Before I quote any sheet metal part, I check eight things: one thickness, one bend radius, flange lengths against the press brake die, hole and slot distances from bends, bend reliefs, the material and temper, the tolerances on the drawing, and whatever hardware or finish goes on afterwards.
Most sheet metal parts that cost too much fail on two or three of those, and nearly all of them are cheap to fix in CAD and expensive to fix at the shop.
Here's the checklist as I actually run it, with the numbers I use as a starting point. Your fabricator's tooling list beats any rule of thumb, so treat these as defaults to confirm, not law.
One thickness and one inside radius per part
A sheet metal part is cut from one sheet.
That sounds obvious, but I still get models where one flange is 2 mm and another is 1.5 mm, usually because two bodies were merged late in the design.
The same goes for bend radii. If every bend on the part uses the same inside radius, the shop runs one punch and one die for the whole part. Mix 1 mm and 3 mm radii and you've added a tool change, sometimes a second setup, and a chance to mix them up.
My defaults: inside radius equal to the material thickness for mild steel and stainless, and the same for 5052 aluminium. Then I stop and check the material callout, because of the next point.
Material and temper: the 6061-T6 problem
Last year a hardware startup sent me a 2 mm bracket in 6061-T6 with tight inside bends, drawn exactly like a steel part. It looked fine in CAD. It would have cracked on the outside of every bend.
6061 in the T6 temper doesn't like being bent tight. You need a much larger radius (often three times the thickness or more, depending on the supplier), or you switch to 5052-H32, which bends happily at around one times thickness and is what most shops stock for formed aluminium anyway. We switched. The part got cheaper and the strength was still more than enough for a bracket holding a PCB.
So the material question comes early in my review, not at the end. Stainless (304 vs 316), galvanised vs plain mild steel, and grain direction on brushed finishes all change what the part can do and what it costs.
Flange length against the die you'll actually get
A flange has to be long enough to sit across the V-die while it bends.
Too short and it slips into the die, and the bend comes out wrong or not at all.
The quick rule I start from is a minimum flange of about four times the thickness, measured from the outside of the bend. For 2 mm steel that's roughly 8 mm, though many shops would bend that on a 12 or 16 mm V-die and want 10 to 12 mm to be comfortable. If a design genuinely needs a 6 mm flange on 2 mm stock, that's a conversation with the shop, not an assumption.
Short flanges are the single most common reason I see a "we can't bend this as drawn" reply.
Holes, slots and cutouts near bends
Put a hole too close to a bend and it stretches into an oval when the part is formed.
A slot running parallel to a bend line can pull and distort the whole edge.
My defaults, in thickness units (T) and inside radius (R):
- Hole edge to the bend: at least 2.5T plus R. Closer than that, expect distortion or a hole that has to be drilled after forming.
- Hole diameter: at least T, so a 1.5 mm hole in 2 mm steel is asking for a broken punch on a turret or a fussy laser cut.
- Hole to the sheet edge: at least 1.5T to 2T.
- Hole to hole: at least 2T.
If a hole really has to sit near a bend (a fixing point, a cable gland), a relief slot or cutting the hole after forming is cheaper than arguing with physics.
Bend reliefs and corners
Where a bend runs into an unbent edge, the material tears unless there's a relief cut. CAD tools add these automatically, and the automatic ones are usually fine. Check them anyway.
A relief at least as wide as the thickness and running past the bend by about T plus R is the default I use. For corners where two flanges meet, decide whether you want a small gap, an overlap or a welded closed corner, and say so on the drawing. "Closed corner" without saying how it gets closed is a quote the shop will pad.
Tolerances that sheet metal can actually hold
This is where I push back hardest, and it's counter-intuitive for people coming from machined parts.
Laser-cut features on a flat blank are accurate, typically around ±0.1 to 0.2 mm. Once you bend, every bend adds its own error, often in the region of ±0.5 mm and ±1° per bend on standard work. Dimensions that cross two or three bends stack those errors.
I came into sheet metal from microfluidics, where I was assembling parts to a 5 micrometre CNC tolerance. That background makes me more relaxed about sheet metal, not less, because I've seen what holding a tight number really costs. If a sheet metal assembly needs a precise fit, I put the precision in features on the same flat face (two holes cut in one operation) and dimension from them, instead of asking for ±0.1 mm across three bends.
The manufacturing drawing checklist goes into datums and how to dimension so the shop measures what you care about.
Hardware, welds and finish
Self-clinching nuts and studs need a minimum sheet thickness and a minimum distance from the edge, both listed by the fastener maker. I check every insert against its datasheet. A clinch nut that needs 1.5 mm sheet will not hold in 1 mm, however neat it looks in the model.
Welds: can a fold do the job instead? A folded and riveted corner is often cheaper and stays flatter than a welded one. If it has to be welded, tabs and slots that locate the parts against each other save fixture time.
Finish: powder coat adds roughly 60 to 100 micrometres per surface, more on edges. That eats into fits on slots and tabs, and threads need masking. If a lid slides into a coated housing, model the clearance after coating, not before.
What I'd actually send with a sheet metal RFQ
A STEP of the formed part. A flat pattern as DXF, with bend lines on their own layer. A PDF drawing with material and temper, thickness, the inside radius, finish, hardware callouts and only the tolerances that matter. Quantity, because 10 parts and 500 parts get very different process choices.
That's it.
I model in Fusion 360 and deliver SolidWorks-compatible files, so the flat pattern and the 3D model come from the same sheet metal rules and the K-factor isn't a guess.
The broader DFM checklist covers machined, molded and printed parts as well, and the DFM review page explains what a full review includes. If you've got a sheet metal part heading to a shop and want a second pair of eyes first, you can request a free initial DFM review of one part.