Prototype versus production design: what tooling changes

A prototype bracket arrives in ten days, fits, and the programme moves to production. Six weeks later the tool is cut and the first parts do not fit. The holes are in the same place to within 0.1 mm, the bend heights are 0.4 mm short, and the material is the grade the mill had rather than the grade on the drawing.

That gap is normal, and it is a design problem rather than a toolmaking problem. The prototype was made by laser and press brake, where every part can be adjusted one at a time. Production is made by a die, where the first part and the fifty-thousandth have to be the same part with no operator in between.

This comparison of prototype versus production design for sheet metal sets out what actually changes when tooling arrives, the numbers behind each change, and the drawing decisions that have to move before the die is cut. The design rules behind those decisions sit in the Design and CAD hub.

What changes when a prototype becomes a production part?

Six things change: the process, the hole strategy, the radii, the tolerance distribution, the flat pattern and the material grade. The interfaces should not change.

The process change is the root of the other five. A laser cuts any contour in any order with no tooling, and a brake bends one feature at a time with a programmable angle. A die does all of it in one stroke, in a fixed sequence, with clearances cut into steel. That single difference explains why a prototype can hold a tolerance on a bend that a die cannot, and why a die can hold a hole position that a brake cannot.

The second change is the hole strategy. A prototype can carry a 6.3 mm hole because the drawing said 6.3 mm. A die wants a standard pierce punch, so the hole becomes 6 mm or 6.5 mm with a matching punch that is already on the shelf, or a new punch is ordered. Every non-standard hole in a prototype becomes a tooling line item.

Prototype versus production design: the values that move

The table sets the two routes side by side. The prototype column is what a laser and a 200 T brake deliver; the production column is what a progressive die on our press line delivers. The right-hand column is the decision each row forces.

The tolerance row is the one that surprises designers. A die is more accurate on pierced holes and less accurate on formed heights than a brake. If the drawing puts ±0.15 mm on a bend height because that is what the prototype achieved, the die cannot hold it and the toolmaker will ask for a drawing change. If the drawing puts ±0.15 mm on a hole pattern, the die will hold it easily.

Which prototype features do not survive the die?

Four, and each has a replacement.

Tight bend radii on thick material. A 1t radius on 3 mm CRCA is at the edge of what a brake can do and beyond what a die should attempt without a coining station. Production moves to 1.5t, which changes the flat pattern and the bend deduction.

Non-standard hole and slot sizes. A 6.3 mm hole, a 4.2 mm slot and a 12.7 mm cutout become 6, 4 and 12 mm. Fastener clearance is unaffected at these sizes; the drawing note "unless otherwise specified" is not.

Edge distance tuned to the prototype. A hole 7 mm from the edge passes on a laser blank and tears on a die that strips the part. Keep the hole at least 1.5t from the edge, and 2t where the strip has to carry the part through the next station.

Bend relief added by hand. A laser-cut prototype often gets a relief notch added on the bench where a bend crack appears. The die needs that notch designed in, with a radius of 0.5 mm minimum and a width of at least the material thickness plus the bend radius.

How does the flat pattern change?

The flat pattern is the same idea on both routes and a different number on each. A brake uses a K-factor derived from the tooling and the material, typically 0.42–0.48 for CRCA. A die uses the same physics with a different effective K because the material is coined or bottomed at the bend, which pushes K towards 0.5 and reduces the bend allowance slightly.

Take a 90° bend in 2 mm CRCA at R2. With K = 0.44, bend allowance is π(2 + 0.88) × 0.5 = 4.52 mm. With K = 0.50, it is π(2 + 1.0) × 0.5 = 4.71 mm. The difference is 0.19 mm per bend. On a part with four bends, using the prototype flat pattern in the die makes the part 0.76 mm long across the developed length, which is enough to move a hole out of tolerance at the far end.

The practical rule: never issue the prototype flat pattern as the production blank. Issue the finished part drawing with bend radii, and let the toolmaker develop the blank from the die's own K. The bend allowance guide and the K-factor guide carry the arithmetic.

What decides die clearance and springback?

Die clearance is set per side at 5–8% of thickness. For 2 mm CRCA that is 0.10–0.16 mm. Too little clearance and the punch shears the sheet with a secondary crack and a taller burr; too much and the cut edge rolls over and the hole is tapered. The clearance is not on the drawing, and it does not need to be, but it explains why a die supplier may ask for the material grade and the thickness tolerance before quoting.

Springback is the other half. A 90° bend does not come out at 90° because the material unloads elastically. For CRCA at 1–3 mm, the recovered angle is typically 1–3° for a free bend and under 1° for a bottomed or coined bend. A die handles it in three ways: it overbends the punch, it bottoms the material against the die, or it adds a cam to restrike the corner.

