Key takeaways
- A tolerance that is wider than plus or minus four standard deviations supports a Cpk of 1.33 and about 63 defects per million; narrower than that, the defect rate is written into the drawing.
- On a 300 mm bracket with two bends, the combined sigma is 0.103 mm, so a ±0.15 mm callout gives Cp 0.49 and about 15% of parts outside the band.
- Laser hole position varies with sigma near 0.03 mm and formed dimensions near 0.07 mm, so a formed tolerance below ±0.3 mm needs a different route, not a harder inspection.
- A gauge should resolve one tenth of the tolerance; a ±0.15 mm callout needs 0.015 mm resolution, which a standard caliper cannot provide.
- Set the tolerance from the assembly limit and the measured spread, not by dividing the assembly allowance by the number of parts.
A drawing calls ±0.15 mm across two bends on a 300 mm bracket. The shop's combined standard deviation on that dimension is 0.10 mm, so the tolerance band is 1.5 standard deviations per side and about 13% of parts fall outside it. Nobody has done anything wrong: the tolerance was written to an assembly need that was probably real, and the process is running normally. The number on the drawing and the number the process produces were never compared.
Tolerance versus capability is that comparison. Tolerance is the band the drawing allows. Capability is the spread the process produces when it is running normally, expressed as a standard deviation. A tolerance wider than the process spread is an instruction the shop can meet. A tolerance narrower than the spread is a defect rate written into the drawing, and it will be paid for in inspection, sorting and scrap rather than in the piece price.
The sections below give the arithmetic for setting a tolerance from a process, the spread each sheet metal feature actually produces, and the point at which the honest answer is to change the design rather than to demand a tighter number.
What do Cp and Cpk measure?
Cp is the tolerance width divided by six standard deviations. It answers how much room the band has compared with the process spread, assuming the process is centred. Cpk is the same ratio measured to the nearer limit, so it also penalises a process that runs off-centre.
The index converts to a defect rate with a normal distribution assumption. At Cp 1.0 the band is ±3σ and about 2,700 parts per million fall outside. At 1.33 it is ±4σ and about 63 parts per million. At 1.67 it is ±5σ and about 0.6 parts per million. At 0.67 it is ±2σ and roughly 45,000 parts per million, which is a part in twenty-two.
For sheet metal the useful thresholds are 1.33 on anything that controls assembly or carries a load, 1.0 on cosmetic and non-functional dimensions, and no index at all on dimensions that do not matter, because the cheapest tolerance is the one you did not specify.
The first question is never "what is the Cpk" but "what is σ". A process that has never been measured has no capability, and a supplier who quotes a number without a study is quoting an opinion.
What spread does each sheet metal feature produce?
The table gives the standard deviation that a stable process produces on common features, the resulting 6σ spread, and the tolerance that a Cpk of 1.33 supports, which is ±4σ. The figures are for steel from 1.0 to 3.0 mm on production equipment, and they widen on thicker or harder stock.
| Feature | Typical σ | 6σ spread | Tolerance for Cpk 1.33 (±) | What moves the figure | Ganesh limit or note |
|---|---|---|---|---|---|
| Laser-cut hole position | 0.02-0.03 mm | 0.12-0.18 mm | 0.08-0.12 mm | Sheet thickness, nozzle condition, nesting | ±0.10 mm typical up to 3 mm |
| Laser-cut profile length | 0.03 mm | 0.18 mm | 0.12 mm | Lead-in, kerf compensation, material stress | Tighter callouts agreed per feature |
| Bend line position | 0.05-0.08 mm | 0.30-0.48 mm | 0.20-0.32 mm | Backgauge, blank straightness, springback | ±0.5 mm typical on formed parts |
| Bend angle | 0.3-0.5° | 1.8-3.0° | 1.2-2.0° | Material yield, tooling, ram repeatability | 200 T brake, 4,450 mm bed to 10 mm |
| Hole to hole across a bend | 0.08-0.12 mm | 0.48-0.72 mm | 0.32-0.48 mm | Two bend positions plus cut error | The stack that catches most drawings |
| Stamped feature to datum | 0.03-0.05 mm | 0.18-0.30 mm | 0.12-0.20 mm | Die clearance, strip feed, press repeatability | Progressive tools held in-house |
| Welded frame datum to datum | 0.5-0.8 mm | 3.0-4.8 mm | 2.0-3.2 mm | Fixture, weld sequence, heat input | Fixtures built in-house |
| Panel flatness over 1,000 mm | 1.0 mm/m | 6.0 mm/m | 4.0 mm/m | Residual stress, bend sequence, gauge | Straightening is a separate operation |
Read the bend row against the opening example. A tolerance of ±0.15 mm across two bends sits below the 0.32-0.48 mm that Cpk 1.33 supports, and below the 0.20 mm that even a single bend position supports at its best. It is not a difficult tolerance. It is a tolerance outside the process by a factor of two.
