How to Design for Sheet Metal: A Practical DFM Guide
Design for manufacture (DFM) guide for sheet metal parts. Covers bend radii, hole spacing, tab design, relief cuts, and common mistakes to avoid.
Why DFM Matters for Sheet Metal
Designing a part that looks good in CAD is easy. Designing one that can actually be manufactured efficiently — without cracking, warping, or costing twice as much as it should — takes some understanding of the process.
Sheet metal fabrication typically involves:
- [Laser cutting](/services/laser-cutting) (or punching) the flat pattern
- Bending on a press brake
- Welding or fastening (if multi-piece)
- Finishing (deburring, coating, etc.)
Each step has constraints. Design within those constraints and you'll get better parts, faster, at lower cost.
Material and Thickness
Standard Thicknesses (mm)
Design to standard sheet thicknesses to avoid custom material orders and long lead times:
- [Mild steel](/materials/mild-steel): 0.8, 1.0, 1.2, 1.6, 2.0, 2.5, 3.0, 4.0, 5.0, 6.0, 8.0, 10.0, 12.0
- [Stainless steel](/materials/stainless-steel) (304/316): 0.8, 1.0, 1.2, 1.5, 2.0, 2.5, 3.0, 4.0, 5.0, 6.0
- [Aluminium](/materials/aluminium) (5052/6061): 0.8, 1.0, 1.2, 1.6, 2.0, 2.5, 3.0, 4.0, 5.0, 6.0
If your design calls for 2.3mm material, round to 2.5mm. The cost of non-standard material far outweighs the small weight difference.
Sheet Size
Standard Australian sheet sizes are typically 2400x1200mm or 3000x1500mm. Design your parts to nest efficiently within these sheets. A part that's 1250mm wide wastes almost half a sheet.
Bend Design
Bending is where most sheet metal design mistakes happen.
Minimum Bend Radius
The inside bend radius should be at least equal to the material thickness. Going tighter risks cracking, especially in stainless steel and aluminium.
| Material | Minimum Inside Radius |
|---|---|
| Mild steel | 1× thickness |
| 304 Stainless | 1× thickness |
| 5052 Aluminium | 1× thickness |
| 6061 Aluminium | 1.5–2× thickness |
Tip: If your design doesn't specify a bend radius, most fabricators will default to a radius roughly equal to the material thickness. This is generally the safest and most economical option.
Minimum Flange Length
The flange (the flat section after the bend) needs to be long enough for the press brake tooling to grip. As a rule:
Minimum flange = 4× material thickness + bend radius
For 3mm mild steel with a 3mm radius, that's 4×3+3 = 15mm minimum flange. Shorter flanges need special tooling and cost more.
Bend Relief
When a bend line runs into another feature (an edge, a tab, or another bend), you need a relief cut to prevent tearing.
A bend relief is a small slot or notch at the end of the bend line. It should be:
- Width: At least 1× material thickness (2× is safer)
- Depth: At least 1× material thickness past the bend line
Minimum Distance Between Bends
Parallel bends that are too close together can interfere with tooling. Keep at least 6× material thickness between bend lines (measured from the inside of one bend to the inside of the next).
Bend Orientation
Bending perpendicular to the rolling direction of the sheet produces better results (less risk of cracking). If bend orientation matters, note it on your drawing.
Hole and Feature Placement
Distance from Bends
Holes and features near a bend line will distort during bending. Keep all holes and cutouts at least 2× material thickness + bend radius away from any bend line.
For 3mm steel with a 3mm radius: minimum 9mm from the bend line.
Hole Size
Minimum hole diameter for laser cutting is generally about 0.5× material thickness, though smaller holes are possible at reduced speed. For best results, keep holes at least 1× material thickness in diameter.
Hole Spacing
The edge of a hole should be at least 2× material thickness from the edge of the sheet or from another hole. Closer spacing risks deformation or cracking during bending.
Slot Design
For slots, minimum width should be at least 1.5× material thickness. Very narrow slots in thick material are slow to cut and prone to heat distortion.
Tab and Slot Assembly
For parts that will be welded together, tab-and-slot joints provide self-fixturing — the parts locate themselves during assembly.
Tab Design
- Tab width: 1.5–3× material thickness
- Tab length: approximately equal to the slot part's material thickness
- Include 0.1–0.2mm clearance on each side of the tab for easy assembly
- Round the tab corners slightly to avoid stress concentrations
Slot Design
- Match the tab width plus clearance
- Slot length should exceed the mating material thickness by 0.5–1mm
Common Mistakes
1. Forgetting Bend Allowance
When sheet metal bends, the material stretches. The flat pattern is not simply the sum of the flange lengths — you need to subtract the bend allowance. Most CAD tools handle this automatically if you use the sheet metal module, but if you're drawing flat patterns manually, you need to account for it.
2. Non-Standard Bend Angles
90° bends are the most common and cheapest. Non-standard angles (e.g., 45°, 120°) may require special tooling. If you must use non-standard angles, call them out clearly on the drawing.
3. Tight Tolerances Everywhere
Sheet metal fabrication typically holds ±0.5mm on laser-cut features and ±0.5–1° on bends. Don't specify ±0.1mm unless it's truly needed — tighter tolerances mean more time, more inspection, and higher cost. See our Tolerance & Design Guide for achievable tolerances by process.
4. No Access for Fasteners
If you're using bolts, rivets, or PEM inserts, make sure there's enough clearance for the tool to reach the fastener. A nut that can't be reached with a spanner is a design problem, not a manufacturing problem.
5. Ignoring the Flat Pattern
Always check your flat pattern before sending a part for quoting. If the flat pattern has overlapping geometry, the part can't be made. Most CAD sheet metal tools will flag this, but it's worth verifying.
CAD Tips
- Use your CAD tool's sheet metal module — SolidWorks Sheet Metal, Fusion 360 Sheet Metal, Inventor Sheet Metal all produce accurate flat patterns with proper bend allowances.
- Export DXF for laser cutting — The flat pattern DXF is what the laser cutter uses. Make sure it's clean (no duplicate lines, no construction geometry).
- Export STEP for quoting — STEP files carry 3D geometry that allows instant quoting tools to automatically detect bends, measure cut lengths, and calculate pricing.
Get Your Parts Made
Upload your STEP or DXF file to our instant sheet metal quoting tool for immediate pricing on laser cutting and bending. We handle everything from single prototypes to production runs. For bend calculation details, see our guide on sheet metal K-factor. For DFM rules specific to laser cutting, see our Laser Cutting Design Guide. Want a rough price without a file? Try our Sheet Metal Cost Estimator. Get a quote →
Related Services
Need Parts Made?
Upload your CAD files and get instant pricing, or request a custom quote for any project.