The Real Cost Drivers in Sheet Metal Prototyping
Sheet metal parts look simple on a drawing — a flat blank, a few bends, some holes. In reality, the difference between a $12 prototype and a $40 prototype often comes down to decisions made before the first laser fires. At Protom, we run CNC machining and sheet metal side by side, and the cost logic is surprisingly different. Metal machining charges for material removal. Sheet metal charges for setup, tooling, and handling.
If you are ordering five pieces of a bracket, the laser cutting time might be under two minutes per part. The setup — loading the program, nesting the blank, calibrating the head — can take twenty. That means your per-part cost is dominated by setup, not cycle time. The lesson is obvious: consolidate prototypes into slightly larger batches when possible. Ten parts often cost only 30–40 percent more than five.
Bend Radius and K-Factor: Get Them Right Early
Every bend has a minimum radius determined by material and thickness. Go too tight and you get cracking on the outside of the bend. Typical minimums:
- Cold-rolled steel (CRS), 1.5 mm: 1.5× material thickness = 2.25 mm inside radius.
- 304 stainless, 2 mm: 2× thickness = 4 mm minimum. Stainless work-hardens aggressively; tighter bends need heat or grain direction awareness.
- 5052-H32 aluminum, 1.6 mm: 1× thickness = 1.6 mm. Softer alloys allow tighter bends than steel.
The K-factor — the ratio of the neutral axis to thickness — determines flat pattern length. A K-factor of 0.5 means the neutral axis sits at mid-thickness. In practice, it ranges from 0.42 to 0.5 depending on radius and material. Use 0.45 as a safe starting point for CRS, but verify with a test bend if your flange length tolerance is under ±0.2 mm. Nothing ruins a prototype faster than a flat blank that is 1 mm too short after forming.
Hole Placement Rules That Save Rework
Holes too close to a bend line distort during forming. The rule of thumb is: hole edge to bend line should be at least 2× material thickness plus the bend radius. For a 2 mm CRS part with a 3 mm inside radius, keep holes at least 7 mm from the bend tangent line. Closer than that, and the hole will ovalize or tear.
Similarly, avoid placing holes on the bend itself. It is possible with special tooling, but it adds cost and often weakens the joint. If you need a through-hole on a folded flange, design it on the flat face and accept the offset after bending, or switch to a welded nut.
Tab width matters too. Narrow tabs — under 3× thickness in width — tend to twist or deform during bending. If your design needs a narrow locating tab, add a gusset or increase width and trim afterward.
Nesting and Material Yield
Laser and punch machines cut from standard sheets: 1,000 × 2,000 mm or 1,250 × 2,500 mm are common. A good nest fits your parts with minimal skeleton waste and keeps grain direction consistent. For cosmetic parts, grain direction should run parallel to the longest visible edge; otherwise you will see streaks after brushing or anodizing.
Small parts can sometimes be tabbed together in the nest and broken apart after forming. This reduces handling but adds a small cleanup operation. For prototypes under ten pieces, manual breakout is usually fine. For fifty or more, plan for a deburring step.
Finish Options and Their Trade-offs
Sheet metal prototypes rarely ship as-cut. The most common finishes:
- Deburr only: Removes sharp edges and dross. Fastest, cheapest. Good for hidden brackets.
- Bead blast + clear coat: Uniform matte appearance, light corrosion resistance. Popular for aluminum panels.
- Powder coat: Durable, thick (60–80 µm), available in any color. Adds a day or two for masking and curing. Not ideal for tight-tolerance interfaces because the coating thickness must be factored into holes and slots.
- Anodize (Type II): Hard, thin (5–15 µm), electrically insulating. Best for aluminum that needs wear resistance without dimensional change. Type III is thicker and more abrasion-resistant but can close small holes.
If your part needs both powder coat and a precise press-fit bore, specify the bore as a masked area or plan for post-coat reaming. Reaming after coating adds cost but saves assembly headaches.
When to Choose Sheet Metal Over CNC Machining
There is a crossover point. Thin-walled enclosures, brackets, and chassis are usually cheaper in sheet metal. Solid blocks with complex 3D geometry, tight bores, or threaded features are better machined. A good rule: if the part can be unfolded into a flat pattern with uniform thickness, try sheet metal first. If the thickness varies or you need blind holes and pockets, machining is the safer path. For parts with complex internal geometry and higher volumes, die casting can sometimes beat both sheet metal and machining on per-unit cost, though it requires upfront tooling investment.
Hybrid approaches work too. A sheet metal chassis with CNC-machined mounting bosses welded in gives you the light weight of formed metal and the precision of machined interfaces. Just watch your weld distortion near critical datum features.
Final Checklist for Your Next RFQ
Before sending a sheet metal prototype request, confirm:
- Material, thickness, and temper are specified.
- Bend radii respect minimums for that material.
- Holes and slots are at least 2×T + R from bend lines.
- Flat pattern tolerances account for K-factor variation.
- Finish is defined, including masked areas if needed.
- Grain direction is noted for cosmetic faces.
Getting these right on the first drawing saves one to two days of back-and-forth and often cuts prototype cost by 20 percent or more. At prototype volumes, setup time is the enemy. Design to reduce it, and your quotes will reflect the difference.
