Weldments - Creating a Custom Profile

You can create your own weldment profiles (external link to YouTube.com) to use when creating weldment structural members. You create the profile as a library feature part, then file it in a defined location so it is available for selection.

Additional weldment profiles are available on the Design Library tab . Under SOLIDWORKS Content , in the Weldments folder, Ctrl + click items to download .zip files.

To create a weldment profile:

  1. Open a new part.
  2. Sketch a profile. Keep in mind that when you create a weldment structural member using the profile:
    • The origin of the sketch becomes the default pierce point.
    • You can select any vertex or sketch point in the sketch as an alternate pierce point.
  3. Close the sketch.
    In the case of multiple sketches, select the specific sketch from the FeatureManager design tree before you save it.
  4. Optional: If the Save As New dialog box appears, click Save to This PC.
  5. Click File > Publish.
  6. In the dialog box:
    1. In Save in, browse to install_dir\data\weldment profiles and select or create appropriate <standard> and <type> subfolders. See Weldments - File Location for Custom Profiles.
    If you cannot save the profile to the installation directory, you can save it locally by creating a subfolder structure. See Storing Custom Profiles in a Separate Folder Structure.
    1. In Save as type, select Lib Feat Part (*.sldlfp).
    2. Type a name for Filename.
    3. Click Save.
      The name that you give to the library feature part appears in the Size list in the Structural Member PropertyManager when you create a weldment structural member. For example, if you name the profile 1x1x.125.sldlfp, then 1x1x.125 appears in Size. If you name the part big.sldlfp, then big appears in Size.