When you cut a hole on a bent face in SolidWorks, you get a circular feature in 3D. When you flatten the part, that same hole can appear as an ellipse in the flat pattern — and that ellipse is what gets exported to your DXF and sent to the laser cutter. The laser punches an ellipse. Your hole doesn’t fit the fastener.

This isn’t a bug. It’s geometry. But the fix is straightforward once you understand what’s happening.

Why Bent-Face Holes Become Ellipses

A circular hole cut perpendicular to a bent face sits at an angle relative to the sheet’s neutral axis. When SolidWorks unfolds the bend, it unrolls the material around the bend radius — and that unrolling stretches any geometry that was cut into the angled face.

The math: for a hole of diameter d on a face inclined at angle θ from the flat base plane, the flat pattern produces an ellipse with:

  • Minor axis = d (unchanged, parallel to the bend axis)
  • Major axis = d / cos(θ)

At 90° — a standard right-angle flange — cos(90°) = 0, which breaks the formula. In practice, holes placed exactly on the bend radius flatten to shapes that depend on their position along the arc length of the bend. Holes that straddle a bend can produce very distorted outlines.

Holes on flat faces (not on bends, not crossing bends) are unaffected. They remain perfectly circular in the flat pattern because unfolding flat-face geometry involves no stretching.

The three cases where you get distortion:

  1. Hole center on a bent face — the entire hole is on the flange or on the flanged portion of the radius. The resulting flat pattern geometry is an ellipse.
  2. Hole crossing the bend tangent line — part of the hole is on the flat base, part on the radius. This produces a kidney-bean outline in the flat pattern — non-circular and non-elliptical.
  3. Hole on the bend radius itself — the hole straddles the actual bend zone. Flat pattern result is geometry that SolidWorks may flag as invalid, depending on bend radius vs hole size ratio.

The Wrong Way to Fix This

The instinct is to place the hole on the flat portion of the flange, set back from the bend tangent line. That works, but it changes your part geometry — the hole moves, which may violate your assembly constraints.

The second wrong approach: modeling the hole as an ellipse in the flat pattern sketch and expecting it to appear circular in 3D. That only works for the inverse case — when you need a specific 3D shape that depends on the flat stock geometry. It doesn’t help when you need a true circular hole in the folded part.

The Correct Fix: Unfold → Cut → Fold

SolidWorks provides Sheet Metal > Unfold and Sheet Metal > Fold specifically for this workflow. The logic:

  1. Unfold the relevant bend(s) before cutting the hole
  2. Cut the hole on the unfolded (flat) geometry
  3. Fold the bend back

When you cut on flat geometry, the hole is circular in the flat state — and because it was cut flat, SolidWorks carries that flat circle through the fold and produces a circular hole in the folded 3D model. The flat pattern DXF exports the circle correctly.

Step by step in SolidWorks:

1. Sheet Metal toolbar > Unfold
   - Select the stationary face (the face that doesn't move)
   - Select the bend(s) to unfold
   - OK

2. Sketch > create a hole sketch on the now-flat face
   Extruded Cut (Through All) to cut the hole

3. Sheet Metal toolbar > Fold
   - Same stationary face
   - Same bend(s)
   - OK

The Unfold and Fold features appear in the FeatureManager tree as paired items. If you later modify the hole sketch, SolidWorks updates the flat pattern automatically — the Unfold/Fold pair is fully parametric.

What you see in the feature tree:

Sheet-Metal
Base-Flange
Edge-Flange1
Unfold1           ← unfolds the edge flange bend
Cut-Extrude1      ← hole cut on flat geometry
Fold1             ← folds back
Flat-Pattern

Verifying It Worked

Check the flat pattern before exporting. In the ConfigurationManager, activate the Flat Pattern configuration or right-click the Flat-Pattern feature and choose Unsuppress. Your hole should appear as a circle, not an ellipse.

