I have to build a weldment using a square tubing (2"X2" X0.083") which is not on the solidworks structural members standard library. What is the way to add to library a new size for the tubing?
Welcome to the forum. I'm not surprised that that odd size isn't there. Do you already have .sldlfp files set up for tubing? If so, the simplest way would probably be to open an existing file that's close, edit the sketch to fit this profile, and Save as.. under a new name.
If not, I'm enclosing mine for 2 x 2 x 1/8. Open it up, edit the sketch, and save it with the new name in the location you have listed at Tools > Options > System Options > File Locations > Weldment Profiles. You probably already know this, but you need the correct number of sub-folders in the folder listed. For example, mine points to our network drive > SolidWorks > Weldment Profiles. Inside the Weldment Profiles folder, there are folders for ANSI and Metric, and in ANSI, there are folders for HSS Square, HSS Round, etc. with the files in these folders.
Let me know if this works okay, or if not let me know and we'll try again.
Thanks a lot for your prompt and very detailed answer, this was very helpful.
I'm glad I could help. And since you're a new forum member, here is a discussion with information to help you get the most out of it if you'd like to take a look: https://forum.solidworks.com/thread/39793.
By the way, if you ever need to save a new shape to your weldment profiles, it's pretty simple but won't work if it's not done right. Just start a new part, create your sketch on either of the main planes (keeping in mind that the origin will be the default insertion point when used with the Structural Shape function), close the sketch, click on the sketch in the tree to highlight it, and Save as... Library Feature Part (.sldlfp) in the proper folder. It's important that the sketch is highlighted when saving or it won't work. That's the step that throws people quite often.
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