange to inverse the mating flange direction, according to its orientation. As as consequence, the mating shape is displayed on the other side of the reference location. Check Both sides to create a both-side mating flange using a second reference element. By default, the Reference element, as well as the second Reference direction, are the same as the first reference element and direction, but you can choose other ones. Similarly to the first Reference direction, contextual menu items (Default Selection and Clear Selection) are available for the second Reference direction. With the same reference element With a second reference element     The second reference location is aggregated under the Mating Flange feature and can be used as an input for a further operation. This option is available with Trim and Split, providing the reference elements are different. In this case, the portion between the two elements is kept. Flip Flange is grayed out when Both sides is activated. Check Linked directions to link the second reference direction to the first one. Both directions are the same, the second Reference direction field is grayed out and filled with the same value as the first Reference direction field. This option is automatically checked if Both sides is checked. If Both sides is unchecked, it is grayed out. Check Deviation to specify an individual deviation value. This can be needed, for example, if unwanted tiny edges are created because the default deviation tolerance is too small. In these cases, you can increase the deviation value until the tiny edges are removed. By default, the deviation tolerance set in the Maximum Deviation box in Tools > Options > Generative Shape Design > General tab is used. Also, the default deviation value used depends on the design range settings. Tiny Edge Created with a Swept Surface as Input Element Tiny Edge Removed by Increasing Deviation

You can now create a mating flange on a part of the base surface that contains a hole simply by setting the Default thickness to 0mm.
 

Mating flange created on a surface with a hole by setting the default thickness to 0mm.