Design review checklist for sheet metal: what to check

A drawing that reaches the shop floor without a design review is a set of promises nobody has checked. Most of them are kept. One or two are not, and those are the ones that turn into a rework note, a tooling amendment or a concession at the customer's incoming inspection.

The arithmetic that justifies the hour is well known in manufacturing: a change made in CAD costs one unit of effort, the same change after tooling costs about ten, and after the part is in service about a hundred. On sheet metal the jump from one to ten is not gradual. It is a step, because a press tool is cut once and a bend programme is proved once.

This design review checklist for sheet metal is the sequence we run when a drawing arrives, in the order that finds the expensive problems first. It covers the eight checks that decide whether the part can be made, the limits we hold on each, and what to write on the drawing so that the next person does not have to guess. The wider set of design rules sits in the Design and CAD hub.

What does a design review decide before a drawing is released?

It decides three things: whether the part can be formed at the thickness drawn, whether the tolerance on each feature can be held by the process chosen, and whether the finish and assembly steps have somewhere to work. Everything else is detail.

Take the first. A 90° bend in 2 mm CRCA with a 1 mm inside radius is a 0.5t radius. The outer fibre strain at that radius is roughly t/(2R + t), so 2/(2 + 2) = 0.5, or 50%. CR1 commercial-quality sheet cracks well before that; CR3 deep-drawing grade tolerates more but still shows orange peel on the outside of the bend. The usual rule for CRCA is an inside radius of at least 1t, with 1.5t where the part will be coated and the bend is visible.

Take the second. A drawing that says ISO 2768-1 class m on every dimension has said, in effect, that nothing matters more than anything else. Class m gives ±0.2 mm between 6 and 30 mm and ±0.3 mm between 30 and 120 mm. Those are general-tolerance defaults for a machined or formed part; they are not a statement about what a press brake or a laser can hold on a particular feature. The features that carry the assembly — hole patterns, mating faces, datum edges — need their own callouts.

Take the third. A canopy panel that is drawn without a drain path, a masking note on the earth stud, or a lifting point will be built without them. A manufacturing engineer can drill a drain hole, but only against a revision, and a revision before the first article costs a week.

The design review checklist for sheet metal, with numbers behind it

The table is the review sheet we use. The middle column is what to look at on the drawing; the right-hand column is the limit we work to and where the constraint comes from. The values are for CRCA and mild steel unless stated.

Two rows of that table account for most of the rework we see. The first is thickness tolerance. A designer specifies 2 mm, the mill supplies 1.8 mm at the low end of the normal tolerance, and the bend deduction in the flat pattern is now 0.3 mm out. On a part with four bends the error accumulates to more than a millimetre, and the hole pattern no longer lines up with the mating part.

The second is the hole-to-bend distance. A hole punched or cut too close to the bend line is pulled into an oval by the material flowing into the bend. The hole still measures correctly on the flat; it is only after forming that the inspector finds it 0.6 mm out of round and the fastener will not sit.

Which checks change the price, and by how much?

Four checks move the piece price more than the rest, and each one is a number the designer controls.

Bend count and bend radius. Each bend is a stroke, and each stroke has a setup share on a short run. On the 200 T, 5-axis brake with the 4,450 mm bed, a programme stores the angle and the backgauge position, so a repeat order pays almost no setup. The first order pays for the programme and the test bend. Reducing a part from six bends to four is worth more than reducing the blank by 10%.

Bend allowance and the flat pattern. Bend allowance for a 90° bend is BA = π(R + Kt)θ/180. With R = 2 mm, t = 2 mm, K = 0.44 and θ = 90°, BA = π × (2 + 0.88) × 0.5 = 4.52 mm. The bend deduction is 2(R + t)tan(θ/2) − BA = 2 × 4 × 1 − 4.52 = 3.48 mm. A part with two 50 mm legs therefore needs a flat length of 50 + 50 − 3.48 = 96.52 mm, not 100 mm.

If the CAD flat pattern uses a different K, the blank is wrong before the first cut, and the error repeats on every part in the nest. The bend allowance calculation and the K-factor guide carry the full derivation.

Hole and slot count. Laser cutting is priced largely on cut length and pierces. A 10 mm hole has a 31 mm circumference; forty of them add 1.26 m of cut to a part that may only carry 2 m of outline. Replacing forty small holes with a perforated pattern that is bought as sheet, or with a single louvred vent, changes the cut length and therefore the price.

Tolerance class. A ±0.2 mm callout on a hole pattern that sits in a formed panel forces either a post-form machining step or a fixture that holds the part during drilling. Most sheet metal parts do not need it. A ±0.5 mm pattern, checked with a go/no-go gauge, does the same job for a fraction of the effort.

How much tolerance can a formed part actually carry?

A single formed feature holds ±0.5 mm comfortably. A chain of five formed features does not hold ±0.5 mm at the end of the chain, and this is where most released drawings are optimistic.

Consider a bracket with five dimensions in sequence, each at ±0.5 mm, ending at a mounting hole. Worst-case arithmetic adds every tolerance: ±2.5 mm at the hole. Root-sum-square arithmetic adds them in quadrature: √(5 × 0.5²) = ±1.12 mm. Reality sits between the two. If the five features are formed in one press tool from one blank, most of the error is common — the same material thickness and the same tool wear shift all five in the same direction — and the result behaves closer to the RSS figure. If the five features are formed on five separate brake setups, each setup contributes an independent error and the result drifts towards the worst case.

