A fabricator running a CNC tube laser — Trumpf TruLaser Tube, BLM LT-Free, Mazak FT-150 — expects the DXF cope geometry to land flush against the mating tube. When it doesn’t, someone grinds. When it really doesn’t, the joint gets welded with a visible gap, weakening the bead and failing inspection.
The problem starts in SolidWorks before the export ever happens.
How SolidWorks Models Weldment Tubes
The SolidWorks Weldment feature builds structural members by sweeping a 2D profile sketch along a 3D path. The profile is constant — it maintains its exact shape and size throughout the entire sweep. When two members intersect, SolidWorks trims them automatically to create the cope (the curved notch that allows one tube to seat against another).
This is clean, predictable behavior for columns, beams, and frames where the tubes are straight. The problem emerges the moment a tube is bent.
What Actually Happens to a Tube During Bending
When a round tube is bent, the cross-section at the bend deforms. Longitudinal tensile stress on the outside of the bend and compressive stress on the inside force the circular profile to flatten into an ellipse. The degree of flattening — called ovalization — depends on the tube’s D/t ratio (outer diameter divided by wall thickness) and the bend radius.
This behavior is governed by the Brazier effect, a structural mechanics phenomenon documented in tube bending literature since the 1920s. The relationship is nonlinear: thin-walled tubes (high D/t) ovalize significantly more than thick-walled ones. Rough empirical ranges:
- D/t ≈ 10 (thick-walled, e.g. 50mm OD × 5mm wall): ovalization 2–4%
- D/t ≈ 20 (common structural tube, e.g. 50mm OD × 2.5mm wall): ovalization 5–10%
- D/t > 40 (thin-walled): ovalization 15%+ without mandrel support
A 10% ovalization on a 50mm tube means the minor axis shrinks to roughly 45mm and the major axis grows to roughly 55mm at the bend tangent. That’s not a rounding error — it’s 5mm of deviation at the cope contact line.
Why This Makes the Cope Wrong
SolidWorks computes the cope as the intersection of two circular profiles. When you trim two structural members, it finds where a cylinder of radius R1 intersects a cylinder of radius R2 at the given joint angle and produces the saddle curve that separates them.
That calculation is correct — for straight tubes.
For a bent tube, the cross-section at the bend tangent (exactly where the cope lives) is not circular. It’s an ellipse with a different minor and major axis. The saddle curve SolidWorks computes assumes a circle. The actual geometry the laser cuts needs to account for an ellipse.
The mismatch produces a cope that is too deep at the minor axis of the ellipse and too shallow at the major axis. The tube doesn’t seat flush. Instead of a tight, continuous contact line around the joint perimeter, you get alternating gaps and interferences.
In practice, fabricators see this as:
- Visible gaps at the weld joint, usually at the extremes of the oval’s major axis
- Interference (overlapping material) at the minor axis, preventing the tube from seating at all
- Rocking — the coped tube can sit at different angles depending on which way it’s rotated against the mating member
- Rework time — angle grinders and hand files to make the joint acceptable before welding
For structural applications, weld quality at a poorly fitted joint is degraded: the welder has to bridge a gap rather than fuse two surfaces in contact, which means less penetration and a weaker bead at the stress concentration.
The Export Dependency
Every DXF export from a SolidWorks weldment — whether via native Save As or through a batch tool like CadShift — reflects the geometry as modeled. If the cope was computed against a circular cross-section, the exported DXF cope is circular. The error is upstream, in the SolidWorks model, not in the export step.
This is worth being explicit about because it changes where the fix must happen. No export setting, no post-processing script, and no CAM software correction will produce a geometrically correct cope from an incorrect CAD model. The correction has to happen in SolidWorks before you get to export.
Three Ways to Get the Right Cope Geometry
Option 1: Measure and Manually Correct (Empirical)
Bend a sample tube under the same conditions as the actual job — same material, same OD and wall, same bend radius. Measure the actual cross-section at the bend tangent with a caliper or coordinate measuring device. You’ll get an ellipse with measured major and minor axes.
Take that measured ellipse into a separate sketch. Overlay it with the SolidWorks-generated cope curve. The difference between the two gives you the correction amount at each point. For simple cases, you can often approximate the correction as a uniform radial offset applied to the cope curve in the DXF.
Where this works: Low-volume, one-off fabrication where you have a sample tube and the time to measure it. The correction doesn’t propagate back to the SolidWorks model, so design changes require the process to restart.
Where it breaks: Production runs, parts with design iterations, anything where the CAD model drives downstream processes. You end up maintaining a DXF correction separate from the model, which diverges as soon as the design changes.
