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Weldments · Lesson 2

Custom weldment profiles

A weldment profile is just a fully defined sketch saved as a library feature part (.sldlfp) in the right folder. The folder names become the Standard and Type lists in Structural Member, the file name becomes the Size — or, in a configured profile, each configuration is a size. Add pierce points and properties once, and every member inherits them.

Kevin Walsh Kevin Walsh Updated Checked for SOLIDWORKS 2026
Rectangular tube profile sketch with pierce points and the folder tree standard, type and size

Where to find it

File → Save As → Lib Feat Part (*.sldlfp); Tools → Options → File Locations → Weldment Profiles

Folder structure

Profile type Folder → file
One size per file Profiles folder → Standard → Type → Size.sldlfp
Configured profile Profiles folder → Standard → Type.sldlfp, sizes as configurations

Configurations can be driven by a design table for many sizes. Ready-made standards (ANSI, AS, BSI, CISC, DIN, GB, JIS) download from the Design Library.

Step by step

  1. 1

    Sketch the section

    In a new part, on the Front plane, sketch a 40 × 20 rectangle centred on the origin with a 2 mm offset inside it (a rectangular tube wall). Fully define it and exit the sketch.

  2. 2

    Add pierce points

    Add sketch points at the corners and mid-sides of the outer rectangle. The origin is the default pierce point; the others can be picked with Locate Profile.

  3. 3

    Save as a library feature part

    Select the sketch in the tree, then File → Save As → Lib Feat Part (*.sldlfp). Name it 40 x 20 x 2.

    Save As dialog with file type Lib Feat Part sldlfp for a weldment profile sketch
    Save the selected sketch as a library feature part.
  4. 4

    Put it in the right folder

    Save into a folder tree like My Profiles\rect tube\40 x 20 x 2.sldlfp and add My Profiles' parent under File Locations → Weldment Profiles. Restart Structural Member and pick it.

Common mistakes

  • A folder one level too deep or too shallow — the tree must be profiles folder → standard → type → size.
  • Custom profiles inside the install folder — an update or uninstall can delete them.
  • Profiles stored on one PC only — others cannot rebuild models that use them; keep them in a shared folder.

Lesson 2 of 7 in the weldments course.

Practice

Save the 40 × 20 × 2 profile and use it for a new structural member. Check: Structural Member lists My Profiles → rect tube → 40 x 20 x 2, and Locate Profile offers your extra sketch points as pierce points.

Sources

Checked November 2026. SOLID WORKS Club is independent; menu names can differ slightly between releases.

Frequently asked questions

How do I create a custom weldment profile in SOLIDWORKS?

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Sketch the cross-section in a new part, select the sketch, and save it as a Lib Feat Part (.sldlfp) in a standard\type folder listed under File Locations → Weldment Profiles.

What is a configured profile?

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One .sldlfp in the Standard folder whose file name is the type and whose configurations are the sizes. Since 2021 the default profiles are configured.

How do I get the description into the cut list?

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Add custom properties such as Description and Material to the .sldlfp file. Members built from it pass them to the cut list.

Where are the default weldment profiles?

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In the folder shown under File Locations → Weldment Profiles; recent versions keep it under C:\ProgramData\SOLIDWORKS\SOLIDWORKS 20xx.