We will look at possible reasons why you cannot see your custom weldment profile as a structural member.
Reasons:
1) File structure is incorrect.
2) Profile is not properly saved as a library feature part.
3) File location for custom weldment profiles aren't assigned
First we need to understand the file references for a structural member:
Standard/File: The file you create with your standard or name for your folder ie. Custom profiles.
Profile: The sketch profile you created.
Configuration: The configuration you created within your profile sketch.
1) File structure is incorrect.
The file structure for weldment profiles are CRITICAL. If the File structure is incorrect, the weldment profile will not show under structural members.
The file structure needs 2x Folders before the library part is assigned. Configurations are also needed for the structural member to show the weldment profile.
The first of the 2 folders would be the folder that you would assign in SOLIDWORKS file locations.
An example of a file structure would be as follows:
Weldment Profiles (assigned folder) > Custom profiles (standard/file folder) >
Flat bar (Library part with more than one configuration, not adding extra configurations would result in the library part not working)
2) Profile is not properly saved as a library feature part.
If the profile is not saved as a library feature part (.sldlfp), it will not show in the structural members for weldment.
How to save a custom profile:
1) Draw your desired profile.
2) Right click on your sketch and navigate to "Configure Feature".
3) Add more configurations to your sketch.
4) Click on you sketch and click File>Save As... (Be sure to click on your sketch before you click on "Save As", or else the file will not be saved as a library feature, the sketch should be highlighted).
5) Save the part in the desired location as a Lib Feat Part (*.sldlfp). (Refer to "File structure is incorrect" mentioned earlier in the article, to make sure to use the correct file structure).
6) If these steps were followed correctly, an "L" should appear over sketch icon as seen below. If this does not appear, the file was not correctly saved.
You can now close your profile and should be able to access it within the structural members feature.
3) File location for custom weldment profiles aren't assigned.
When using custom weldment profiles with an external folder(recommended), one needs to assign the folder within the file locations for SOLIDWORKS weldments.
To locate the files follow the following steps:
1) Navigate to the options.
2) Under system options navigate to "File locations"
3) Drop down the "Show folders for" menu and navigate to "Weldment Profiles".
4) Click on "Add..."
5) Locate your custom folder (be sure to select the correct folder as seen above in "File structure is incorrect") and click on select folder.
6) Click "OK" to finish adding your file location.
7) Click "Yes" on the pop-up dialog box stating "Would you like to make the following changes to your search paths?"
Your file is now located and you should be able to access your custom profile within the structural members feature.
Date published: 03/06/2022