When saving a sketch as a library feature part (.sldlfp file) to be used in the Structural Member function on the Weldments toolbar, it’s necessary to have the sketch selected (so it’s highlighted in the graphics area and has the blue box around it in the tree) when you go to Save as…sldlfp. That step is commonly over-looked. After saving the file the Sketch icon will have the green "L" on it if it was saved correctly.
If you've saved the profile sketch correctly and it shows the green L, check the folder you're pointing to at Tools > Options > System Options > File Locations > weldment profiles. Keep in mind that you need to have the correct number of sub-folder levels in this folder, and this will vary depending on whether or not you're using configurations in your weldment profile sketches. If you aren't using configurations, then your first level of sub-folders will appear in the Standard drop-down (such as ANSI and ISO), the second level will have sub-folders for the profile Types (HSS Square, Angle, Pipe, etc.), and these folders will contain the individual files (left screenshot below). If you are using configurations then the .sldlfp files will be in the Type folder and you'll choose the desired configuration from the Size drop-down (center screenshot below, HSS Square is the file name). I use both, so my .sldlfp files with configurations are in the same folder as the sub-folders containing the .sldlfp files that don't have configurations (the right screenshot shows the files in my ansi inch folder).