What Is a Weldment Profile in SOLIDWORKS?

A weldment profile is a predefined 2D sketch saved as a Library Feature Part (.SLDLFP). It is applied along sketch paths using the Structural Member tool to generate welded structures quickly and accurately.

Default File Location for Weldment Profiles

SOLIDWORKS stores weldment profiles in a predefined system directory.

How to Find the Weldment Profile Location

1. Go to Tools → Options

2. Select System Options

3. Choose File Locations

4. From the drop-down, select Weldment Profiles

Default Path (Example)

 

C:\ProgramData\SOLIDWORKS\SOLIDWORKS 2025\Weldment Profiles


You can:

• Store your custom weldment profiles in this default folder, or

• Maintain a separate custom folder and add its path in System Options → File Locations

Either method will make the profiles available in the Structural Member feature.

Weldment Profile Folder Structure Explained

SOLIDWORKS recognizes two common weldment profile structures:

1. Single SLDLFP with Multiple Sizes

• One .SLDLFP file

• Multiple configurations, each representing a different size

2. One SLDLFP per Size

• Each .SLDLFP file represents only one profile size

• Easier to manage for non-standard or custom shapes

Recommended for custom profiles: One file per size for clarity and control.

How to Create a Custom Weldment Profile in SOLIDWORKS

Step 1: Design the Custom Shape

1. Open a new Part file

2. Create a 2D sketch on any default plane

3. Fully define the sketch

4. Ensure the sketch represents the cross-section of the weldment

Tip: Place the sketch origin logically, as it controls profile alignment.

Step 2: Save as Library Feature Part (.SLDLFP)

Weldment profiles must be saved as Library Feature Parts, not standard part files.

Steps:

1. Select the sketch in the FeatureManager

2. Go to File → Save As

3. Choose Library Feature Part (*.sldlfp)

4. Select your weldment profile folder

5. When prompted, click No (do not convert to a feature)

Important: Selecting the sketch before saving ensures it is recognized as the profile reference.

After saving:

• The part icon changes to a Library Feature bookmark

• The profile becomes available in the Structural Member tool

Using the Custom Weldment Profile

1. Activate Weldments

2. Open Structural Member

3. Select:

   • Standard (folder name)

   • Type (subfolder)

   • Profile (your custom .SLDLFP)

4. Apply it to sketch segments

Your custom profile now behaves like any standard SOLIDWORKS weldment profile.

Best Practices for Custom Weldment Profiles

• Use clear folder naming conventions

• Keep profiles fully defined

• Avoid unnecessary sketches or features

• Maintain separate folders for company standards

• Back up custom profile libraries regularly

Conclusion

Customizing non-standard weldment profiles in SOLIDWORKS allows you to model real-world fabricated structures with precision. By understanding the correct file location, folder structure, and Library Feature workflow, you can efficiently create reusable profiles and streamline your weldment design process.

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An Elite Application Engineer, with a strong emphasis on cultivating long-term relationships and driving customer success. And, plays a pivotal role in ensuring clients derive maximum value from their SOLIDWORKS solutions, specializing in personalized support during PDM implementation projects, combines years of industry experience to provide expert guidance. Recognized as a go-to expert in technical support and customer success, focuses on helping clients optimize their use of SOLIDWORKS CAD, SOLIDWORKS PDM (Product Data Management), and the robust 3DEXPERIENCE platform, enabling businesses to streamline their processes and enhance their product development workflows.