If you’ve tried to get a flat pattern from a cylindrical collar in SolidWorks, you’ve hit this wall: the Sheet Metal toolbar’s normal workflow assumes you start flat and bend up. A cylinder was never flat. SolidWorks has no direct “unroll cylinder” command, and if you try to use the Convert to Sheet Metal tool on a solid cylinder, it either rejects the geometry or produces a body with wrong thickness.

The workaround that actually works is the Insert Bends method with an axial slit — and it produces a mathematically exact flat pattern, not an approximation. Here’s why it works and exactly how to do it.

Why a Cylinder Can Be Unrolled Exactly

A cylinder has zero Gaussian curvature. This means it’s a developable surface — it can be unrolled onto a flat plane without stretching or compressing the material. The flat pattern is exact, not an approximation. Gaussian curvature is the product of the two principal curvatures at any point; for a cylinder, one principal curvature is 1/R (around the circumference) and the other is 0 (along the axis). Zero product = developable.

This matters because SolidWorks sheet metal flat patterns are fundamentally about developable surfaces. The modeller knows how to unfold them — it just needs the geometry set up as sheet metal with an open edge to unroll from.

A sphere, a torus, or any double-curved surface is not developable. You cannot flatten those without material distortion. A cylinder and a cone are. If you’re working with a conical collar, the same method applies (SolidWorks will correctly produce the radial flat pattern for a cone).

The Problem with the Normal Sheet Metal Workflow

SolidWorks’ normal sheet metal workflow expects you to start from a planar sheet, add flanges and bends, and let the flat pattern fold back out. When you bring in a solid cylinder — or model one — the Convert to Sheet Metal feature has two requirements: a planar face to establish the thickness direction, and an edge to define the bend origin. A cylinder has neither.

The shelling approach people try first: create a solid cylinder, shell it to the wall thickness, then try to apply sheet metal to it. This gets you a tube, but SolidWorks doesn’t recognize it as a sheet metal body. The flat pattern option doesn’t appear in the feature tree.

The Insert Bends Method

The key insight: SolidWorks’ Insert Bends feature converts an existing thin-wall solid into a sheet metal body — but it requires an open edge to unfold from. You create that open edge with a very thin axial slit.

Step 1: Model the Cylinder

Model the cylindrical collar as a thin-wall solid. The typical approach:

  1. Revolve a closed profile (outer and inner diameter) 360°, or
  2. Revolve a surface then thicken it

Make the wall thickness exactly your design specification. SolidWorks will use this as the sheet metal gauge.

Step 2: Add the Axial Slit

This is the step that makes everything work. Cut a thin slot along the entire axial length of the cylinder:

  1. Create a plane containing the cylinder axis
  2. Sketch a very thin rectangle: 0.005mm to 0.01mm wide, full length of the collar
  3. Extrude Cut → Through All

The slit width should be less than 5% of the wall thickness to avoid affecting your flat pattern dimensions. With a 2mm wall, a 0.01mm slit is 0.5% — negligible. SolidWorks keeps this gap in the flat pattern, but it’s small enough to ignore for laser cutting or plasma cutting.

If the slit is too wide (approaching the material thickness), the Insert Bends step may fail with a topology error because the opening looks more like a missing face than an edge.

Step 3: Apply Insert Bends

Go to Insert > Sheet Metal > Insert Bends.

  • Fixed face: Select any flat annular face (the top or bottom of the collar). This is the reference face SolidWorks holds stationary during unfolding.
  • Bend radius: Set to your material’s minimum bend radius. For a rolled cylinder, this is typically set equal to the wall thickness (R = t) as a placeholder, but it doesn’t affect the flat pattern dimensions for a true cylinder since there are no discrete bends — the entire surface is the “bend.”
  • K-factor: Set your K-factor here. For a true cylinder with no bends, the K-factor doesn’t affect the flat pattern area — the cylinder unrolls at the neutral axis regardless. But SolidWorks requires the value to be set.

After confirming, SolidWorks adds a Flat-Pattern folder to the feature tree. The cylinder is now a sheet metal body.

Step 4: Add the Angled Cut

This is the order that matters. The angled cut must come after Insert Bends, not before.

If you apply the angled cut to the solid cylinder before converting to sheet metal, SolidWorks will struggle to unfold the angled end geometry. The cut edge is a planar ellipse on a cylinder — not a standard sheet metal form. After Insert Bends, the body is already recognized as developable sheet metal, and SolidWorks can correctly map the angled cut into flat pattern space.

To add the angled cut:

  1. Create a reference plane at the desired angle to the cylinder axis
  2. Cut Extrude using this plane as the cut face, or use a sketch on the angled plane

After the cut is applied, toggle the Flat-Pattern folder — the flat pattern updates to show the sinusoidal edge.

Understanding the Sinusoidal Edge in the Flat Pattern

The flat pattern of a cylinder with an angled cut through it has a sinusoidal (cosine-shaped) profile on the cut edge. This isn’t an approximation or a SolidWorks quirk — it’s exact geometry.

