A fabricator opens your STEP file. They run Insert Bends. SolidWorks creates a flat pattern. The dimensions are wrong.

Not slightly wrong — off by several millimetres on every bend. Enough to cause rework. Enough to get a call from the shop floor.

The reason is that STEP files don’t carry k-factor data. They never did. Understanding why, and what to do about it, is the difference between a clean handoff and a rebuild.

What STEP Actually Encodes

STEP (ISO 10303) encodes boundary representation geometry: surfaces, edges, vertices, and the topological relationships between them. For a sheet metal part with a 90° flange, STEP stores the final folded shape — a precise solid with a cylindrical inner radius at each bend.

What STEP does not store:

  • K-factor
  • Bend allowance or bend deduction method
  • Gauge table assignment
  • The flat pattern dimensions
  • Material specification in a machine-readable form usable by CAM

This is by design. STEP is an exchange format for geometry, not manufacturing intent. The folded solid is mathematically unambiguous. The manufacturing parameters that produced it are out of scope for the format.

AP203, AP214, and AP242 all have this characteristic. AP242’s MBD (Model-Based Definition) extension adds PMI — GD&T annotations, surface finish callouts — but it still does not include bend allowance method or k-factor value. Those remain outside the STEP spec.

What Happens During Insert Bends

When you import a STEP and run Insert Bends (Sheet Metal toolbar → Insert Bends), SolidWorks:

  1. Detects the uniform wall thickness from face-to-face measurements
  2. Identifies cylindrical faces as bend regions
  3. Extracts the inner bend radius from the cylinder geometry
  4. Creates a flat pattern using your current document k-factor default

Step 4 is where the flat pattern breaks.

If the original designer modelled with k=0.38 (typical for 304 stainless steel with a standard press brake punch), and your SolidWorks default is k=0.50 (the SolidWorks factory default), your flat pattern will be longer than the original on every bend. For a part with six 90° bends at 2mm material, this accumulates to 3–5 mm of total blank length error — enough to scrap the part if the tolerance is tight.

The geometry looks correct in the folded view. The flat pattern is dimensionally wrong.

Convert to Sheet Metal vs Insert Bends

These two commands handle STEP imports differently:

Insert Bends (Sheet Metal → Insert Bends): Takes a solid that already has sheet metal geometry — uniform walls, cylindrical bend regions — and adds the Sheet Metal feature to the model. Preserves the existing folded geometry. Applies your system default k-factor to generate the flat pattern. This is the correct approach for most imported STEP sheet metal files.

Convert to Sheet Metal (Sheet Metal → Convert to Sheet Metal): Designed for solid block models where you pick a base face and define rip edges to create bends. The geometry is restructured from a solid into a parametric sheet metal feature tree. Rarely useful for imported STEP sheet metal parts — those already have the correct bend geometry present. Use it when you have a solid block and want SolidWorks to build the sheet metal feature tree from scratch.

For a STEP import of an existing sheet metal part, Insert Bends is the right tool.

The Geometry That Fails

Even Insert Bends has geometry it cannot handle. The operation fails or silently omits features when:

Holes through bend regions: SolidWorks cannot determine the flat pattern shape for holes that span the bend neutral axis. The hole geometry is valid in the folded solid but undefined in the flat state. Insert Bends either errors or drops the hole silently from the flat pattern.

Edge flanges on curved base flanges: A flange added to a curved edge — say, a cylindrical base plate with an attached perpendicular flange — requires unrolling a compound-curved surface. SolidWorks sheet metal handles single-axis bends. Compound curves are outside scope.

Forming tools embedded in geometry: Formed features (lance-and-form, offset punch patterns, dimples) appear as raised or depressed geometry in the STEP solid. Insert Bends sees a bump on a surface, not a forming operation. The flat pattern cannot correctly unfold forming tool geometry.

Tapered cross-sections: Sheet metal parts that taper in width along their length don’t map to SolidWorks sheet metal’s uniform-width assumption.

When Insert Bends fails on any of these, the only reliable path is to rebuild the part natively using the STEP as a dimensional reference.

Correcting K-Factor After Insert Bends

Once Insert Bends creates the Sheet-Metal feature, correcting the k-factor is straightforward:

  1. In the FeatureManager, right-click Sheet-Metal1 → Edit Feature
  2. Under Bend Allowance, change the method and value to match your gauge table
  3. Rebuild — the flat pattern updates immediately

For batch correction via API, ISheetMetalFeatureData exposes the k-factor property:

' VBA: Correct k-factor on imported STEP sheet metal part
Dim swApp As SldWorks.SldWorks
Dim swDoc As SldWorks.ModelDoc2
Dim swFeat As SldWorks.Feature
Dim swSMData As SldWorks.SheetMetalFeatureData

Set swApp = Application.SldWorks
Set swDoc = swApp.ActiveDoc

' Sheet-Metal feature is always named "Sheet-Metal1" on Insert Bends
Set swFeat = swDoc.FeatureByName("Sheet-Metal1")
Set swSMData = swFeat.GetDefinition()

' Set k-factor for 304 SS with standard press brake tooling
swSMData.KFactor = 0.38

Dim bRet As Boolean
bRet = swFeat.ModifyDefinition(swSMData, swDoc, Nothing)
swDoc.EditRebuild3

The k-factor value must match what your press brake operator uses for that material and thickness, not what the original designer assumed. That number comes from your gauge table. For background on how k-factor affects flat pattern dimensions in general, see why DXF flat pattern dimensions don’t match the folded part.

What Fabricators Actually Do

Shops handling incoming STEP sheet metal files follow one of three approaches:

Request native files. The cleanest outcome. SolidWorks (.sldprt), Inventor (.ipt), or Parasolid (.x_t) files retain the feature tree. The shop opens the file, checks the k-factor assignment against their gauge table, adjusts if needed, and exports their own flat pattern. No guessing. Most professional fabrication shops add this to their standard RFQ requirements.

Rebuild from scratch. For parts where the design will repeat, where forming tools are present, or where Insert Bends fails on the geometry, shops model natively from the STEP geometry as a reference. The rebuilt model uses the shop’s actual material thickness, bend radius, and gauge table from the start. More time up front; no corrections later.

Import, insert bends, correct. For simple parts — two to four bends, no formed features, no compound geometry — shops import the STEP, run Insert Bends, verify wall thickness against the material spec on the drawing, then manually set k-factor to their gauge table value. Faster than rebuilding. Acceptable risk for straightforward geometry. The key verification step: check that the flat pattern blank size makes physical sense before cutting anything.

Most shops doing volume fabrication won’t cut from a STEP flat pattern without at least a k-factor check. The flat pattern they trust is the one their CAM system produces from the rebuilt native model or from a corrected Insert Bends file.

Getting Clean DXF Flat Patterns from Corrected STEP Imports

Once k-factor is set correctly, the flat pattern export workflow is:

  1. Import STEP
  2. Run Insert Bends (or rebuild natively if Insert Bends fails)
  3. Set k-factor to your shop’s specification for that material
  4. Visually verify the flat pattern blank size is plausible
  5. Export DXF from the flat pattern view

CadShift handles step 5 in batch across an entire assembly: it exports flat patterns from every sheet metal component, with correct DXF layers (outer profile, bend lines, internal features), BOM quantities, and part numbers embedded in the DXF. That matters when you have 30 imported STEP parts that all need flat patterns corrected and exported.

The k-factor correction still has to happen before the export run — CadShift exports whatever flat pattern SolidWorks has computed. Set the manufacturing parameters correctly first, then batch export.