Sheet metal is the most cost-sensitive process to model correctly. A drawing with imprecise bend allowances or a DXF with overlapping lines forces our partner to either ask questions (slowing the quote) or guess (creating rework risk). Both outcomes are fixable in the design phase.
K-factor and bend allowance fundamentals
The K-factor describes where the neutral fiber sits inside the bend. If your CAD package uses a generic K of 0.44 you will be close on aluminum and mild steel but off on stainless or thicker stock. Use the values below as starting points and refine based on supplier feedback.
| Material | Thickness | Inside radius | K-factor |
|---|---|---|---|
| Aluminum 5052 | ≤ 1.5 mm | = thickness | 0.40 |
| Aluminum 5052 | 1.5 - 3 mm | = thickness | 0.43 |
| Mild steel 1008/CR4 | ≤ 2 mm | = thickness | 0.42 |
| Stainless 304 | ≤ 2 mm | 1.5x thickness | 0.45 |
| Stainless 304 | 2 - 3 mm | 1.5x thickness | 0.47 |
Minimum bends, holes, and edges
- Minimum hole diameter: ≥ thickness; tighter than that requires drilling instead of laser piercing.
- Minimum hole-to-edge distance: 2x thickness.
- Minimum hole-to-bend distance: 3x thickness from the bend tangent line.
- Minimum bend-to-bend distance: 6x thickness, plus the bend radii.
- Bend reliefs: at least thickness wide and 1.5x thickness deep.
Forgetting reliefs at the corners of a bend that meets an edge is the #1 reason for cracks in stainless and aluminum. Add them in CAD before exporting flat patterns.
DXF hygiene
Most laser shops will only cut clean DXFs. Clean means closed contours, no overlapping lines, no zero-length segments, and no spline-only curves where polyline-arc representations are expected. The Uretyco platform runs an automated check on upload and surfaces issues before quoting.
- Use millimeters and explicitly set units in the DXF header.
- Convert splines to polylines when possible; complex splines slow down the laser controller.
- Place text and dimensions on a separate layer so they can be ignored by the cutter.
- Provide flat-pattern DXF plus a 3D model with bend annotations for any non-trivial part.
Realistic tolerances
| Feature | Achievable tolerance |
|---|---|
| Cut edge length (laser) | ±0.10 mm |
| Hole diameter (laser) | ±0.10 mm; for fits, drill instead |
| Bend angle | ±1° standard, ±0.5° on request |
| Flatness on parts > 300 mm | 1-2 mm warp possible |
| Hole position after bend | ±0.3 mm typical |
Edges and finishes
Laser-cut edges are slightly oxidized; ask for deburr if the part is handled. Powder coat and zinc plating are the most common downstream finishes. For stainless, brushed grain finish is a popular default.
Pre-upload checklist
- 1Export flat-pattern DXF
Closed contours, no overlapping lines, mm units.
- 2Provide STEP with bends
Helps suppliers verify the flat pattern matches the 3D model.
- 3Annotate bend lines and angles
Down-bend vs up-bend, angle in degrees, inside radius.
- 4Specify material and grain
Grade, gauge or thickness, grain direction if cosmetic.
- 5Call out finishes and hardware
Powder coat, plating, PEM inserts, weld nuts, hardware BOM.
Related articles
Can't find what you need? Contact our team for expert assistance with your manufacturing project.