Problem

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

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

Step 1: Weldment Profiles File Location

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

1. With SOLIDWORKS opened, go to Tools > Options > System Options > File Locations > Show folders for "Weldment Profiles"

   

2. Browse to the location that is listed through the Windows 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. 

   

3. If the location listed in the File Locations in SOLIDWORKS is not where we want to put the weldment profile locations, we can create a "custom weldment profiles" folder where desired through the Windows File Explorer, such as in the Documents folder.

4. Click the "Add" button in File Locations

   

5. In the "Select Folder" dialog box, browse to the "weldment profiles" folder we have created and select it.
6. Click the "Select Folder" button at the bottom right-hand corner of the dialog box

7. The path to the folder will be added to the Weldment Profiles Folders list

   

Step 2: Weldment Folder Structure

Now that we have let SOLIDWORKS recognize where to find the weldment profile, we need to understand that 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 we can select a sketch and create a structural member: Standard, Type, and Size.

The first way is to save a .sldlfp file with multiple configurations to represent various sizes. In this case, the .sldlfp file is directly placed inside the Standard folder. The file itself represents the Type, and its various Size options are made through various configurations. 

The second way is to save out a .sldlfp file as a file that represents one size only. In this case, the .sldlfp file is placed in a folder that is named for its Type, which is placed inside a Standard folder. The .sldlfp file contains one size of the Type it's under. 

Step 3: Making and Saving Custom Profiles

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

1. Open a new, empty part
2. Start sketching on any of the default planes and fully define it, as fitted to the specifications needed, then exit out of the Sketch tool
3. Add more configurations and configure the sketch dimensions as needed, if we are going for structuring the folder with the First Way listed in the Weldment Folder Structure section. In this example, we are making one size per part.

4. After the sketch has been set up, we will now save it out.  Note: We must select the sketch before we save this out as a profile part file

   

5. After the sketch is selected, go to File > Save As

6. In the Save As dialog box, change the Save as type to "Lib Feat Part"

   

7. Browse to the location of the weldment profiles folder and create the folder structure according to the desired folder structure, and save the file in the right folder

   

8. The sketch should now have an "L" icon in the FeatureTree

9. Now we can use the new custom weldment

   

   For additional support, existing customers can submit a ticket or new customers can contact Hawk Ridge Systems.