Why: When you unroll a cylinder of radius R onto a flat sheet, the circumferential direction becomes the x-axis of the flat. A plane inclined at angle θ from perpendicular to the cylinder axis intersects the cylinder at an ellipse in 3D space. That ellipse, when mapped onto the flat sheet, produces:

y(x) = h + R · tan(θ) · cos(x / R)

Where:

  • x is the position along the unrolled circumference (0 to 2πR)
  • y is the axial position on the flat
  • h is the axial height at the slit location
  • θ is the cut angle from perpendicular (0° = perpendicular cut, 90° = parallel to axis)

For a standard collar with a 45° angled cut and 50mm radius, the sinusoidal variation in the flat pattern is 50mm peak-to-peak (50mm · tan(45°) = 50mm). A 30° angle gives 28.9mm variation. This is the correct profile for the laser or plasma cutter to cut.

SolidWorks’ flat pattern should match this exactly. If it doesn’t, the model has a geometry error.

Exporting the DXF

Once the flat pattern is correct, export via File > Export > DXF/DWG with the flat pattern active, or use right-click the Flat-Pattern folder > Export to DXF/DWG.

For batch export from an assembly of multiple collars, CadShift handles this from the assembly level without opening each part individually — useful when you have varying collar heights or angles across a job.

Key DXF export settings for this geometry:

  • Geometry to Export: Exterior edges (solid lines). If you’re using a plasma cutter that needs lead-in clearance, also export bend lines as a separate layer (even though this part has no discrete bends, SolidWorks will include a bend line at the slit location).
  • DXF version: R2013 (DXF 2013) is safest for most laser/plasma CAM systems. See DXF R12 vs R2000 vs R2010 options if your CAM software has version requirements.
  • Export coordinate system: Match your CAM machine’s import coordinate system to avoid offsetting parts on import. This matters when nesting multiple collars from the same job.

API Approach for Batch Export

If you’re processing multiple collar parts programmatically, you can retrieve the flat-pattern body and export via the SolidWorks API:

// Get the flat-pattern folder from the active part
IPartDoc swPart = (IPartDoc)swModel;
IFlatPatternFolder fpFolder = (IFlatPatternFolder)swPart.GetFlatPatternFolder();

if (fpFolder != null && fpFolder.IsFlatPatternPossible())
{
    // Suppress all features above flat pattern (temporarily unflatten)
    fpFolder.Flattened = true;
    
    // Export DXF
    int errors = 0, warnings = 0;
    string dxfPath = outputDir + "\\" + partName + ".dxf";
    swModel.Extension.SaveAs(
        dxfPath,
        (int)swSaveAsVersion_e.swSaveAsCurrentVersion,
        (int)swSaveAsOptions_e.swSaveAsOptions_Silent,
        null, ref errors, ref warnings
    );
    
    // Restore to formed state
    fpFolder.Flattened = false;
}

The IFlatPatternFolder.Flattened property toggles the flat pattern on and off without manually suppressing features. IsFlatPatternPossible() returns false if the sheet metal body has geometry SolidWorks can’t unfold — use this to catch failed conversions in a batch run.

For more on the export settings available via API, see why DXF export settings don’t persist and the API fix.

Common Failures

Insert Bends fails with “could not create sheet metal body”: Usually caused by one of three things. The slit is too wide — try 0.005mm. The fixed face selected is not truly flat (it has a chamfer or small face adjacent to the slit edge). Or the cylinder has any non-manifold geometry from an upstream import — inspect with Geometry Analysis (Evaluate > Geometry Analysis) before attempting the conversion.

Flat pattern shows a straight edge instead of sinusoidal: The angled cut was applied before Insert Bends. SolidWorks couldn’t map the angled geometry correctly and approximated it as a straight line. Delete the cut, redo Insert Bends, then re-apply the cut in the correct order.

The flat pattern width doesn’t match 2πR: The model has a sketched arc instead of a revolve, meaning SolidWorks treated the cylinder as a series of flat faces. Check the feature tree — you should see a Revolve feature, not a series of extrudes. Alternatively, the K-factor is set incorrectly and shifting the flat pattern boundary. For a pure cylinder (no discrete bends), K-factor should have no effect on the outside perimeter — if it does, the geometry isn’t being recognized as a true developable surface.

The angled cut doesn’t show in the flat pattern: The cut feature is outside the scope of the sheet metal body’s flat pattern suppression chain. Check the feature order in the tree — Insert Bends must appear before the angled cut. If Insert Bends is below the cut in the tree, use Move/Copy Feature to reorder.

For sheet metal geometry that SolidWorks genuinely can’t model — compound-curved surfaces, truly non-developable geometry — the FreeCAD Sheet Metal workbench approach covers the alternatives including Rhino Squish for approximate unrolling.