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A few years ago I started creating plate using the Structural Member function instead of doing it with an Extruded Boss/Base. By doing this the cut list properties for Plate are generated automatically by the software just like they are for Square Tubing, Channel, W-sections, etc., which saves a great deal of time.  The sketch below is an example.



I have a different .sldlfp file for each common thickness, along with a few that I created for a specific project.



The widths are all 2", since it would be impractical to have a separate file for every possible width.  After using the feature I edit the sketch that's absorbed in the feature to match the width I want.  Since weldment sketches are copied when used for Structural Members and not linked you can edit the sketches in the Part without affecting the .sldlfp file.  The Description property is linked to the dimensions, so it will update to match the edit.



Occasionally I want the thickness or width driven by other features in the model, so in those cases I edit the sketch, make the dimension driven, and then use relations to fully define the sketch. (Deleting the dimension instead of making it driven would mess up the property.)


I attached one of my files.  If you like you can modify it to suit, or to use as a template to create other thicknesses.  As I said above, I just edit the sketch in the Part to get the desired width, but if you have a common size you use often I'd recommend making a .sldlfp file specifically for it so you won't need to edit the sketch in the Part.


You could of course create a single file with configurations if you prefer that workflow.


This technique also works well for other non-traditional shapes, like lumber, rebar, wire, etc.