Why Weldments Beat Multi-Body Modeling for Structural Frames
If you have tried modeling a structural steel frame by extruding individual members and positioning them with mates in an assembly, you know how slow and fragile that approach is. Change the frame height and you are manually editing a dozen extrude dimensions. Add a diagonal brace and it intersects other members incorrectly. The BOM shows twelve separate part files that need individual drawings.
SolidWorks Weldments solves this. The entire frame is one part file. A 3D sketch defines the skeleton — all the member centerlines. Weldment profiles are swept along those lines automatically. Trim and extend handles intersections. A cut list generates the BOM automatically. This is the right tool for any structure made of standard structural sections.
The 3D Sketch: The Foundation
A Weldment model starts with a 3D sketch that defines the skeletal geometry — lines and arcs representing the centerlines or reference lines of all structural members.
Create a 3D sketch: Insert > 3D Sketch (or click the 3D Sketch tool in the Sketch tab). In 3D sketch mode, you can draw lines in any plane — the view orientation determines whether a line goes X, Y, or Z. Use the Tab key to switch the sketch plane while drawing.
Practical approach: start with the primary frame perimeter, then add vertical columns, then diagonal braces and cross-members. Fully constrain the 3D sketch using dimensions and relations just as you would a 2D sketch. An unconstrained 3D sketch means frame dimensions can change unpredictably.
Group related lines using selection and relations: vertical lines that are all the same height should be Equal. Horizontal members at the same level should be Collinear or have equal dimension constraints. Build in the symmetry that the physical structure requires.
Structural Member Profiles
Once the 3D sketch is complete, add structural members: Insert > Weldments > Structural Member. The property manager asks for:
- Standard: ISO, ANSI, DIN, etc.
- Type: square tube, rectangular tube, round tube, angle, channel, I-beam, etc.
- Size: the specific cross-section (e.g., 50x50x4 SHS, HEA 160)
Select the sketch lines that represent this member type. SolidWorks sweeps the selected profile along the lines, automatically mitering corners where lines connect.
Profile alignment options: center at sketch line, corner at sketch line, or custom offset. For structural calculations, center alignment is standard. For detailing where member faces must align at a specific position, use offset alignment.
The Profile Library
SolidWorks ships with structural profiles for ISO, ANSI, DIN, and other standards. The library files are located in the SolidWorks installation folder under data\weldment profiles.
If your standard profile is missing (company-specific extrusion, custom tube size), create it: sketch the cross-section profile in a new part file, save it as a .sldlfp (library feature part) in the weldment profiles folder under the appropriate standard and type subfolder. It then appears in the Structural Member dialog like any other profile.
For teams: store custom profiles on a shared network folder and add that path to Tools > Options > System Options > File Locations > Weldment Profiles. All team members then access the same custom profiles.
Trimming and Extending Members
Where members intersect, SolidWorks handles corner conditions automatically for simple cases (miter, butt, corner). For more complex intersections — diagonal braces meeting column faces, cross-members at mid-span — use Trim/Extend: Insert > Weldments > Trim/Extend.
Select the member to trim and the trimming body (the face or body to cut against). Choose the treatment: butt cut (90° end cut), cope (fishmouth cut that allows one member to pass through another’s profile), or miter. The physical weldment detail drives which option to use — consult your fabricator’s practice.
Trim operations add significantly to rebuild time in large weldments. Apply them after the basic structure is complete and verified, not during initial layout iterations.
Gussets and End Caps
Gussets reinforce joints between members. Insert > Weldments > Gusset: select the two faces you want to reinforce, specify thickness and profile shape (flat plate, angular, etc.), and SolidWorks places the gusset geometry. The gusset appears as a separate body in the weldment multi-body part, with its own cut list entry.
End caps close open tube ends: Insert > Weldments > End Cap. Select the open face of a hollow section, specify the thickness, and the cap is added. Standard practice for structural tubes that will be exposed to moisture — open tubes collect water and corrode from the inside.
The Cut List: Automatic BOM
The cut list (right-click on “Cut list” in the Feature Manager tree, select Update) automatically groups identical members and calculates quantities and lengths. This is the weldment’s BOM.
Each cut list item can have custom properties: description, material, finish. Right-click a cut list folder, select Properties, and enter the data. Link cut list properties to a drawing table the same way part custom properties link to a title block.
The cut list is the foundation for the fabrication workshop drawing — it tells the welder exactly what to cut, how many pieces, at what length, from what material.
Creating Weldment Drawings
A weldment drawing typically includes:
- Overall assembly view with principal dimensions
- Individual member detail views showing end treatments and hole locations
- Cut list table (Insert > Tables > Weldment Cut List in the drawing environment)
- Weld symbols on joint locations
For individual member detail drawings, use the “Weldment Detail” function in the drawing: Insert > Relative to Model or Create Drawing from Cut List Item. SolidWorks generates a detail drawing for each unique member, with the correct length and end treatment shown, ready to be dimensioned.
Key Takeaways
- Weldments model an entire frame in one part file, driven by a 3D sketch skeleton. This is dramatically faster and more manageable than assembling individual part files.
- Fully constrain the 3D sketch. Frame dimensions that are not fully constrained will drift on rebuild.
- Store custom profiles on a shared network path accessible to the whole team.
- Use Trim/Extend for complex intersections. Apply it after the basic structure is verified to avoid slow iterative rebuilds.
- The cut list generates a fabrication BOM automatically. Populate cut list custom properties for description and material so the workshop drawing is complete.
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