Hide Table of Contents

Weldments - Creating a Custom Profile

You can create your own weldment profiles 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 tab_Design_Library.gif. Under SolidWorks Content Open_in_SW.gif, 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.
  4. In the FeatureManager design tree, select Sketch1.
  5. Click File > Save As.
  6. In the dialog box:
    1. In Save in, browse to install_dir\lang\language\weldment profiles and select or create appropriate <standard> and <type> subfolders. See Weldments - File Location for Custom Profiles.
    2. In Save as type, select Lib Feat Part (*.sldlfp).
    3. Type a name for Filename.
    4. 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.

Provide feedback on this topic

SOLIDWORKS welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

Subject:   Feedback on Help Topics
Page:   Weldments - Creating a Custom Profile
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:


We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again

Web Help Content Version: SOLIDWORKS 2013 SP05

To disable Web help from within SOLIDWORKS and use local help instead, click Help > Use SOLIDWORKS Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.