SolidWorks Sheet Metal Design: From 3D Part to Flat Pattern

Why Sheet Metal Deserves Its Own Workflow

Sheet metal parts are not standard extrudes with thin walls. A standard solid model has no understanding of bend allowance, grain direction, or forming limitations. If you model a bracket as a thin boss-extrude with manually sketched bends, you will get the 3D shape roughly right — but the flat pattern will be wrong, and parts cut from that DXF will not fold to the correct dimensions.

SolidWorks Sheet Metal is a dedicated environment that understands bend geometry, material stretch, and manufacturing constraints. Use it for any part that starts as flat stock and is formed into shape.

The Base Flange: Where Every Sheet Metal Part Starts

The Base Flange/Tab feature creates the initial flat sheet. You sketch a profile — usually a simple rectangle or closed contour — and specify thickness and bend radius.

Key inputs at this stage:

• Thickness: the material gauge. Common values: 1.0, 1.2, 1.5, 2.0, 3.0 mm. Use a global variable here so you can change gauge across the entire part from one place.
• Bend radius: the inside radius of all bends. Standard practice is 1× material thickness for mild steel, 1.5× for stainless, 2× for aluminum alloy. Check with your fabricator — their press brake tooling may limit minimum radius.
• Sheet Metal Gauge Table: if your company has a gauge table (Excel file with thickness-to-radius mapping), link it here. This eliminates manual entry errors.

Edge Flange: Adding Bends to Existing Edges

Edge Flange folds a new flange from any existing straight edge. Select the edge, set the angle (most commonly 90°), the length, and the position (inside, outside, or material inside/outside).

The position option is frequently misunderstood:

• Material Inside: the new flange starts at the inner face of the base. The overall outside dimension grows by the flange length plus bend radius.
• Material Outside: the new flange ends at the outer face of the base. The overall dimension stays closer to the base dimension.
• Bend Outside: the bend starts at the outer face. Used when the base dimension is the controlling dimension.

When tolerances matter — and they always do in assembly — specify the position explicitly rather than accepting the default. The difference between Material Inside and Bend Outside can be several millimeters on a thick plate.

Bend Allowance, Bend Deduction, and K-Factor

When sheet metal bends, the material on the outside of the bend stretches and the material on the inside compresses. The neutral axis — the plane where no stretching or compression occurs — sits somewhere in between. The K-factor defines where that neutral axis is, expressed as a fraction of material thickness.

K-factor formula:

K = t / T

Where t = distance from inside surface to neutral axis, T = material thickness.

Typical values:

• Mild steel (soft): K = 0.44
• Cold-rolled steel: K = 0.42
• Stainless steel: K = 0.44 to 0.50
• Aluminum (soft): K = 0.40
• Aluminum (hard): K = 0.50

SolidWorks uses the K-factor to calculate bend allowance (BA), which is the arc length of the neutral axis through the bend:

BA = π × (R + K×T) × (angle / 180)

Bend deduction (BD) is the alternative representation: BD = 2×OSSB − BA, where OSSB is the outside setback. SolidWorks can work in either system — choose the one your fabricator uses and be consistent.

A wrong K-factor produces a flat pattern that is off by a predictable amount on every bent edge. If your first article comes back slightly short or long, recalibrate the K-factor based on the measured deviation and update the gauge table.

Miter Flange and Hem

Miter Flange creates a flange along multiple edges simultaneously, automatically mitering the corners where adjacent flanges meet. This is the right tool for box enclosures and channel profiles — far faster than placing Edge Flanges one at a time and manually trimming corners.

Hem folds a thin return edge for safety (eliminating sharp edges) or stiffness. Common hem types: closed (folded flat), open (180° with a gap), teardrop, and rolled. Specify the hem gap using your sheet metal standard — typically 0 to 0.5 mm for closed hems depending on material and forming method.

Forming Tools

Forming tools create embosses, lances, louvers, and dimples — features that cannot be represented as simple bends. SolidWorks includes a default forming tool library in the Design Library. You can also create custom forming tools from solid parts.

Important: forming tools must be applied in the correct orientation relative to the sheet surface direction. If the stopping face (the flat face that contacts the sheet) is oriented incorrectly, SolidWorks will place the feature on the wrong side. Always verify the resulting feature on both the formed view and the flat pattern.

Note that forming tools do not always flat-pattern correctly for complex shapes. Consult with your fabricator about formability and whether the flat pattern representation in SolidWorks matches their actual process.

The Flat Pattern

The flat pattern is the unfolded shape used for cutting. Access it via Insert > Sheet Metal > Flat Pattern, or by clicking the Flat Pattern feature in the tree. SolidWorks calculates the flat layout automatically based on K-factor and bend parameters.

To verify your flat pattern is correct before sending to production:

1. Check overall flat dimensions against hand calculations: flat length = leg1 + leg2 + BA (for a simple 90° bend).
2. Verify bend lines are positioned correctly. The bend line in the flat pattern shows where the press brake ram contacts the sheet.
3. Check that all holes and cutouts appear in the correct location in the flat pattern.

Exporting the Flat Pattern for Laser Cutting

The standard workflow:

1. In the part file, click the Flat Pattern feature to enter flat pattern state.
2. File > Save As > DXF or DWG.
3. In the DXF export options, select “Sheet Metal” export to get a clean single-layer flat pattern. Avoid exporting the 3D view — you want only the flat outline.
4. In the DXF options, specify the layers. Standard practice: outline on layer 0, bend lines on a separate layer (e.g., “BEND”), internal holes on another layer (e.g., “CUT”). Your laser cutting supplier will tell you their layer naming requirements — ask before your first order.

For plasma cutting or waterjet, the same DXF applies. For press brake forming, also provide a PDF drawing with bend sequence, bend angles, and the bend table from the drawing.

Common Design Mistakes

Key Takeaways

• Use SolidWorks Sheet Metal features — not Boss-Extrude with thin walls — for any bent sheet metal part. The flat pattern will be accurate only if the bend parameters are properly defined.
• Set K-factor based on your actual material and fabricator’s process. Default values are starting points, not production values.
• Export DXF from the Flat Pattern state, with bend lines on a dedicated layer, and confirm layer names with your laser cutting supplier before the first order.
• Keep holes at least 1.5×T from bend lines to prevent hole distortion during forming.
• Calibrate your flat pattern against a physical test bend before releasing production quantity.