The flat pattern comes out wrong. The folded part measures correctly. The DXF dimensions are off by a few millimeters — or sometimes more. Your press brake operator is asking questions you can’t easily answer.
This is a K-factor problem, and it’s common enough that manufacturing shops build their own macros to detect it. Understanding why it happens, and how to set SolidWorks up to avoid it, is worth the time for any team doing regular sheet metal work.
What K-Factor Actually Controls
When sheet metal bends, the material on the inside of the bend compresses and the material on the outside stretches. Somewhere between those two surfaces is a theoretical neutral axis — a layer that neither stretches nor compresses during forming.
The K-factor defines where that neutral axis sits, expressed as a ratio of its distance from the inside face to the total material thickness. A K-factor of 0.5 puts the neutral axis exactly in the middle of the material. In practice, K-factors range from about 0.25 to 0.50, depending on material type, thickness, and the specific tooling.
SolidWorks uses the K-factor (or alternatively, bend allowance or bend deduction tables) to calculate how much material length is consumed in each bend. The flat pattern is the unfolded geometry based on that calculation. If the K-factor is wrong, the flat pattern is wrong — and so is every DXF you export from it.
Where the Misconfiguration Happens
There are three places K-factor can be set in SolidWorks, and they can conflict with each other:
1. SolidWorks Tools → Options → Document Properties → Sheet Metal
This is the document-level default. It applies to any sheet metal feature created in a new part unless overridden at the feature level. Teams that never touch this setting are using whatever the default was when they installed SolidWorks — which may or may not match their actual press brake tooling.
2. Sheet Metal feature definition (the Base Flange)
When you create the base flange of a sheet metal part, the Sheet Metal dialog includes a Bend Allowance section where you can set K-factor, bend allowance, or bend deduction directly. This overrides the document default for that part. If a part was created by someone else with different settings, this is where their values live.
3. Gauge Tables
If your team uses gauge tables (Excel files that define thickness and bend allowance by gauge number and tooling), the bend allowance values come from the table rather than a K-factor entry. This is the most reliable approach when your shop has well-characterized tooling — the table directly maps material/gauge combinations to the deduction values your press brake produces.
The mismatch scenario that causes trouble: Document Properties says K=0.42, the base flange says K=0.33, and the operator’s press brake tooling actually produces results consistent with K=0.38 for that material and thickness. Every downstream DXF is carrying the wrong flat pattern.
How to Check What Your Part Is Using
Open the sheet metal part, edit the Base Flange feature, and check the Bend Allowance section. The value there is what SolidWorks is using for that part — regardless of what’s set in Document Properties.
To verify across an assembly, check each part individually. There’s no assembly-level view that summarizes bend allowance settings across all contained sheet metal parts in a single dialog.
For a quick sanity check, flatten a bend manually (right-click a bend face → Flatten) and measure the flat length against a hand-calculated bend allowance using your press brake’s known deduction values. If they don’t agree within tolerance, the K-factor is wrong.
Setting Up Correctly
The most reliable approach for teams with consistent tooling is a gauge table that encodes the actual deduction values from the press brake manufacturer’s specification or from measured test bends.
- Create or obtain a gauge table Excel file (SolidWorks has sample templates in the lang folder of the installation directory).
- Populate bend allowance values per material, thickness, and tooling radius based on your actual press brake.
- Set the Document Properties to reference this gauge table by default.
- When creating new sheet metal parts, use the gauge table option in the Base Flange dialog rather than a manual K-factor entry.
This means anyone creating a new part gets consistent settings automatically. Existing parts need to be audited and updated — there’s no batch operation for this in standard SolidWorks.
What Happens at DXF Export
When you export a flat pattern to DXF — whether manually or through a batch export tool — SolidWorks flattens the geometry using whatever bend allowance the part was built with. The export itself doesn’t recalculate or override the flat pattern dimensions.
This is why getting the K-factor right at the modeling stage matters more than the export workflow. A batch export tool will faithfully export whatever flat pattern the part produces. If the flat pattern is wrong, the DXF is wrong — and you won’t catch it until the part is cut and it doesn’t fold correctly.
Batch exporting DXF files from a SolidWorks assembly is the right workflow for scale, but it amplifies whatever’s already in the models. If ten parts in an assembly have the wrong K-factor, batch export gives you ten wrong DXFs simultaneously.
CadShift respects the flat pattern as defined in the part — including the bend allowance settings — and exports exactly what SolidWorks would produce manually. That’s the correct behavior. The fix is upstream, in the part definition itself.
What Fabricators See
When a flat pattern dimension is off, the fabricated part doesn’t match the drawing. The magnitude of the error scales with the number of bends and the severity of the K-factor deviation. A single 90° bend in 3mm steel with a K-factor error of 0.05 produces roughly 0.15mm of flat pattern error per bend — which compounds across multi-bend parts.
For laser cut parts going to a press brake, the cutter produces the flat exactly as specified in the DXF. If the flat pattern is wrong, the finished part is wrong. There’s no opportunity to catch this at the cutting stage — the error only shows up when the part is bent.
Some fabricators have started requesting that engineers include the K-factor and bend deduction values as a note on the drawing, or embedded in the DXF layer metadata, precisely so they can flag mismatches against their tooling before cutting. This is a reasonable request. What fabricators actually need from your DXF files goes beyond geometry, and K-factor documentation is part of that picture.
Standardizing Across the Team
If multiple engineers are creating sheet metal parts and each has slightly different bend allowance settings, you’ll get inconsistent flat patterns across the assembly. This becomes visible at fabrication — some parts fit, others don’t.
The fix is standardization at the template level:
- Create a SolidWorks part template with Document Properties correctly configured, pointing to the gauge table.
- Save it in a shared location and make it the team’s default sheet metal template.
- For existing parts, review and update the Base Flange feature for any part where the bend allowance settings don’t match the standard.
Some Swedish manufacturing companies have documented this problem specifically in the context of press brake tooling standardization — recognizing that the CAD model’s K-factor needs to match what the machine actually produces, not just what the material specification suggests.
The underlying principle is that flat pattern accuracy is a chain: material properties → tooling selection → K-factor/bend deduction → part model → flat pattern → DXF. Break any link in that chain and the part won’t fold correctly. Getting the CAD side of that chain right is the engineer’s responsibility before the file ever reaches the shop floor.
The Kernel Connection: Why This Matters Beyond SolidWorks
The K-factor calculation feeds into the geometric kernel’s unfolding algorithm. In SolidWorks, the flat pattern is generated by the CATIA CGM kernel’s sheet metal body classes (CATSHMBody, CATSHMFace, CATSHMEdge) running on top of Parasolid’s B-Rep representation — as we documented in our flat pattern deep dive. The unfolding is a kernel-level operation, not just a UI feature.
If you’re migrating sheet metal parts between CAD systems, be aware that different kernels may compute slightly different flat patterns from the same bend parameters. A part designed in SolidWorks (Parasolid + CATIA CGM) and imported into FreeCAD (OpenCASCADE) won’t carry its K-factor settings — and even if you manually re-enter the same K-factor, OCCT’s unfolding algorithm may produce a marginally different flat pattern because the kernel’s bend deduction math isn’t identical. The same applies to Inventor (ShapeManager/ACIS). These differences are typically small (fractions of a millimeter), but they compound across multi-bend parts. For more on how the three major kernels handle geometry differently, see our kernel fillet comparison.