Worked example: the 300 mm bracket
The bracket has two 90° bends and a 250 mm hole-to-hole dimension across both. The error sources are independent, so they add in root-sum-square rather than in a straight line.
- Hole position from the laser: σ = 0.03 mm per hole end.
- Bend line position, two bends: σ = 0.07 mm each.
- Combined: the square root of (0.03² + 0.07² + 0.07²), which is 0.103 mm.
The drawing's ±0.15 mm gives Cp = 0.30 / (6 × 0.103) = 0.49. A centred process at that index produces roughly 15% out of tolerance, and a process running 0.05 mm off centre produces more on one side.
To reach Cpk 1.33 the tolerance has to be ±4σ, which is ±0.41 mm. That is inside the ±0.5 mm typical band for formed parts, and it is the number to take to the assembly stack. If the joint cannot accept 0.41 mm, the answer is to change the joint or to add an adjustment, not to write 0.15 mm and hope.
The second arithmetic is what the tight tolerance does to inspection. A gauge should resolve at least one tenth of the tolerance, so ±0.15 mm needs a resolution of 0.015 mm and a gauge repeatability well inside that. A vernier at 0.02 mm resolution cannot make the call, which means 100% inspection on a CMM or an air gauge, which means the inspection cost is now part of the piece price.
Where the tolerance budget actually goes
A tolerance on a drawing is a share of an assembly budget. The assembly has a clearance, a gasket compression range or a bolt hole float, and every part in the stack takes a slice. Two allocation methods are used, and they give very different answers.
Worst-case allocation adds every contributor at its limit. If three parts each carry ±0.2 mm, the assembly varies by ±0.6 mm before any weld or coating. Root-sum-square allocation treats the contributors as independent and gives the square root of the sum of squares, which for the same three parts is ±0.35 mm. RSS is statistically defensible when the processes are independent and centred; worst case is the right method when a single part can be at its limit in the direction that matters, such as a sealing face.
The mistake is to allocate by dividing the assembly tolerance by the number of parts. That assumes every part will sit at its limit simultaneously, which is why drawings inherit tolerances no process can hold. Start from the assembly limit, allocate by the method that matches the failure consequence, then check the result against the table above. Tolerance stack-up: worst case versus RSS works the arithmetic in full.
There is a third contributor that is usually left out: coating. Powder at 60-80 µm adds 0.06-0.08 mm per coated face, so a 10 mm hole closes to about 9.86 mm and a 100 mm outside dimension grows to 100.14 mm. On a tolerance of ±0.15 mm, the coating alone consumes half the band. Either mask the feature, specify it before coating and accept the shift, or open the tolerance.
The measurement has to be capable too
A process is only as capable as the gauge that judges it. Gauge repeatability and reproducibility, the R&R study, compares measurement variation with the tolerance. The common acceptance is 10% of tolerance for a capable gauge, up to 30% for a marginal one, and above 30% the gauge is not suitable for that feature.
Take a ±0.10 mm bore position checked with a gauge whose R&R is 0.04 mm. The measurement consumes 20% of the tolerance, so a part at the limit can be accepted or rejected depending on the day. The shop reacts by tightening the process to protect against the gauge, which costs money for no gain in the part. A better gauge is usually cheaper than a tighter process.
The rule of ten follows from the same logic: the gauge should resolve one tenth of the tolerance. A ±0.5 mm formed dimension needs 0.05 mm resolution, which a caliper provides. A ±0.1 mm laser feature needs 0.01 mm, which a caliper does not. Writing the inspection method on the drawing prevents the argument at first article, and it also tells the supplier which gauge to budget for.
Why a capable process drifts out of capability
A capability study describes a window, not a guarantee. Three things move the window during a programme, and each one has a different response.
Tool wear moves the mean. A piercing punch that has worn 0.05 mm produces a hole 0.05 mm larger, so a dimension that started at the centre of its band walks toward one limit. The regrind interval is the control: the process is re-centred when the punch is sharpened, and the study is repeated after the regrind, not before.
Coil change moves the spread. A new heat with a yield 30 MPa higher bends to a different angle at the same ram depth, which shows up as a shift in the formed dimension. The first-off check after a coil change is what catches it, and it is why a lot that passed last month can fail this month without anything in the shop changing.
Fixture wear moves both. A locating pin that has worn 0.1 mm adds 0.1 mm to every part made on that fixture, and the effect is invisible until the assembly stops fitting. The check is a fixture verification at a defined interval, not a visual inspection.
A capability figure quoted at quotation is therefore a statement about the process as it will be run, with the maintenance intervals and the first-off checks included. A figure quoted without those is a figure for the first hundred parts only.
How to set a tolerance the process can hold
The sequence is short and it is the same for a new part and a complaint.
