How to Integrate the Surface World into Solid Modeling

This section discusses the different ways of integrating surface modeling into solid modeling.

Using Surface-based Features to Integrate Surface Modeling into Solid Modeling

Using surface-based features (Split , Thick Surface , Close Surface , Sew Surface ) is not a new way of integrating surfaces into solid modeling. However, what hybrid design changes is the fact that surfaces can now be included in the same body as the features they support. Here is an example of what you can now obtain:

In such a case, surfaces are necessarily defined prior to defining the feature. Indeed, this is because that the order principle inherent to hybrid design must be respected. If you modify these surfaces, the solid features located after the modifications will be affected by those modifications.

Using Boolean Operations to Integrate Volume Design Into Solid Design

You can use Boolean operations (Assemble , Intersect , Add , Remove )  to integrate volumes into bodies. Boolean features are the only features that can reference volumes.

This task shows you how to integrate a volume via an Intersection operation.
Open the HybridDesign.CATPart document.
  1. Select Insert > Boolean Operations > Intersect...
    The Intersect dialog appears.

  2. Select Volume Extrude.1. to create the intersection between the volume and the solid.

  3. Click OK to compute the result:
    The intersection is visible, and you can note that Intersect.1 has no children, it references Volume Extrude1. If you wish to, just use the Parents/Children command onto it to

Using Insert Added Volume to Integrate Volume Design into Solid Design

This task shows you how it is now possible to apply Part Design capabilities onto volumes created in Generative Shape Optimizer product. Prior to applying these capabilities, you need to perform just one operation as illustrated in this scenario.
To perform this scenario, create the volume of your choice.
  1. Select the extrude volume you have just created.

  2. Right-click and select the Volume Extrude.1 object-> Insert Added Volume... contextual command.

    The result is immediate. The Add.3 entity has been created. It contains a body on which you can apply Part Design capabilities.

  1. Now set Body.2 as the current object by using the Define in Work Object capability.

  2. For example, you can now chamfer the volume using the Part Design Chamfer capability .