This sheet metal design checklist covers the 15 checks we'd run on your drawing anyway: material, cut features, bends, joining, finishing, and the file itself. Do them before you send it and most quotes go straight through without a single email back and forth.
Each check is a practical rule of thumb, not a law. Shops, materials, and machines differ, and sometimes a part has a good reason to break a rule. But if you break one, break it on purpose and mention it on the quote. Work through the groups in order; the early decisions (material and thickness) change the numbers in the later ones.
Material and thickness (checks 1–3)
1. Is the material right for where the part lives?
Indoor and painted: mild steel is usually fine. Wet, industrial, and nobody's admiring it: look at 3CR12. Visible bare stainless or food contact: 304. Near the sea or around chlorides: 316 or a coated part. Light weight: aluminium. If you're unsure, say so on the quote and ask.
2. Is the thickness given in millimetres?
Write "2 mm", not "14 gauge". Gauge numbers mean different thicknesses for steel and aluminium, and South African suppliers sell sheet by the millimetre.
3. Is it one thickness per part?
A sheet metal part is cut from one sheet, so every flange on a bent part is the same thickness. If one area needs to be thicker, it's a separate part that gets welded or bolted on.
Cut features (checks 4–7)
4. Are holes at least as big as the material is thick?
A good starting rule is hole diameter at least equal to material thickness. A 3 mm hole in 3 mm steel is fine; a 2 mm hole in 4 mm steel is asking for trouble. Small holes in thick plate may need drilling instead.
5. Are slots and webs at least one thickness wide?
Narrow slots and thin bridges between features distort from the heat of the cut. Keep them at least one material thickness wide, more on thick plate.
6. Are features at least one thickness from an edge?
A hole 1 mm from the edge of a 3 mm plate leaves a thin sliver of metal that can bulge or tear. Keep holes and slots at least one thickness away from any edge.
7. Are parts drawn at finished size?
Don't offset lines to allow for the laser beam. The cutting software compensates for kerf. If you do it too, holes come out oversize.
Bends (checks 8–11)
8. Is the inside bend radius realistic?
As a starting point, use about 1× thickness for mild steel and soft aluminium, 1.5–2× for stainless, and more for hard aluminium like 6082-T6. A sharp 0 mm inside corner on a bent part isn't realistic on a press brake.
9. Are flanges long enough?
The flange has to reach across the V-die to be bent. A practical rule is a minimum flange of about 4× thickness, so roughly 8 mm on 2 mm sheet. Shorter flanges may need special tooling or a different design. Our post on minimum flange length explains why.
10. Are holes far enough from bend lines?
Holes too close to a bend stretch into ovals. Keep them at least about 2.5× thickness plus the bend radius from the bend line. On 2 mm mild steel with a 2 mm radius, that's around 7 mm.
11. Is there bend relief where a bend meets an edge?
Where a bend runs into an uncut edge, the metal tears or bulges. A small relief cut, about one thickness wide and extending at least one thickness past the bend line, solves it.
Joining and finishing (checks 12–14)
12. Is every weld necessary?
Each weld adds labour and distortion. Could two welded pieces be one bent part? Could a continuous weld be stitched? Mark which welds are visible and which are hidden.
13. Are critical dimensions marked, and the rest relaxed?
Welding and bending both move metal. Mark the two or three dimensions that must be exact, such as mounting holes, and allow a general tolerance on everything else. Tight tolerances everywhere cost more and often aren't achievable on a welded part.
14. Is the finish specified, with masking?
State raw, brushed, painted, or powder coated, and give the colour as a RAL code or name. Powder coating typically adds around 60–80 µm per coat, enough to clog threads and tight fits. Mark threads, bores, and contact faces to mask. Our guide to masking for powder coating covers what usually needs it.
The file (check 15)
15. Is the file clean and complete?
For flat parts: a DXF at 1:1 in millimetres, closed outlines, no duplicate lines, no dimensions or title blocks in the cut file. For bent parts: a STEP model of the folded part, or a flat DXF with bend lines on their own layer plus a PDF showing bend directions. For assemblies: a drawing with a parts list. Name files sensibly, with material, thickness, and quantity. Our post on preparing a DXF for laser cutting goes through the file checks step by step.
The checklist at a glance
| # | Check | Quick rule of thumb |
|---|---|---|
| 1 | Material suits environment | Say "not sure" if unsure |
| 2 | Thickness in mm | No gauge numbers |
| 3 | One thickness per part | Thicker areas are separate parts |
| 4 | Hole size | Diameter ≥ thickness |
| 5 | Slots and webs | Width ≥ thickness |
| 6 | Edge distance | ≥ 1× thickness |
| 7 | Finished size | No kerf offset |
| 8 | Bend radius | About 1T mild steel, 1.5–2T stainless |
| 9 | Flange length | About 4T minimum |
| 10 | Hole to bend | About 2.5T + radius |
| 11 | Bend relief | About 1T wide, 1T past the bend |
| 12 | Welds | Only where needed |
| 13 | Tolerances | Mark critical ones only |
| 14 | Finish and masking | RAL code, mask threads |
| 15 | File | Clean DXF or STEP, sensible name |
Sending it for a quote
Once the checks are done, upload your files with the material, thickness, quantity, and finish. The quote form takes DXF, DWG, STEP, PDF, or a photo up to 10 MB. If a check didn't pass and you're not sure how to fix it, send it anyway with a note; it's easier to solve at quote stage. See our laser cutting service for materials, or start a quote and add bending, welding, and coating to the same order.