The consequence is a decision, not a calculation. If the assembly needs ±1 mm at the hole, five chained ±0.5 mm features are marginal on a brake and should be reduced to three, or the hole should be slotted, or the mating part should carry the adjustment. Putting ±1 mm on the drawing without changing the design transfers the problem to the supplier, and the supplier will meet it by adding an operation.

The worst-case versus RSS tolerance stack guide works through the same bracket with a datum scheme, which is the other half of the problem. A stack is only meaningful if every dimension starts from the same datum. Drawings that dimension from five different edges force the inspector to reconstruct the datum before measuring anything.

What the review has to catch that CAD cannot show

A model shows geometry. It does not show the order of operations, and several decisions only make sense in that order.

Bend sequence and collision. A box with four walls and a top flange cannot always be bent in the order the model suggests. The punch and the part collide on the third bend unless one flange is shortened or the bend is moved. This is a two-minute check on a brake simulation and a two-week problem if it is found after the tool is cut.

Weld access. A fillet weld specified on the inside of a 60 mm deep channel cannot be reached by a MIG torch with a 15 mm nozzle. The weld symbol is valid; the joint is not. Either the channel gets a wider opening, or the joint becomes a plug weld, or the part is redesigned as a folded section.

Coating drainage and throw. Powder and pretreatment chemicals have to reach every surface and drain from every pocket. A closed box with no drain hole traps pretreatment liquid, which bleeds out during cure and leaves a stain or a blister. Two 8 mm drain holes at the lowest point of each closed section solve it, and they need to be on the drawing.

Grain direction. A part bent along the rolling direction of the coil cracks at a larger radius than the same part bent across it. If the blank nests with the bend line parallel to the coil edge, the part may need a larger radius or a different grade. The nesting decision belongs to the supplier, but the bend direction on the part is the designer's.

Lifting and handling. A 1,800 × 900 mm canopy panel in 1.5 mm steel weighs about 19 kg. Two people can lift it; one cannot safely. A lifting point or a handling note changes the packing and the freight, and it is cheap to add at release.

What Ganesh checks when the drawing arrives

Every enquiry gets a manufacturability review before it gets a price. The review is not a courtesy; it is where we decide which machine the part runs on and whether the tolerance on the drawing matches that machine.

Blanks and outlines go to the 12 kW fibre laser with its 40 ft × 16 ft bed, which takes a full canopy side or a long rail section in one piece. Formed features go to the 200 T, 5-axis CNC press brake with a 4,450 mm bed and Delem control, which holds 10 mm thickness and stores the programme for repeat orders.

Small pressed parts move to the 20–300 T press line where the volume justifies a tool, and the tool is designed in our own tool room. Welded assemblies run on three CLOOS robotic MIG cells or one of more than 30 manual stations, with fixtures built in-house. Coated parts go through seven-tank pretreatment, a 16 ft × 16 ft shot blast chamber where the specification calls for a profile, an 18 ft × 14 ft electrostatic powder booth and a curing oven, with DFT and cross-hatch adhesion checks.

The review returns three things: a list of features we cannot hold at the drawn tolerance, a list of features that will add cost without adding function, and a proposed drawing change for each. On a repeat part the review is shorter because the process is already fixed. On a new part it is the most useful hour in the programme.

Our sheet metal bending capability page carries the brake envelope and the thickness range, and the drawing notes guide covers the note wording that survives a revision. Both are worth reading before the review, not after.

What to put on the drawing before release

1. Material grade and standard — IS 513 CR3, 2.0 mm, half-tolerance if the bend deduction depends on it.
2. Bend radius at each bend — inside radius, not "sharp".
3. Bend direction — up or down, with a note if the bend must run across the coil grain.
4. Datum scheme — three datums, with the critical hole pattern dimensioned from them.
5. Tolerance per feature — general tolerance class plus individual callouts on mating features.
6. Hole-to-bend and flange minimums — or a note that the supplier may adjust within the stated limits.
7. Weld symbols and sequence — including which face is cosmetic and must not be welded.
8. Finish schedule — pretreatment, powder type, colour, DFT in µm, masking points, earth stud treatment.
9. Drain and vent holes — position and diameter for every closed section.
10. Handling and packing — lifting points, stack limit, interleave requirement.

The DXF and drawing hand-off checklist carries these fields in the order a nesting engineer needs them, which shortens the gap between a released drawing and a first article.

When a design review is the wrong tool

A review cannot rescue a part that should not be sheet metal. If the geometry needs a wall thickness above 6 mm, a machined or cast part is usually cheaper and stiffer. If the part needs a seal face flat to 0.05 mm, a formed panel will not hold it without machining after forming. If the annual quantity is under about 200 and the part has eight bends, the setup cost per part dominates and a welded fabrication from standard sections may be the better route.

A review also cannot substitute for a prototype. It can tell you that a bend is tight or a flange is short. It cannot tell you whether the assembly sounds right, whether the door closes with the gasket fitted, or whether the coating survives the first monsoon. Those need a first article and a field trial.

What the review does is stop the drawing from carrying problems that nobody intended. Send the current revision through request a quote and the review comes back with the price, rather than a fortnight later as a clarification.