Bent Tube Developed Length from SolidWorks Weldments — Getting a Number Your Tube Bender Trusts

Your tube bender needs one number before they can key anything into the CNC machine: the developed length, also called the cut length — the stock length of straight tube that goes in and produces your bent part when it comes out. Give them the wrong number and you are either scrapping material or re-cutting after the fact.

SolidWorks weldments give you a length. The question is what that length actually represents, and when it matches what the bender needs.

What SolidWorks Reports in the Cut List

When you create a structural member along a 3D sketch path, SolidWorks sweeps the selected profile along the path segments and stores a LENGTH property in the cut list. That length is the geometric arc length of the path sketch — measured along whatever path you drew, at whatever radius the sketch circles were drawn.

For a path with two straight runs connected by a 90° arc, the cut list entry sums:

• Straight segment 1: its sketch length
• Arc segment: CLR × (π/2) where CLR is the centerline bend radius (the arc radius in your sketch)
• Straight segment 2: its sketch length

If you drew the sketch with the arc centered on the tube centerline — which is the natural thing to do in SolidWorks — CLR in that formula is the tube’s centerline bend radius.

What Merge Arc Segments Does (and Does Not Do)

The Merge Arc Segments checkbox on a structural member feature (right-click the member in the FeatureManager → Edit Feature) controls how many cut list rows the member produces.

Without it: a tube with three bends produces seven cut list rows — four straight segments and three arc segments, each with its own length.

With it: all segments merge into a single cut list row showing one total length. That total is the sum of all individual arc lengths and straight run lengths.

This is useful for BOMs and cut list tables. It does not change how the length is calculated. The merged length is still the sum of path arc lengths — the same number you would get by adding the rows manually.

What Merge Arc Segments does not do:

• Apply any bend correction or neutral axis offset
• Distinguish between segment types (you lose per-bend visibility)
• Give you a number that accounts for material behavior during bending

For many structural framing applications, the path arc length is close enough to the developed length that the difference is within your tube stock tolerance. For tight bends or precision parts with stacked bends, it is not.

The Neutral Axis Offset — When It Matters

During tube bending, material on the outside of the bend stretches and material on the inside compresses. The neutral axis is the imaginary line through the tube wall where the stress is zero — where the material neither stretches nor compresses. The length along the neutral axis before bending equals the arc length of that section after bending.

For round tube with large bend radii (CLR ≥ 3× OD), the neutral axis lies very close to the tube centerline. The difference between the path centerline arc length and the neutral axis arc length is under 0.5% per bend. For typical structural frames with tolerances of ±1–2mm, you can ignore the correction entirely.

For tight bends (CLR < 2× OD) or thick-walled tube (OD/wall < 10), the neutral axis shifts measurably. The shift depends on the tube’s D/t ratio (diameter to wall thickness), the CLR/D ratio (bend radius to diameter), and the bending method (draw bending, rotary draw, mandrel bending). Mandrel bending on thin-wall tubing produces the least ovalization and keeps the neutral axis close to the centerline; compression bending on heavy tube pushes it further in.

The practical threshold: if your CLR is less than 2.5× the tube OD, verify your cut lengths against the tube bender’s bend factor data before ordering stock. If CLR is 3× OD or more, the path centerline length is fine.

Method 1: Equation Sum of Sketch Dimensions

The most common approach in tutorials. Edit the 3D sketch used for the structural member path, add arc length dimensions to each arc segment (select the two arc endpoints, then the arc itself), add driven linear dimensions to each straight segment. Create a global variable in Tools > Equations that sums them:

"CUT_LENGTH@Part1"= "ArcLen1@3D Sketch1" + "Seg1@3D Sketch1" + "ArcLen2@3D Sketch1" + "Seg2@3D Sketch1"

Link this to a custom property (File > Properties → Custom) so it appears in your BOM and on the drawing:

Name: CUT_LENGTH
Type: Text
Value: $PRP:"CUT_LENGTH@Part1"

This gives you the path centerline arc length. For most structural tube bending (CLR ≥ 3× OD), this is the number your tube bender programs into the machine as the developed length.

Limitation: this approach requires manual dimension placement in the sketch. If you later change the 3D sketch path, the driven dimensions update automatically, but arc length dimensions on SolidWorks sketch arcs do not always survive sketch rebuilds cleanly. Test after any path change.

Method 2: Composite Curve and IMeasure

For a complex path with many segments, create a Composite Curve (Insert > Curve > Composite) by selecting all the 3D sketch segments that make up the tube path. Then use Evaluate > Measure, select the composite curve, and SolidWorks reports the total arc length.

This is the same number as Method 1, obtained without manually dimensioning every segment.

