Sheet Metal Prototyping: Design Rules That Cut Cost and Lead Time
Most sheet metal prototypes cost more than they should because of a handful of design choices:
bends too tight for the material, holes too close to a bend, missing bend reliefs and tolerances tighter than the process can hold. Fix these in CAD and the same part is cheaper, faster to make and more likely to be right first time.
These rules come from what our sheet metal shop sees every week on incoming drawings. None of them limit your design; they keep it inside what press brakes and laser cutters do well.
Key Facts
- HLH makes sheet metal prototypes with a minimum order quantity of one.
- A safe inside bend radius is at least equal to the material thickness.
- Holes should sit at least 2.5 times the material thickness plus the bend radius away from a bend.
- Laser-cut features typically hold about ±0.1 mm; dimensions across bends typically hold ±0.25 to
±0.5 mm. - Powder coating adds roughly 0.06 to 0.1 mm per surface, which affects tight fits.
Why Do Design Rules Matter for a Prototype?
A sheet metal prototype is made with the same press brakes, lasers and punches as a production part, so it follows the same physics. A feature that is awkward to bend in production is just as awkward to bend once. The difference is that on a prototype the extra setup time lands on one or two parts, so the cost per part rises sharply.
Designing to these rules from the first prototype also means the design you approve is one you can produce in volume without a redesign.
Keep One Thickness Throughout the Part
Sheet metal parts are cut from a single flat sheet, so every wall has the same thickness. If a feature needs to be stiffer, add a flange, a rib or a hem rather than thickening the wall. If two areas truly need different thicknesses, design them as separate parts joined by welding, rivets or self-clinching hardware.
Pick thicknesses that are stocked. Standard gauges in aluminum 5052, cold-rolled steel and 304
stainless ship fastest.
Use Bend Radii the Tooling Already Has
Set the inside bend radius to at least the material thickness. Tighter radii can crack the outside of the bend, especially in harder aluminum such as 6061-T6, which is why 5052 is the usual choice for bent aluminum parts.
Use the same radius on every bend if you can. One radius means one set of tooling and no changeovers, which is one of the simplest ways to shorten lead time on rapid sheet metal prototyping.
Give Flanges Enough Length to Bend
A press brake needs something to grip. Make each flange at least four times the material thickness long. Short flanges slip in the tool and come out with an inconsistent angle, or need a special process that adds cost. If a design needs a very short lip, consider cutting it longer and trimming it after bending, or ask us about alternatives before the drawing is final.
Keep Holes and Slots Away From Bends
Holes placed too close to a bend line stretch into ovals when the metal is formed. Keep holes at least 2.5 times the material thickness plus the bend radius away from the bend. Slots and cut-outs need a little more room.
Make hole diameters at least equal to the material thickness. Smaller holes can be cut by laser, but they are harder to keep clean and may need deburring by hand.
Add Bend Reliefs Where Bends Meet an Edge
Where a bend ends partway across a sheet, the metal tears unless it has somewhere to go. A small rectangular or round relief cut at the end of the bend solves this. Make the relief at least as wide as the material thickness and deep enough to pass the bend radius.
Corners where two flanges meet need a corner relief too. Without it, the flanges collide or bulge.
Set Tolerances the Process Can Hold
Laser cutting holds about ±0.1 mm on flat features, but each bend adds variation. Dimensions measured across one or more bends typically hold ±0.25 to ±0.5 mm. Calling for ±0.05 mm across three bends on a prototype sheet metal enclosure forces extra inspection, rework and cost.
Put tight tolerances only where they affect function, such as mounting holes for a PCB, and dimension those features from the same flat face where possible. Leave the rest at a general tolerance.
For mating parts, tolerance the fit, not every dimension: slotted holes on one part often absorb the
variation that would otherwise need a tight tolerance on both.
Choose Hardware and Joining Early
Self-clinching nuts, studs and standoffs give strong threads in thin sheet, but they need minimum edge distances and a specific hole size. Specify the hardware part numbers in the drawing so the holes are cut right the first time.
Welding adds labor, heat distortion and finishing time. Where you can, use tabs and slots, rivets or hardware instead, and keep welds for joints that truly need to be sealed or structural.
Plan for Finishing From the Start
Powder coat, anodizing and plating all add thickness. Allow for it on sliding fits, threaded holes and mating parts, and mark any surfaces that must stay bare for grounding.
If the prototype is meant to prove the production part, make it from the same material and finish.
Metal rapid prototyping in a substitute material can hide problems with forming, corrosion or fit that appear later.
Stick to Standard Hole Sizes and Features
Punched holes, louvers, embosses and countersinks are fastest when they match tools the shop already holds. Use common metric or imperial hole sizes, and avoid one-off diameters that differ from a standard size by a few hundredths of a millimeter.
Formed features such as louvers, lances and embosses need distance from bends and edges too, usually at least three times the material thickness. If a feature is only cosmetic, ask whether it could be laser-etched or printed instead of formed.
Countersinks in thin sheet are a frequent problem. If the sheet is thinner than the countersink depth, the hole becomes a knife edge. Use a dimpled countersink, a thicker sheet or a pan-head fastener instead.
Think About Grain Direction and Springback
Rolled sheet has a grain. Bends made across the grain are stronger and less likely to crack than bends made along it, which matters most on tight radii in aluminum and stainless steel. If a part has bends in two directions, a slightly larger radius helps both.
Every material springs back a little after bending. Press brake operators compensate for it, but very long flanges, high-strength steels and thin aluminum spring back more. Allow for this in angle tolerances, which are typically ±1° for prototype parts.
Prototype the Way You Plan to Produce
Prototypes are often laser cut and press brake formed, while production parts in large volumes may be punched or stamped. If you already know production will use stamping dies, tell us. We can keep the prototype geometry compatible with that process, so the parts you test are a true preview of
production.
For low and mid volumes, the prototype process is often the production process too. HLH makes sheet metal parts from one unit to low-volume batches on the same equipment, so a design that works as a prototype can move straight into production.
What Should You Send With Your Sheet Metal Quote?
Send a 3D STEP file and a 2D drawing showing material, thickness, finish, hardware and critical tolerances. A flat pattern helps but is not essential, as our engineers can unfold the part. Add your quantity and target date.
Before quoting, our engineers review the design for manufacturability and flag any of the issues above, with suggested fixes. Most can be changed in minutes in CAD.
Frequently Asked
What is the most common mistake on sheet metal drawings?
Tolerances that are too tight across bends, followed closely by holes placed too near a bend line.
Can you make just one sheet metal prototype?
Yes. HLH’s minimum order quantity for sheet metal parts is one unit.
Q: Which aluminum is best for bent parts?
5052 is the usual choice because it bends without cracking; 6061-T6 is stronger but needs larger bend radii.
Do I need to supply a flat pattern?
No. A 3D model is enough for us to create the flat pattern, though your own flat pattern is welcome as a reference
Have a sheet metal enclosure, bracket or chassis to prototype? Upload your CAD file at hlhprototypes.com for a free quote and project review, email FreeQuote@HLHPrototypes.com or call +86 755 8256 9129 (ext. 817 for English).