Key takeaways
- A progressive die holds a tight band on a stable feature and a much wider band across a bend or between stations.
- Thickness tolerance and material grade move the achievable band as much as the tool does.
- Position tolerances should be referenced to the die datum, not to a random edge or a feature made at another station.
- An inspection method that cannot reach the feature turns a tolerance into a recurring cost.
A tolerance is a statement about the process
A tolerance does not describe how good a supplier is. It describes what the process can repeat. A progressive die cuts and forms in a sequence, and the strip moves one pitch per stroke. Features made at the same station, in the same stroke, have a tight relationship. Features made at different stations inherit the pitch error, the pilot clearance and the strip stretch between them.
That is why two dimensions on the same drawing can need very different bands. A hole pattern pierced at one station can hold a close position tolerance. A bend formed four stations later, after the strip has been notched and lanced, is working against a moving reference. The tool can still hold it, but the band is wider and the inspection has to match.
The practical approach is to decide which features locate the part, which carry current or force, and which are cosmetic or clearance. Put the tight bands on the first two groups and let the general tolerance cover the rest. A drawing that applies a close band everywhere tells the supplier nothing about where to spend the tool budget.
Realistic bands by feature
The values below are illustrative starting points for a progressive die in 1.0 mm mild steel. They are not a standard and they are not a promise. They are a way to sanity check a drawing before the quote, and they should be confirmed with the toolmaker for the actual part, thickness and strip layout.
Hole diameter is one of the most stable calls because the punch size sets it directly. Wear moves it over the tool life, so the band has to include the wear allowance. Hole position is stable when the hole is pierced at the same station as the datum, and less stable when it is measured from a feature made elsewhere.
Bend angle is the call that causes the most discussion. A progressive die can hold a bend angle, but the material lot, the springback and the tool wear all move it. A band of plus or minus one degree is a practical starting point for a mild steel form at a moderate radius. Stainless or high-strength steel needs a wider band or a re-strike station.
| Feature | Starting band | What moves it | How to check |
|---|---|---|---|
| Hole diameter | ±0.05 mm | Punch wear, slug clearance, material | Plug gauge or calliper |
| Hole position | ±0.10 mm | Pilot clearance, station sequence | CMM or pin gauge in a fixture |
| Bend location | ±0.15 mm | Strip stretch, bend allowance, tool wear | Height gauge from the datum |
| Bend angle | ±1.0 degree | Springback, material lot, die gap | Angle gauge or profile projector |
| Overall length | ±0.20 mm | Pitch error, trim station, burr | Calliper or vision system |
| Flatness | 0.10 mm total | Residual stress, handling, stacking | Surface plate and indicator |
| Burr height | 0.05 mm maximum | Die clearance, punch wear, material | Profile projector or micrometer |
Illustrative only, for a conventional progressive die. Confirm the band with the toolmaker and the inspection plan for the actual part.
Thickness and material move the band
The nominal gauge is not the thickness the die sees. A coil supplied at the top of the mill tolerance forms a different bend allowance and a different springback from one at the bottom. If the drawing gives a close band on a bend location without a thickness tolerance, the two calls can contradict each other. Ask for the mill tolerance and check the stack.
Material grade changes the shear behaviour as well. Mild steel cuts cleanly and wears the tool slowly. Stainless work-hardens at the edge, raises the punch load and wears the tool faster, so the band widens over the tool life. High-strength steel does both and may need a premium punch material. Copper and brass cut easily but can smear, which affects the hole size and the burr.
The die clearance is set for a material and a thickness. Running a different gauge through the same tool changes the clearance ratio, the burr and the fracture zone.
Position, datums and stack-up
A position tolerance is only meaningful with a datum. The die has a datum: the pilot holes and the strip edge that locate every station. The drawing should use the same idea, so the inspection fixture and the tool agree on what is fixed. When the drawing dimensions a hole from a cosmetic edge, the supplier has to translate, and the translation adds uncertainty.
