ASSEMBLY/WELDMENT

Go to McMaster.com

Search 8020

Find a 1.5"x1.5" regular member (as shown below)

Download the SolidWorks file from the product details page

Open the downloaded part

Create a sketch on one of the end-faces

Use convert-entities to grab all of the edges into the sketch

Select all of those entities

Copy (CTRL+C) the entities

Create a new part (this step may be optional)

1. Create a new sketch

2. Paste (CTRL+V) the selected entities

3. If they are not centered, use Move Entities to locate the circle centered on the origin

4. Exit the Sketch

Select the sketch from the Feature Manager Design Tree

Click File→Save As→Library Feat Part

Navigate to the weldments folder

1. C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\lang\english\weldment profiles\

2. If  yours is different, it may be found via Options→System Options→File Locations→Show Folders For→Weldment Profiles

Create a new folder (next to ANSI/ISO) named "CUSTOM"

Create a folder within "CUSTOM" named "1515"

Save your *.sldlfp as "15x15x8020.sldlfp"

This profile may now be found using the Structural Member Feature on the Weldments Tab