Problem

In SOLIDWORKS, one way to send someone an assembly without the internal components is to save the assembly as a part of the exterior faces only using File > Save As. However, it sometimes does not save all the surfaces, causing the saved part to have holes in it. This happens because of a limitation of the current algorithm for collecting faces. According to the SOLIDWORKS QA article QA00000107027, the algorithm looks at the model from 14 directions based on the faces and diagonals of a cube. Any face that does not occupy a pixel in at least one of those views is dropped, even if it is an exterior face.  

Solution

The workaround is to use the Defeature tool to defeature the assembly and then save that as a part, which is one of the recommendations from the SOLIDWORKS QA article, QA00000119695.

1. Open SOLIDWORKS and open the desired Assembly
2. Access Defeature from Tools > Defeature

3. In Defeature, use the Silhouette defeature method and hit the right arrow to continue

   

4. On the "Define Groups" page, create a group by selecting the outer components and choose a Simplification method to use. Note: A preview will be shown to the right and will update if the simplification method is changed or the setting "Enclose in one body" is turned on.

   

5. Once done creating and adjusting groups, click the right arrow to continue

6. On the "Defeature Complete" page, choose "Save as a new document" so a new part file is created of the defeature, and click the Green Checkmark

   

7. Give the file a name and choose where to save it

   

8. Open the new part file to review it. Then either use Save As to save the part file with only external faces if desired, or, if you are satisfied with how it looks, save the part file

For additional support, existing customers can submit a ticket or new customers can contact Hawk Ridge Systems.