One of my favorite tools in SolidWorks is the Delete Face command. It probably has too many uses for me to list them all here but what I use them for mainly is surface reconstruction in SolidWorks native files and feature removal in imported files (files with NO feature tree).
In this tip, I wanted to show a little trick I learned recently while preparing some CAD data for FEA analysis. Sometimes, small features are removed for FEA analysis in order to simplify the meshing process. In this particular part to the left, the two circular cut features needed to be removed. This is a perfect 
application for the Delete Face command with the “Delete and Patch” option selected. After selecting only the faces that were part of the circular feature, the Delete Face command was invoked only to get a warning message that the faces could not be patched due to a “geometry condition”. Sometimes you run into this when the geometry of the features you would like to remove is too much for SolidWorks to handle.
To simplify the faces being removed, a rectangular cut was added which removed 
the two circular features completely thus creating a larger, yet more simple cut. The Delete Face command was then applied to the three faces left by the rectangular cut and the feature was removed (and seamlessly patched) successfully!
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thanks
Dave
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First and foremost, thank you for asking the question.
With a feature like this I can think of 3 common situations in modeling where the use as I have shown it would be beneficial. (I'm sure there are more, but these are the three that popped into my head :-))
The first situation would be where you have an imported model that has no features. Your entire solid model comes in as a single imported feature so you don’t have the luxury to delete any individual feature.
The second situation would be where you are looking at a feature that may have multiple references further down the feature tree. To remove or suppress this feature would result in the suppression of additional features. You could remove the relationships and proceed with deletion of the feature but in some cases the removal of this geometry might be temporary, (like for FEA analysis) so it is sometimes easiest to handle it down at the bottom of the feature tree using Delete Face without having to modify multiple features.
The third situation deals with instances where you design multiple parts using the multi-body functions in a single part file. If you are designing a plastic housing assembly it can be advantageous to use this method if the geometry of one “half” need to have curvature continuity or share features with the other “half”. For use in assemblies the Split Part command can be used to separate the multiple bodies into individual part files. In cases like this the separated part files of the case halves will not have individual features. It will have a “Stock part” feature that ties it parametrically to the multibody master file. If you need to use this individual part externally for FEA analysis or export to another system, you can remove features with the delete face command without having to mess with the original geometry. Again, in this situation this would be for temporary changes.
For situations 2 & 3 if the removal of the feature is permanent, I would remove the feature altogether by deleting the feature.
I hope this makes sense to you. If it doesn’t, let me know and I can elaborate more.
Thanks for the comment and thanks for reading my blog!
Best Regards,
Ricky Jordan
http://www.rickyjordan.com
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