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How to Create SOLIDWORKS Custom Weldment Profiles

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.

  1. With SOLIDWORKS opened, go to Tools > Options > System Options > File Locations > Show folders for "Weldment Profiles"tools options system options show folders weldment profiles
  2. 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. shows where to click; empty space after the path
  3. 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
  4. Click the "Add" button in File Locationsthe add button in the file location dialog box is highlighted
  5. 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
  6. The path to the folder will be added to the Weldment Profiles Folders listshows an additional path has been added to the folder box

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.

  1. Open a new, empty part
  2. 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
  3. 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.
  4. 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 partsketch feature is selected/highlighted in the FeatureTree
  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"shows the locaiton of the save as type dropdown menu
  7. 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 folderfile explorer has been browsed to the location of the weldment profiles folder, and is inside of type and standard folder
  8. Your sketch should now have a L icon in the FeatureTreethe sketch picture in the FeatureTree now has a L icon
  9. Now you would be able to use this profile for Weldmentthis shows the Standard, Type, and Size fileds in the Structural Member's PropertyManager has been filled out. The sketch has been selected in the viewport and the member is correctly previewed.

Contact Us

For further technical support, please contact Hawk Ridge Systems at 877.266.4469 for the U.S. or 866.587.6803 for Canada.

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