First check when you have structural members: Options \ File locations. From the dropdown list select Wledment profiles.
Go in Windows Explorer to this folder, next to the Standard and Type folder.
Copy and paste some Weldment profile and change its name
Open this profile in SolidWorks by dragging to the upper SolidWorks bar (if something is open in SW). If not, you can drag it to graphics area.
Modify sketch dimension
Go to the file properties and modify Description
Save and you can use it
You can also go to the right Task pane, to Design Library tab, expand SolidWorks Contend, and then select Weldments. With CTRL key you can download almost full Standard.
After unzipping it move this folder to the location that is set in SolidWorks.
so much tanks it helps me a loooott thnak you
This is definitely the way to do it.
Just wanted to mention that with configuration support for weldment library features being added in a previous release (2014... I think) it is very handy to create configurations of your profiles instead of individual files. When changing between sizes etc. you won't get as many mate conflicts. The only reason why I took the time to build a configured profile library was because I use weldments a lot. If I didn't I would have just used to supplied individual profiles.
Hope this helps,
Another thing to remember is that you can edit the profile sketch. Just find it in the feature tree, right click on it and select edit sketch.
This doesn't change the profile in the weldment library, but is useful for one-off profiles, or for adding a point to locate the profile someplace besides the default corners and centerpoints.
Also, if you are making custom profiles for your library as described above by Wojciech, and get the message that you do not have privileges to save to the weldments folder, try saving to the desktop and then copy and paste into the correct folder. I don't know why I'm allowed to paste something into a folder that I can't save to, but. . .
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