- Name the interface. What does this dimension touch, and what is the clearance or interference at that joint?
- Set the assembly limit. The total movement the joint can absorb, including coating and weld distortion.
- Allocate by consequence. Worst case for sealing and safety, RSS for independent cosmetic stacks.
- Check against capability. Use the table, or the supplier's study if one exists. If the allocation is below 4σ, the design or the process has to change.
- Write the datum and the method. A tolerance without a datum is not measurable, and a tolerance without a method is argued at inspection.
Step four is where most drawings fail. A designer who has not seen a capability study will set the tolerance from a CAD model, and the model has no spread. The supplier then either quotes a high price to cover the inspection or accepts the order and delivers a proportion outside the band, and both outcomes are worse than a five-minute conversation about σ.
What Ganesh runs, and where the limits sit
The forming route determines the spread. Laser cutting on the 12 kW fibre machine with a 40 ft × 16 ft bed holds hole position to about ±0.10 mm at thicknesses up to 3 mm, and the 200 T, 5-axis brake with a 4,450 mm bed holds formed dimensions to ±0.5 mm typical, with tighter callouts agreed per feature. Custom parts run from 0.8 mm to 40 mm.
The agreement matters more than the headline. When a drawing needs ±0.2 mm on a formed feature, the route changes: a fixture-built subassembly, a post-form adjustment, or a first article with a capability study on the critical dimension. Those are quoted as a different route rather than absorbed into the standard tolerance. PPAP and first article inspection are available where the programme requires them, and the dimensional report measures the dimensions the drawing controls.
Where the feature needs better than the process can hold, we say so at quotation. A bearing seat, a mating connector footprint or a sealing face is usually a machined or a purchased component, and forcing it into a sheet metal tolerance is how a drawing acquires a permanent deviation.
When a tight tolerance is the right call
A tight tolerance is correct when the function demands it and the process can be made to deliver it: a hole pattern that locates a motor, a bend that sets a door gap, a flatness that lets a gasket seal. In those cases the tolerance should be tight, the datum explicit, the gauge named and the capability proven, and the cost is justified by the function.
It is wrong when the tolerance is inherited from a template, when it is tighter than the assembly needs, or when it compensates for a stack that was never calculated. The test is simple: if the dimension went out by the full tolerance, what would fail? If the answer is nothing, the tolerance is decoration.
For the inspection side, bending tolerances and inspection covers how a formed dimension is measured, and laser cutting tolerances for OEM parts covers the cut figures that feed the stack. The design and CAD hub collects the rest of the drawing decisions. Send the drawing with the critical dimensions marked to our engineering team and we will return the achievable figure and the inspection method for each one.
Frequently asked questions
What Cpk should a sheet metal part have?
Use 1.33 on dimensions that control assembly or carry a load, which is a tolerance of plus or minus four sigma. Use 1.0 on cosmetic dimensions, and do not specify an index on features that do not affect fit or function. A supplier who quotes a Cpk without a study is quoting an opinion.
Why is ±0.5 mm typical on formed parts?
Because the formed dimension carries cut error, bend deduction, thickness variation and springback. On 1.5-2 mm CRCA those combine to a sigma near 0.07 mm per bend, so a ±0.5 mm band is roughly ±7σ on a single bend and holds a two-bend stack at about Cpk 1.6 when centred.
Can a press brake hold ±0.1 mm?
Not on a formed dimension of any length. The backgauge can position to 0.01 mm, but the bend deduction varies with thickness and yield, and springback varies with the coil. A ±0.1 mm requirement on a formed feature is a request for a fixture-built assembly or a post-form operation.
How does coating affect the tolerance?
Powder at 60-80 µm adds 0.06-0.08 mm per coated face. A 10 mm hole closes to about 9.86 mm and a 100 mm outside dimension grows to 100.14 mm, which consumes a large share of a ±0.15 mm band. Mask the feature or account for the film in the stack.
What is the difference between Cp and Cpk?
Cp compares the tolerance width with six sigma and assumes the process is centred. Cpk measures to the nearer limit, so it falls when the process runs off centre. A process can have a healthy Cp and a poor Cpk, which is what happens after a tool wears or a backgauge drifts.
Sources and further reading
- ISO 2768-1:1989 - General tolerances, linear and angular dimensions without individual tolerance indications · reviewed 3 Nov 2026
- ISO 22514-1:2014 - Statistical methods in process management: capability and performance · reviewed 3 Nov 2026
- ISO 9013:2017 - Thermal cutting, classification of thermal cuts, geometrical product specification and quality tolerances · reviewed 3 Nov 2026
Have a tolerance that keeps failing first article?
Send the drawing and mark the dimensions that control assembly. We will return the measured spread, the achievable tolerance and the inspection method for each one.
Request a quote