Cavity Extraction

In this task, you are going to use the Cavity Extraction command to create a Cavity Extraction feature. The Cavity Extraction feature will be placed into a new body, and will reference an existing body (the source Body). The Cavity feature creates a protected volume, so to visualize the geometry a Cavity shape feature will be created in the new Body.

The Cavity Extraction feature produces geometry useful in defining a cavity plate for molding the source Body. The output is associative, meaning if the source Body changes, the Cavity Extraction geometry will automatically change.

The output geometry includes the Cavity, Added, and Protected volumes, as well as the unshelled portions of the Shellable volumes. Features can be excluded, and an optional Extraction Properties feature can be used to omit Protected volumes.

Open the CavityExtraction1.CATPart document.



  1. Click on the Cavity Extraction  icon .The Cavity Extraction dialog box is displayed. Select Body.1 as the Source Body.

  2. Click on the Extract behavior list and select Extraction Properties.1.

  3. Click OK to confirm

  4. Click on the External Feature icon . Select Sketch.7 as the Profile/Surface. Click the Reverse direction button. Set the First Length to 100.  


  6. Click OK to confirm.

  7. Right-click on Body.1 and select Hide/Show from the contextual menu.

  8. Right-click on PartBody and select Hide/Show from the contextual menu.

When you create a Cavity Extraction selecting a Body as Source body on a part which has multiple added/removed bodies or assembled bodies, in this example, the extraction will be generated on the Body (in this case, Solid Functional Set.1) in the first position of the selected Body.

  1. Here is a simple part with two bodies assembled together to illustrate the Cavity Extraction operation.

  2. Create a Cavity Extraction selecting "PartBody" as Source Body as below.

  3. The Protected Extracted Cavity is created on Body1 (Solid Functional Set.1) only as shown below.