When working in SOLIDWORKS, most users spend the majority of their time creating parts and assemblies using standard features. However, there is a tool that often goes underutilized—Weldments. Weldments provide a faster, more structured way to create frames, welded structures and fabrications. They also streamline documentation by generating cut lists and supporting additional fabrication features like gussets, end caps and weld beads.
This article will walk through what weldments are, how to use them effectively, and how to create your own custom profiles. By the end, you will be able to confidently set up and use weldments for both standard and company-specific designs.
What is a Weldment in SOLIDWORKS?
A weldment is a single part file that contains a welded structure, usually made from structural profiles such as tubes, angles or beams. Instead of modelling each beam individually, weldments allow you to define profiles along a sketch, letting SOLIDWORKS handle trimming and corner conditions automatically.
As with most features in SOLIDWORKS there are some questions you might have.
First off, where are weldments applicable? Weldments are not useable in all your models, but some applications include:
- Machine frames and support structures.
- Railings, ladders, and stairs.
- Workbenches and tables.
- Steel fabrications in construction and manufacturing.
The next question you may ask is, why use weldments when you can just create the components as separate parts or as configurations?
For me, the primary answer is consistency. Weldments allows you to create, use and reuse profiles for your company’s structures.
Another advantage is speed. With a sketch (2D or 3D) you can quickly create your structures, and with the automatic cut lists you can easily create the documentation needed for production.
And finally, flexibility. It is easy to either trim, extend or even replace the weldment profiles, in case of changes.
But enough about the why; let’s look at the how.
Basic Use of Weldments
Weldments is included in all SOLIDWORKS packages (Standard, Professional or Premium) and can be easily accessed in the weldment tab.
If it is not visible in your toolbar, right click on the CommandManager, select “Tabs” and select the weldment tab. Your weldments are now available.
Next let’s create our first weldment. Start of with a 3D sketch.
Go to the weldments tab and select Structural Member.
On the left side of the screen, you will now see the Property Manager of the structural member,
which gives you the option to select the standard, the type and the size.
For now I will choose the ISO, the square tube and a 20x20x2 size. There are a few other options, but I will look at those later.
With the size selected, I can now select the first segment of the connected sketch.
Notice that the corners are trimmed according to the corner treatment decided in the properties.
For the next section, I am going to create three more groups of the two connected sketch segments and select them as seen in the screenshot.
In the 6th group, I am going to place the last sketch entries, which are not connected.
Looking at the finished result, the profiles have been created.
It is possible to change the trimming and the corner treatment, but as this is a more introductory article, that can wait for another time.
The Cut List
The cut list allows you to create a detailed list of the length and angles of the profiles used in this weldment, which can be inserted and used in the production drawing.
To create the cut list, look in the property tree for the Cut list section.
If it has not already been created and is still a mess of solid bodies, right click on Cut list and select “Create Cut Lists Automatically.”
This will organize your cut list, and by right-clicking on one of the entries, you can have a look at the properties.
The Cut List Properties dialog will show the length and angles of the profiles created.
This cut list will update automatically when you add more weldments.
With the drawing of the weldment, go to Insert > Tables > Weldment Cut List.
This is your standard cut list, but it is possible to add more properties if need be (for instance material, finish, etc.)
Creating your own weldment profiles
You’ve gotten started with weldments, but you have some very specific profiles in your workshop.
Thankfully, it’s very easy to create your own weldment profile. The first thing you need to do is find the weldment profile location.
Go to Tools > Options > System options > File location, and find Weldment Profiles.
The default location is “C:\ProgramData\SolidWorks\SOLIDWORKS <year>\weldment profiles.”
Make sure you have write rights to that folder, or create your own save location by adding your own folder, which I have done and called it “Custom Profiles.”
Now create a new part and create a sketch of your profile. To start, I have created a simple rectangle.
A few notes on this:
First off, it is important that the sketch is fully defined, as it will allow me easily to create different sizes of my profile.
By default the origin is my insertion point.
In my Custom Profiles folder, I created a new folder called “Tinndahls Profiles” and then save the file as a library feature part (.sldlfp) and call it “Tinndahl.”
The sketch icon has now changed to a library feature.
As a final step, I renamed the configuration to match the measurement (90x120x5) and created another configuration with other measurements.
And finally, I am going to ensure that the dimensions change according to the configuration selected.
Save and close, and we can now test it on a 2D sketch.
Within the weldment, the “Tinndahls Profiles” folder is visible.
The “Type” is the file name: “Tinndahl.”
And the size is the configuration I just created.
And that’s it! There isn’t much more to it when creating your own weldment profiles.
If you want more configurations, you can create a design table to control the measurements.
Conclusion
Weldments in SOLIDWORKS provide an efficient way to design structural frames, allowing engineers to move faster from sketch to fabrication-ready documentation. By learning how to use standard tools, customize profiles and take advantage of configurations and design tables, you can greatly reduce design time while improving consistency across projects.
For teams, setting up a shared library of profiles—whether based on industry standards or company-specific shapes—ensures that everyone works from the same source of truth. The investment in building these libraries pays off quickly in reduced rework, accurate cut lists and easier collaboration.
Now it’s your turn: start small by creating a single custom profile, add a design table for a few common sizes, and test it in a simple weldment. Once you see how much time it saves, expand your library and share it with your team. The sooner you standardize your weldment workflows, the faster you’ll deliver consistent, high-quality designs ready for manufacturer.