How to Create SOLIDWORKS Custom Weldment Profiles – Hawk Ridge Systems Support

weldment example

When using the Weldment tool, SOLIDWORKS installation comes with a default set of weldment profiles that can be selected in their default location. You can also download additional weldment profiles from SOLIDWORKS Content.

What if you need a profile that does not exist in the files provided by SOLIDWORKS? You can create a custom profile, starting from a sketch that meets the standards or specifications you need and saving it out as a Lib Feat Part to use in your weldment design process.

Weldment Profiles File Location

Before you create your own weldment custom files, it's important to first determine where you are saving the profiles. You can save it at where the default profiles are located or at any location as desired.

With SOLIDWORKS opened, go to Tools > Options > System Options > File Locations > Show folders for "Weldment Profiles"
Browse to the location that is listed through your File Explorer. Click on the empty space in the file path to select it and copy the full path. Keep a record of this full path to make saving the custom weldment profile in the later steps easier.
If the location listed in the File Locations in SOLIDWORKS is not where you want to put the weldment profile locations, create a "custom weldment profiles" folder at where you desire through the File Explorer. For example, in your Documents
Click the "Add" button in File Locations
In the "Select Folder" dialog box, browse to the "weldment profiles" folder you have created and select it. Click the "Select Folder" button at the bottom righthand corner of the dialog box
The path to the folder will be added to the Weldment Profiles Folders list

Weldment Folder Structure

Now that we have let SOLIDWORKS recognize where to find the weldment profile, we need to understand there are two ways that weldment profiles can be organized in terms of file structure inside of the file explorer. Note that there are three fields that need to be selected before you can select a sketch and create a structural member: Standard, Type, and Size

First Way - Saving out a .sldlfp file with multiple configurations to represent various sizes

In this case, the .sldlfp file is directly placed inside of the Standard folder. The file itself represents the Type, and its various Size options is made through various configurations.

sldlfp file needs to be placed inside of the Standard folder (only one folder deep from the weldment profiles folder)

Second Way - Saving out a .sldlfp file as a file that represents one size only

In this case, the .sldlfp file is placed of a folder that is named for its Type, which is placed inside of a Standard folder. The .sldlfp file contains one size of the Type it's under.

sldlfp file needs to be placed inside of the Type folder, which is inside of the Standard (two folders deep from the weldment profiles folder)

Making and Saving Custom Profiles

We will now start making the actual sketch for the custom weldment profile.

Open a new, empty part
Start sketching on any of the default planes and fully define it, as fitted to the specifications you need. Exit out of the Sketch tool
Add more configurations and configure the sketch dimensions as needed, if you are going for structuring your folder with the First Way listed in the Weldment Folder Structure section. In this example, I'm making one size per part.
After the sketch has been set up, we will now save it out. You must select the sketch before we save this out as a profile part
After the sketch is selected, go to File > Save As
In the Save As dialog box, change the Save as type to "Lib Feat Part"
Brose to the location that that you are pointing to for Weldment profiles and create the folder structure accordingly to the folder structure you have chosen. Save the file in the right folder
Your sketch should now have a L icon in the FeatureTree
Now you would be able to use this profile for Weldment