Stamping tolerances: what a progressive die can hold

Progressive die tolerances are set by the strip, not by the toolmaker's skill. A die can be built to 0.005 mm and still produce a hole pattern that wanders ±0.12 mm, because the strip indexes between hits and the pilot pins only correct what the feeder left behind.

That is why a drawing calling ±0.05 mm across a six-station layout is not a tighter part. It is a request for a different process: fine blanking, a compound tool that cuts everything in one station, or laser cutting with a jig-bored fixture. Knowing which band belongs to which feature is the difference between a quote that holds and a launch that stalls at first article.

What progressive die tolerances can the tool hold by feature?

The band depends on whether the feature is cut in one station or carried across several. Anything cut inside a single station tracks the tool, which is ground to 0.01 mm. Anything that depends on the strip arriving in the right place tracks the feeder, which is an order of magnitude looser.

Use the table as a starting allocation, not as a promise. A part that stacks four of these bands into one assembly dimension is a tolerance stack problem, and the bracket tolerance guide works through that arithmetic with arithmetic and statistical sums.

Why does hole position move between stations?

Because the strip has to travel. A servo feeder positions 2 mm CRCA to about ±0.05 mm at a 300 mm pitch, and the pilot pins then pull the strip to the tool datum at ±0.02 mm. That correction is good, but it is applied at the pilot station, not at every station the part passes through afterwards. Between the pilot and the last station the strip stretches, twists and takes the camber of the coil with it.

Two consequences follow. First, the distance from a pilot hole to a feature cut two stations later is more reliable than the distance between two features cut at opposite ends of the tool. Second, a part that is checked on the die and then checked on a fixture can show different numbers, because the fixture holds it the way the customer will, and the die held it flat.

The practical rule for a drawing is to put the assembly datum on a feature cut in the first or second station and dimension everything else from it. A hole pattern that is toleranced from a hole cut in station seven inherits every station between the pilot and station seven.

How do die clearance and punch wear set hole size?

Clearance sits between 8% and 12% of thickness per side for CRCA, so a 2 mm sheet runs a 0.16–0.20 mm gap per side and a die opening 0.32–0.40 mm larger than the punch. Too little clearance doubles the burnish band and raises stripping force; too much produces a torn edge and a burr that grows through the run.

The hole follows the punch, and the punch wears. In 2 mm CRCA a punch loses 0.02–0.04 mm of diameter per 100,000 strokes, so an 8.00 mm punch is measuring 7.96 mm at the end of a long run and the hole follows it down. Sharpening restores the size and costs a setup, which is why a stroke counter on the press is a quality instrument and not a maintenance nicety.

The die wears the other way and opens up, which shows as burr rather than as size. A die that starts at 0.05 mm burr reaches 0.15 mm at about 300,000 strokes on 2 mm CRCA, and the part then fails the edge callout before it fails the dimensional one. The progressive die maintenance guide sets out the sharpening interval against stroke count rather than against calendar time.

Material changes the numbers in one direction. Stainless work-hardens at the shear edge, so 304 at 2 mm wants 12–15% clearance per side and a punch that is 0.02 mm oversize to allow for the springback of the slug. Aluminium at 2 mm runs 6–8% and galls unless the punch is polished and the strip is lubricated.

Which tolerances move with thickness and material?

Thickness moves the tonnage directly and the formed tolerances indirectly. Bend angle is the clearest case: at 90° in 2 mm CRCA with a 2 mm inside radius, springback is 1–2°. The same bend in 304 stainless is 2.5–3.5° because the yield strength is roughly double and the elastic recovery scales with it. Aluminium 5052 sits between at 1.5–2.5°.

A tool built to a nominal 90° therefore produces 88.5° in CRCA and 87° in stainless unless it is overbent. That is not a tolerance failure, it is the tool being cut for a material. When a part changes from CRCA to stainless after the tool is approved, the bend angle moves by more than the ±1° band and the tool needs a shim or a re-cut.

Thickness also sets the tonnage, and tonnage sets which press the tool goes on. A 1,200 mm cut perimeter in 2 mm CRCA at 300 MPa shear needs 720 kN, or 73 tonne-force, and 900 kN with the stripping allowance. The same part in 3 mm needs 1,080 kN and 1,350 kN with the allowance, which moves it from a 100 T to a 160 T press. Run the numbers with the press tonnage method before the tool is sized, because a tool that only fits the biggest press in the shop is a scheduling constraint for the life of the part.

What does strip camber do to a long part?

Camber is the residual bow in a coil, and it puts a slow curve into every part cut from it. A coil that is 0.10 mm out of straight over 1,000 mm carries a 1 in 10,000 bow. Over a 300 mm pitch that is 0.03 mm of lateral drift per advance, which the pilot pins absorb; over a 900 mm part it is 0.09 mm of bow across the blank, which no pilot can absorb because the metal is already curved.

The measurable result is a part that measures inside tolerance on the die and outside it on a surface plate. A 900 mm chassis rail that is 0.09 mm bowed in the strip can close up or open out by 0.3 mm after trimming, because releasing the blank releases the stress that held the bow. That is why long parts carry a straightness callout with a reference length, and why the coil specification includes camber rather than only thickness and width.

