solidworks - creating weldment library

Have you ever use standard components like frames, UNP profiles, etc.? To create arrangement of these bars is a simple thing to do in SW. Of course, basically this program has included several standard profiles.But the hard part will come when you need to arrange profiles that are not inside library. So..we must make our own library. I myself learned it just recently from a SW expert's website

Here's how you can do it:

1. Start a new part and start a new sketch

2. Give dimensions and fully constrain you sketch. (If the profile is complicated, you can make part, and then extract / convert the lines

3. Exit sketch and select the sketch from the Feature Manger Tree.

4. Keeping your sketch selected, go to File > Save as

5. Change the file type to Lib Feat part (*.sldlfp)

6. Go to location C:\Program Files\SolidWorks\data\weldment profiles\ and create you own folder or use the exiting folders. You can also set you own location and map the path in the File Locations. I have created a folder “MISUMI” and created another folder named “AlumExt” inside the test folder. SW will list the levels of the directory as Standard/Type/Size. In this case MISUMI is my standard, AlumExt is my type and size is the file name.

7. Give the file name as per your convenience. I have used "80x80" as the name

8. Your file will look like this. Check for the green coloured L and the symbol. This indicates that this file is a SW library file.

9. For checking that everything has been done perfect, open a new part and draw a line. Exit sketch and go to Insert > Weldments > Structural Member.

10. Select MISUMI as standard, AlumExt as type and 80x80 as size and then select the line. Select Ok.

Perfect. You can now make your own customized weldment profiles.