Via API, the same result:

IMeasure swMeasure = (IMeasure)swApp.GetMeasure();
swMeasure.ArcOrSketchSegment = (object)compositeCurveFeature.GetSpecificFeature2();
bool calc = swMeasure.Calculate(null);
double totalLengthMeters = swMeasure.ArcLength; // meters — divide by 0.001 for mm

IFeature.GetSpecificFeature2() on a Composite Curve feature returns an ICurve interface. The IMeasure.ArcLength property returns the total arc length in meters (SolidWorks internal units), regardless of your document unit settings.

This method is faster than Method 1 for complex paths and is API-automatable, but still gives you the path centerline arc length without neutral axis correction.

Method 3: Sketch at the Neutral Axis Radius

The most accurate approach for tight-bend parts: instead of drawing the path sketch at the tube centerline, draw it at the neutral axis radius. Then the path arc length that SolidWorks reports is already the neutral axis arc length — which is what the bender needs.

For round tube with mandrel bending, the neutral axis radius for each bend is approximately:

R_neutral ≈ CLR_centerline - (OD/2) + (OD × K_tube)

Where K_tube is the tube bending K-factor — the fraction of the tube OD from the inner radius to the neutral axis. For thin-wall tube (OD/wall > 20) at CLR/OD ≥ 2.5:

K_tube ≈ 0.45 to 0.50

This makes R_neutral ≈ CLR_centerline for thin-wall tube at common bend radii. The correction is negligible.

For thick-wall tube (OD/wall < 10) at tight CLR (CLR/OD < 2.0):

K_tube ≈ 0.33 to 0.38

Meaning the neutral axis shifts inward toward the inner radius, and the path arc length at the centerline slightly overestimates the developed length.

To implement this in SolidWorks: modify your 3D sketch to draw the arc at R_neutral instead of at CLR_centerline. Use a global equation variable to drive the arc radius so it stays linked to the tube OD and wall:

"R_NEUTRAL" = "CLR_CENTERLINE" - ("OD" / 2) + ("OD" * "K_TUBE")

Then dimension the arc radius in the sketch to $PRP:"R_NEUTRAL" via a driven dimension.

This adds complexity to the model. For most structural tube — CLR ≥ 3× OD — skip it. Reserve Method 3 for precision robotics end-effectors, hydraulic hard-line bends, and parts where ±0.5mm on the developed length matters.

What the Tube Bender’s Machine Actually Uses

CNC tube benders (BLM, Addison, Unison, Transfluid) accept bend programs in two forms:

1. CLR + angle per bend: the machine calculates developed length internally from its own material database. The machine’s calibrated K-factor for your tooling setup takes precedence over anything in your CAD model.

2. Pre-calculated developed length: you provide the cut length, and the machine uses it directly. In this case your CAD-derived developed length must match the machine’s neutral axis model.

Most tube fabrication shops that run production bending work from CLR + angle inputs rather than pre-calculated cut lengths. Your SolidWorks model supplies the CLR and bend angle per bend; the machine does the rest.

If you’re sending programs to a shop for the first time, ask which format they use. If they take CLR + angle: your weldment geometry is the input, and the cut length from the cut list is what they use to order stock — close enough for CLR ≥ 3× OD. If they take developed length directly: apply Method 3 or use their material-specific K-factor correction.

Cut List vs Weldment Summary — Which Length Shows Where

The LENGTH property in the cut list is always the geometric path length. It is not modified by any material property, K-factor setting, or bend factor — those are sheet metal concepts that do not transfer to the weldment environment.

End-Preps and CadShift

If your bent tube has laser-cut cope profiles at the ends (the contoured cut that lets two tubes meet cleanly at a joint), those cope profiles are typically a separate step from the bending. You model the tube in SolidWorks as a weldment member, compute the correct bend geometry, and then export the cope profile to DXF for the tube laser.

CadShift can export flat-pattern DXF files from weldment assembly components, including the extracted profile contours for end-preps. See batch DXF export from SolidWorks assemblies for the export workflow. For the cope geometry itself — why the oval cross-section in a bent tube makes the SolidWorks-computed cope profile wrong — see bent tube weldment cope geometry.

Practical Checklist Before Sending to the Bender

1. Check your CLR/OD ratio first. CLR ≥ 3× OD: use the path centerline arc length. CLR < 2.5× OD: apply the K-factor correction or confirm the machine uses CLR + angle input.
2. Enable Merge Arc Segments to get a single total length in the cut list — easier to read and less error-prone than adding multiple rows.
3. Add a CUT_LENGTH custom property via equations so the number appears in your BOM automatically — no manual entry, no transcription errors.
4. Verify arc length dimensions rebuild correctly after any sketch change. Driven arc length dimensions in SolidWorks sketch arcs can detach during aggressive sketch edits; check they’re still green (driven) before taking the value.
5. Don’t confuse cut list length with drawn length for the shop traveler. The developed length on the traveler is what gets ordered and what goes into the bender. The bent dimension on the drawing is the finished reference. Keep them labeled clearly.

The merge arc segments checkbox tidies your cut list. The neutral axis correction is what closes the gap between what SolidWorks models and what the bender machines.