If the hole is still an ellipse, check the feature order: the Cut-Extrude must fall between the Unfold and Fold features in the tree. If the cut is above the Unfold, it’s being applied to 3D geometry before unfolding happens.

Multi-Body Sheet Metal Parts and the Flat Pattern Limit

This is a separate but related pain point: in a multi-body sheet metal part, SolidWorks creates one flat pattern feature per body. The flat patterns are sequential — there’s no way to simultaneously flatten all bodies at once in the native feature tree.

What this means for DXF export: when you use File > Save As > DXF with a multi-body sheet metal part, SolidWorks only exports the active flat pattern (the currently unsuppressed one). Automating batch DXF export from multi-body parts requires either:

  • A macro that cycles through bodies, activates each flat pattern, exports, moves to the next
  • The Save Bodies command (Insert > Features > Save Bodies) to split the multi-body part into individual part files, then batch export each

CadShift handles both patterns. If your assembly contains individual sheet metal parts (not multi-body), CadShift exports all flat patterns in a single pass with no manual cycling. For multi-body configurations from weldments or complex formed parts, the Save Bodies split-first approach gives clean, predictable results.

The Hole Wizard Case

If you used Hole Wizard for your holes (not a simple Cut-Extrude), the same Unfold/Fold workflow applies. Hole Wizard creates a 3D sketch for hole positioning. When used after Unfold, the 3D sketch positions the hole on the flat face, and the result folds correctly.

The one gotcha: Hole Wizard on a bent face places the hole perpendicular to the face normal — which means perpendicular to the bent face, not perpendicular to the flat stock. If perpendicularity to the flat stock matters for your assembly (most fastener holes), use Unfold first, then Hole Wizard.

When to Just Move the Hole

Not every hole needs the Unfold/Fold treatment. If your manufacturing process is punch-press rather than laser cut, the tooling typically punches holes in the flat state regardless — so the flat pattern circle is what matters, and the 3D “hole” is derived geometry anyway.

For laser cutting and waterjet cutting, the DXF flat pattern is the manufacturing input. Any distortion in the flat pattern geometry goes directly to the machine. These processes need circular holes in the flat pattern.

For CNC drilling of formed parts (drill after forming), the hole location needs to be correct in 3D, and the flat pattern is informational rather than the machining input. In this case, the ellipse in the flat pattern is technically correct — it shows where the drill bit would have entered if you’d drilled the flat blank.

Understanding which process you’re feeding changes whether the ellipse is a problem or a correct representation.

Holes That Cross the Bend Tangent Line

When a hole partially intersects the bend tangent line — part of the hole is on the flange, part on the flat base — the flat pattern produces a notch or kidney shape. This is almost always unintentional.

Fix: check hole placement against the bend tangent line before cutting. SolidWorks doesn’t warn you when a hole crosses the tangent line, but the flat pattern DXF will have unusual geometry that’s immediately visible.

The minimum safe distance from hole edge to bend tangent line depends on your bend radius and material:

  • General rule: hole distance from bend ≥ 2× material thickness + bend radius
  • Below this distance, the material may tear or deform during bending even if the flat pattern looks clean

This distance rule is also why CadShift’s DXF layer output includes separate sketch geometry — your fabricator can check clearances without re-measuring from the finished DXF.

Summary

  • Holes cut on bent faces in SolidWorks produce ellipses in the flat pattern — this is correct geometry, not a bug
  • Fix it with the Unfold → Cut → Fold sequence: cut the hole while the material is flat, fold back after
  • Holes on flat faces (not on bends) are unaffected
  • Holes crossing the bend tangent line produce kidney-shaped notlines — avoid them
  • Multi-body sheet metal parts require manual flat pattern activation or Save Bodies before batch DXF export

If you’re batch exporting DXF flat patterns from a large assembly, verify each part’s flat pattern configuration once before running the batch — a single part with an elliptical hole that should be circular will come back from the fabricator as a defect.