How to Delete Faces in SOLIDWORKS
One of the most powerful and often surprisingly overlooked SOLIDWORKS features is Delete Face. This simple feature can be used to remove nearly any type of unwanted geometry, such as fillets, holes, ribs, bosses, or even imported model objects. This all-in-one feature not only removes the unwanted geometry, but it can also patch and trim the remaining faces as if the original unwanted geometry never existed.
Delete Face works with any native SOLIDWORKS feature as well as imported geometry. Imported geometry lacks a feature history, so modifying or deleting features is not possible. Delete Face can easily directly edit imported files as if they were designed in SOLIDWORKS.
Where to find the SOLIDWORKS Delete Face feature
Delete Face can be found in several locations:
- Direct Editing tab of the CommandManager
- Surfaces toolbar
- Insert > Face > Delete
- Or a simple right-click on a face and selecting Delete in the menu
- Direct Editing tab of the CommandManager
How does Delete Face work?
Once the feature is accessed, there are three options:
Delete – Deletes a face from a surface body or deletes one or more faces from a solid body to create surfaces. This option will simply delete the face(s) and leave an open hole in the model. Choosing this option will also convert a solid body into an open surface body, since the solid no longer has all the faces to close the geometry. The edges of the hole will be displayed in blue indicating they are open edges of a surface body. More features will be required to manually patch the hole(s) left by the missing geometry to complete the surface and make it a solid again. This is a useful option in some cases where the geometry is too complex for SOLIDWORKS to patch automatically when using the next option, Delete and Patch.
Delete and Patch – Deletes a face from a surface body or solid body and automatically patches and trims the body. This is the preferred option. This option attempts to remove all the selected faces and automatically patch up and trim the remaining faces as if the geometry never existed. This option can be used to cleanly remove many different types of unwanted geometry like fillets, chamfers, holes, bosses, etc. If the geometry is too complex to patch automatically, then this option may fail with an associated error or warning. In this case, the Delete option above can be used along with additional surface features to turn the model back into a solid.
Delete and Fill – Deletes faces and generates a single face to close any gap. This is the least used of the three options. This option will remove the selected faces and generate a single unbroken smoothed face to close any gap. The user doesn’t have any control over the shape of the face that’s created. This option may require more advanced surface knowledge to check curvature, etc. in order to verify the solution matches your design intent.
Once complete, an associated feature will be added to the SOLIDWORKS FeatureManager Design Tree. This feature can be edited or suppressed just like any other SOLIDWORKS feature.
Using Delete Face to Remove Geometry
The examples below depict the before and after results of using Delete Face with the Delete and Patch option. The Delete and Delete and Fill options are not represented since Delete leaves an open hole that requires additional features to complete and Delete and Fill also requires advanced surface knowledge to check curvature, etc. to verify the solution matches your design intent.
Delete Fillets and Chamfers to produce sharp corners
Delete Face can be useful to remove fillets and patch/trim geometry back to sharp corners. This is extremely useful for imported models where the size of fillets needs to be changed or simplified.
Here is an example where a chamfer needs to be removed to restore sharp edges.
Delete Holes
Selecting all faces associated to the holes (don’t forget the faces at the bottom of blind holes!) will completely remove and patch the holes as if they never existed.
Delete Bosses
Selecting all faces of a boss will completely remove that feature, leaving a smooth face in its place as if the boss never existed.
Learn more in SOLIDWORKS Advanced Part and Surfacing Training
MLC CAD Systems offers a wide variety of SOLIDWORKS training sessions both in-person and remotely. You can learn how to apply many advanced tools and techniques, such as Delete Face, to help become more proficient in SOLIDWORKS. Visit our training site to learn more about SOLIDWORKS Advanced Part Modeling and SOLIDWORKS Surface Modeling to review the course agenda and sign up for a class!
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