Increasing Your SOLIDWORKS Weldment Profile Library

SOLIDWORKS provides a library of standard weldment profiles that can be used for structural members.  However, you also have the opportunity to download additional profiles or create your own.

Download Additional Weldment Structural Member Profiles

1. Open the Design Library tab in the Task Pane
2. Expand SOLIDWORKS Content and choose Weldments
3. Use Ctrl + click to download a zip file for each standard
4. Unzip the file to the same folder as your default weldment profiles (<install_dir>\data\weldment profiles) or add a new folder location to your File Locations option (Tools > Options > System Options tab > File Locations > Weldment Profiles drop-down menu)

Create Custom Weldment Structural Member Profiles

You can easily create your own profiles using a sketch.  The origin of the sketch will be the default pierce point.

1. 1. Start a new part and create a sketch on a plane
   2. Sketch your profile (any vertex or sketch point can be used as an alternate pierce point)
   3. Close the sketch

Create your Weldment Profile Sketch

1. Go to File > Properties and add a property “Description” with the Value as the description you would like in cutlist properties and the weldment cutlist table
2. Select Sketch1 in the design tree
   

   Add a Description Custom Property

3. Click File > Save As
4. Select Lib Feat Part (*.sldlfp) as the Save As type
5. Browse to the location of your default weldment profiles and select or create appropriate Standard and Type subfolders
6. Enter a filename and click Save (the filename is what appears as the Size when creating the structural member)
7. Now you will be able to access your custom profile when creating a weldment structural member

Save As a Library Part

Structural Member created

Cutlist Properties with Description