Stack-up matters when several features sit in a chain. A hole position measured from another hole accumulates the error of both, plus the error between their stations. A hole position measured from a common datum accumulates only its own, which is easier to hold and easier to inspect.
A tight tolerance across a bend is two problems
The bend moves the material and the tolerance spans two stations. If the feature must be tight, move it out of the bend zone or add a re-strike, rather than tightening the number on the drawing.
Flatness, twist and burr
Flatness is a residual stress call. A part that is flat coming out of the die can bow after plating, after handling or after a day in a stack. The die can improve flatness with a restrike or a straightening station, but the material and the strip carrier also contribute. If flatness matters for assembly, state the measurement condition: free state, clamped, or on a surface plate.
Twist is a different defect from bow. It happens when one side of the part is formed more than the other, or when the carrier releases unevenly. A twist tolerance is usually expressed as an angle over a length, and it needs a fixture to measure. Without a fixture, two inspectors will get two answers.
Burr height is set by the die clearance and the punch wear. A sheared edge always has some burr, so the call should be a maximum and a direction. If the burr sits against a seal or a sliding surface, say so. If the part is deburred, the process adds handling and can change the edge dimension, so the deburr route belongs in the quote.
Capability, inspection and sample size
A tolerance band is not the same as a capable process. A die that holds plus or minus 0.05 mm on the first article may drift over a hundred thousand strokes as the punch wears. The supplier should know the wear allowance and the punch replacement interval, and the inspection plan should catch the drift before the band is exceeded.
Ask for the first article to cover every dimension on the drawing, then agree a shorter in-process check for the critical features. For a progressive die, the check should include at least one feature from each station that can move: a pierced hole, a formed angle and the overall trim length. That gives an early warning without turning every stroke into an inspection.
If the part is supplied with a PPAP pack, the process capability study should use the same datum and the same measurement method as the drawing.
How to write the drawing
Put a general tolerance in the title block, then add tighter bands only where the function needs them. Mark the critical-to-quality features and say how they will be measured. If a feature sits at the process limit, ask for a DFM note rather than assuming the die can hold it.
Give the material grade, the thickness and the thickness tolerance. State the finish and whether it can change the dimension, because plating adds thickness on every surface. State the burr direction and the flatness condition. Those four items remove most of the ambiguity that turns a tolerance review into a negotiation.
- General tolerance and the standard it references
- Critical features with a position or profile call
- Datum scheme that matches the die and the fixture
- Material grade, thickness and thickness tolerance
- Finish and any dimension change from plating
- Burr direction and flatness measurement condition
Frequently asked questions
What tolerance can a progressive die hold?
It depends on the feature. A pierced hole can hold a band in the region of plus or minus 0.05 mm in 1.0 mm mild steel, while a bend location or an overall length is usually wider. Confirm the band with the toolmaker for the actual strip layout and material.
Why is a bend angle tolerance wider than a hole tolerance?
A hole is set by the punch size, while a bend is set by the tool plus the material recovery. Springback, thickness variation and tool wear all move the angle, so the achievable band is wider and the inspection method is different.
Should I tolerance a hole from the part edge or from a datum?
From a datum that matches the die and the inspection fixture. A dimension from a cosmetic edge forces the supplier to translate, and a chain of dimensions accumulates error. A common datum is easier to hold and easier to check.
Does plating change the stamped dimension?
Yes. Plating adds thickness to every surface, so a hole can close and an outside dimension can grow. If the finished dimension is critical, state whether the tolerance applies before or after plating, and give the plating thickness range.
Sources and further reading
- ISO 2768-1:1989, General tolerances, linear and angular dimensions
- ISO 2768-2:1989, General tolerances, geometrical tolerances
- Qumek first article and capability reviews for progressive-die stampings
Qumek Engineering Desk
Engineering team
The engineering team behind Qumek drawings, DFM notes, tolerances and inspection standards. Every guide is reviewed against the drawings and processes used on live programmes.
Check the tolerance before the die is designed
Send the drawing with the material and thickness. The engineering desk will mark the features that need a wider band or a different inspection method.
Send a drawing