How to Integrate the Surface World into Solid Modeling

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

You can integrate a volume via an Intersection operation.

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.

   Tip: Use the Parents/Children command it to check relationships.

   
   
   
   
   

   Note that the Boolean operation is updated according to the final operation performed on the input volume even if the ordered geometrical set is not aggregated to the parent body of the Boolean operation.

You can apply the 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.

   
   
   
   
   

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

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