The design consequence is a limit on what the drawing should ask for. A ±0.5° angle on a 400 mm flange is achievable on a brake with a programme that corrects per part. On a die, the same tolerance needs a restrike station and a die that is ground in after trial. If the part does not need ±0.5°, do not ask for it.

What volume makes the die the right route?

The decision is not "stamping is for high volume". It is a comparison between a fixed tool cost and a variable piece time, and the crossing point moves with part size and feature count.

A small bracket with four bends and six holes can run on a progressive die at a few seconds per stroke. The same bracket on laser and brake takes a nest on the 12 kW machine and four brake setups, which is minutes per part. At 5,000 parts a year, the die sits idle for most of it and the tool is a liability. At 50,000 a year, the die pays for itself and the brake route becomes the constraint.

Size changes the answer. A 1,500 × 800 mm panel needs a die and press that can carry the tonnage and the bed, and the tool cost rises faster than the cycle time falls. Panels in this size class often stay on laser and brake for the whole programme, and the large-format laser work is how that route stays competitive.

The tooling cost versus piece price guide sets out the amortisation properly. The rule to carry into a design review is simpler: agree the annual volume and the expected programme life before the design is frozen, because a part designed for a die and ordered at 8,000 a year is overbuilt.

What should not change between the two routes?

The interfaces. Datums, mounting hole patterns, mating faces, cable entry positions, hinge centres and the finish should be identical on the prototype and the production part. If they are, the assembly proved on the prototype still works when the die parts arrive.

The tolerance scheme can change around them. A prototype might hold ±0.2 mm everywhere because the brake can. Production moves the tight tolerance to the pierced hole pattern and relaxes the formed features to ±0.4 mm. The assembly still fits because the locating feature is the hole pattern, and the hole pattern got better.

Material is the exception that has to be agreed. A prototype cut from CR3 because it was in the rack may be quoted in CR1 for production, and CR1 will crack at a 1t bend that CR3 survived. Either keep the grade or move the radius. The mill certificate should travel with the first production lot, and the material traceability requirements apply to stamped parts as much as welded ones.

How we move a part from prototype to production

The prototype is cut on the 12 kW fibre laser on the 40 ft × 16 ft bed and formed on the 200 T, 5-axis brake with the 4,450 mm bed. Both are programmed from the customer's DXF or STEP, so a prototype carries no tooling and no tooling cost. The same file can be run again next month if the design changes.

When the volume justifies a tool, the part moves to the 20–300 T press line, with a 250 T punching station for the heavier pierce work. The tool is designed and built in our own tool room, which is also where it is maintained and where a worn pierce insert is replaced. That matters at the transition: the person who built the die is the person who runs the first article, and the strip layout is developed against the press it will run on.

The transfer is not automatic. The tool room reviews the prototype drawing for pierce sizes, radii, edge distances, bend sequence and strip layout before the die is designed. What comes back is a marked-up drawing with the changes in the table above. On a typical bracket that review takes a few days and saves a die change later.

For programmes that need both, the two routes run side by side. Prototype and low-volume service parts stay on laser and brake while the production volume runs on the die. The part number is the same; the route differs by quantity. That arrangement is covered in prototype to serial production and in the single-stage versus progressive die comparison.

What to put on the production drawing that the prototype did not need

1. Pierce sizes — standard diameters and slot widths, or a note allowing the toolmaker to standardise within 0.2 mm.
2. Burr side — which face the burr is allowed on, and the maximum burr height.
3. Form height tolerance separate from hole tolerance — they are not the same on a die.
4. Bend sequence note — where the die can and cannot form, especially on a return flange.
5. Die clearance basis — material grade and thickness tolerance, so the tool is cut for the sheet that will actually arrive.
6. Strip direction — bend lines relative to the coil direction, or the grain requirement.
7. Scrap allowance — features that force a wider strip, agreed before the tool is cut.
8. First article requirements — which dimensions are on the FAI report, and the sample size.

The first article inspection guide sets out how those dimensions are checked once the die is running, including the capability study that tells you whether the die holds the tolerance across a shift. The DXF and drawing checklist carries the file-level items that go with them.

When the prototype design should stay as it is

Not every part should be tooled. A part that will run 3,000 a year for five years is a laser and brake part, and tooling it adds a fixed cost with no payback. A part with a feature that may change next season should stay on the flexible route, because a die locks the geometry.

Parts that need a finish on every edge, or that are welded into an assembly with a fixture, are also poor candidates for a first tool. Prove the assembly first, then tool the part that is stable. Tooling a part before the weld sequence is settled is the most common way to cut a die twice.

We build both routes in the same plants, so the conversation is not about which process we prefer. Send the prototype revision and the annual volume through request a quote, and the reply will say which route the volume supports and which drawing changes each route needs.