Camber is a material property, so the control is incoming inspection and coil handling. A decoiler that pulls the strip against a badly aligned straightener adds bow; a coil stored on its side and dented at the edge adds a kink that shows as a step in the blank outline. Check the first and last 20 m of a coil, because the outer wraps take the handling damage.

What tolerance applies to a drawn or coined feature?

A drawn feature is looser than a pierced one, and a coined feature is tighter, so the two ends of the same part can hold bands that differ by a factor of four. A 12 mm diameter emboss 1.5 mm high in 1.6 mm CRCA holds its height to ±0.15 mm and its diameter to ±0.20 mm, because the metal thins at the punch nose and the exact height depends on the blank that fed it.

Coining is the other extreme. A coined rib or a flattened boss is pressed between closed tools at stresses above yield, so the feature takes the tool dimension and holds ±0.05 mm on height. The tonnage for coining is high, often 2–3 times the blanking load for the same area, and that is the trade: a tighter feature costs press capacity rather than tool precision.

The rule for a drawing is to say what the feature does. A boss that takes a screw needs a height band and a pilot hole; a rib that stiffens a panel needs a minimum height and no tolerance at all, because nothing assembles to it. Tolerancing a stiffening rib to ±0.05 mm adds cost to the tool and buys nothing at assembly.

How do you prove a tolerance before releasing the drawing?

You cannot prove it from a first article. A first article shows that the tool can make one good part on one afternoon; capability shows that it makes good parts across a run, a coil change and a sharpening cycle.

The minimum useful study is 25 subgroups of five consecutive parts, 125 pieces in total, taken across at least three coils. From that you get a within-subgroup sigma and an overall sigma, and the two indices that buyers argue about. For a ±0.10 mm position callout, a process sigma of 0.033 mm gives Cp = 0.20 ÷ (6 × 0.033) = 1.01, which is a process that will produce rejects. To reach Cpk 1.33 with the mean centred, sigma has to come down to 0.025 mm, and that is a tool decision: add a pilot, add a restrike, or move the feature into a station where it is cut with its datum.

A short study is worse than none, because it produces a number that sounds authoritative and is not. The confidence interval around an estimated Cpk of 1.33 spans about ±0.18 at 125 pieces and about ±0.36 at 30 pieces. Read that second band back: a 30-piece study reporting 1.33 is consistent with a true value of 0.97, which is a process that will ship rejects. The buyer who accepts the 30-piece number has bought a probability, not a capability.

Sampling frequency follows the risk, not the habit. A feature at Cpk 1.33 needs a sample every few hundred parts with a control chart; a feature at Cpk 2.0 can run on a first-off and last-off check. The stamped part inspection guide sets out which features belong on the first article, which on the patrol inspection and which on the annual layout.

How is this verified at Ganesh Multitech?

Tools are designed and built in the in-house tool room, with checking fixtures made alongside the die, so the fixture that proves the part is built to the same datum as the tool that makes it. Presses run from 20 T to 300 T with 250 T punching, which covers a 1,200 mm perimeter at 3 mm without splitting the operation.

Formed tolerance is ±0.5 mm typical on a stamped part, tighter on critical features by agreement, and the custom-part range is 0.8–40 mm. First article inspection and PPAP documentation are available where the programme asks for them, and the tolerance study goes on the PPAP record rather than into a file that only the supplier sees.

The company has manufactured since 1992 across five units in Mumbai (Vasai) and Nagpur, under ISO 9001:2015 and ISO 14001:2015. Customers include Mahindra, Mahindra Powerol, Godrej & Boyce, TKE, Eros Elevators, Minda, Gunnebo and Indian Railways, and the Farm Division sheet metal supply to Mahindra carries an Annual Commodity Award. The stamping capability page lists the press range and the tool room scope behind those numbers.

What belongs on the drawing?

• Material, grade and thickness with its tolerance class, because 0.10 mm of thickness change moves tonnage by 5%.
• The assembly datum, placed on a feature cut in the first or second station.
• Each critical dimension with its own tolerance, not one general note for the whole part.
• The features that are allowed to run to ISO 2768-1 class m, stated explicitly so the toolmaker knows where to spend effort.
• Bend angle and flange height separately, since they are separate process capabilities.
• Flatness with a reference length, for example 0.2 mm per 100 mm, not a bare 0.2 mm.
• Burr height and burr side, and whether deburring is included.
• The inspection method for each critical feature, so the supplier and the customer measure the same way.
• Annual volume and expected tool life, because a 200,000-stroke programme and a 2,000,000-stroke programme justify different tooling.

When a progressive die cannot hold the tolerance

A progressive die cannot hold ±0.05 mm on a formed feature, cannot hold a burr under 0.02 mm without a shave or a fine-blank operation, and cannot hold a flatness of 0.05 mm per 100 mm on a thin panel that has been trimmed. It is also the wrong route for a part under about 5,000 pieces a year, where the tool cost per part is larger than the process saving.

We do not fine-blank in-house, we do not run presses above 300 T, and we do not grind or machine features after forming unless the route says so. Where a drawing needs any of those, the honest answer is a different process or a different supplier, and the quote should say which. Send the revision with the critical dimensions marked through the RFQ form, and the stamping and press tools hub carries the rest of the design rules behind the numbers above.