Option 2: Model an Explicit Elliptical Profile
Create a custom weldment profile sketch that matches the actual elliptical cross-section of the bent tube at the cope location. Assign this elliptical profile to the structural member at the bend, and let SolidWorks compute the cope against the correct geometry.
The ellipse dimensions come from either:
- Measurement of a physical sample bend (same as Option 1, but the correction goes into the model)
- Calculation using the Brazier effect relationship for your specific D/t ratio and bend radius
Once the elliptical profile is in place, SolidWorks trims the intersection correctly. The cope saddle curve is now computed against the actual cross-section. Export produces geometrically correct cope geometry.
Where this works: Repeatable products with known bend geometries — the same tube, same bend radius, same joint angle, every time. A custom profile is a one-time investment.
Where it breaks: Multi-product environments where bend radius varies by job. You’d need a library of elliptical profiles indexed by D/t ratio and bend radius. Manageable for a small product family; unwieldy at scale. Also: the transition between the circular tube body and the elliptical profile at the bend tangent may require careful sketch placement and can create visual artifacts in the model.
Option 3: Use Dedicated Tube Bending Software
Several tools in the tube fabrication space model bending deformation natively:
Bend-Tech (Bend-Tech Pro, Bend-Tech SE): Full CAD/CAM for tube bending. Models the bending process, computes the actual cross-section deformation, and exports cope geometry to DXF that accounts for the real elliptical profile. Designed specifically for the fabricator-side workflow.
SolidWorks Tube & Pipe (Routing add-in): Handles tube routing within assemblies, but focuses on routing geometry rather than bending physics. Does not compute Brazier ovalization. Useful for routing layout, not for correcting cope geometry on bent structural members.
SigmaTUBE: CAM software that integrates with SolidWorks. Takes tube geometry from SolidWorks, applies bending simulation, and generates correct toolpaths for tube laser cutting. The correction happens in the CAM layer rather than in the SolidWorks model itself.
BLM ArTube: Paired with BLM laser tube cutting machines. Handles the post-bend cutting workflow where the laser cuts the cope after the tube is already bent — at which point the machine can measure and adapt to the actual tube geometry. This sidesteps the ovalizing problem entirely, but requires post-bend cutting capability.
Where this works: High-volume tube fabrication where cope accuracy is a recurring requirement. The software cost amortizes quickly against rework and grinding time on complex assemblies.
Where it breaks: If you’re only occasionally building bent-tube weldments and the joint angles are simple, the overhead of adopting a new tool may not be justified.
How to Know If You Have This Problem
Not all weldment cope joints involve bent tubes. Straight-to-straight joints — a cross brace meeting a column — don’t exhibit this problem. The issue only appears when a structural member is bent and then coped.
Check your model for:
- Swept structural members with curved paths — any member that follows a curved 3D path is potentially bent
- High D/t ratio members — thin-walled round tube is most susceptible; heavy-wall or square section much less so
- Small bend radii relative to tube diameter — tighter bends cause more ovalization than gentle bends
- CNC tube laser cutting as the downstream process — manual notching with a cope notcher is often adjusted by eye; CNC laser cutting exposes the error directly
If you export weldment cut list DXFs for a laser tube cutting house and you’re getting fitup complaints on bent tubes, the cope geometry is the first thing to check. The weldment cut list naming and PARTNUMBER setup is a separate issue, but both affect what arrives at the shop floor.
The SolidWorks API Perspective
For teams building batch export tools or macros that process weldment parts programmatically, the cut list body geometry is accessible through IFeatureCutListFolder and the IBody2 interface on each cut list item. The body geometry is the modeled geometry — the constant circular sweep. There is no property on the body that flags whether the member is bent or reports the degree of ovalizing.
Detecting a bent structural member requires traversing the feature tree to find the path sketch, checking whether the path is curved, and then reading the D/t ratio from the profile dimensions and cut list custom properties. From there you could calculate expected ovalization and warn the user before export.
This kind of pre-export validation — flagging weldment bodies whose cope geometry is likely to be wrong because of tube bending — is the sort of thing that prevents shop floor surprises. The VBA macro edge cases for batch DXF export covers similar upstream detection problems where the model state affects export correctness.
The Short Version
SolidWorks weldments model tubes as constant circular sweeps. Bent tubes have oval cross-sections. Copes computed against a circle don’t fit an oval. The exported DXF inherits whatever cope is in the model.
Fix it before export: measure the actual ellipse and correct the DXF manually (one-off jobs), create a custom elliptical weldment profile (repeatable products), or route through tube-native software that models bending deformation (high-volume production).
If the SolidWorks model has the right geometry, every DXF export — batch or single, via any tool — will have the right cope. If it doesn’t, no export configuration can fix it.