A drawn part does not have one tolerance. It has several, and they are not equally hard to hold. A diameter set by the last draw or sizing stage behaves completely differently from a wall thickness produced by the blank, and a sealing face that must hold a fine band is a machining question rather than a forming question. Treating every dimension on the print as if it belonged to the same class is the most common reason a drawn part looks expensive before it is even quoted.
What tolerances can deep drawing hold?
Deep drawing holds different tolerances on different features rather than one blanket figure. Diameters set by the final draw or a sizing stage are the most controllable and are commonly quoted between plus or minus 0.05 and 0.15 mm on small shells, widening with diameter. Height and overall length are typically plus or minus 0.1 to 0.5 mm and depend on whether the end is coined or trimmed after forming. Wall thickness follows the strip tolerance where the wall is only drawn, and follows the punch-to-die gap where the wall is ironed, where 0.3 to 1.5 mm walls are routine. Concentricity and roundness depend on tooling alignment across stages, not on the press. Any feature that must be tighter than the forming process can economically hold should be machined after drawing, and that is a deliberate process choice rather than a fallback.
A drawn part has four tolerance zones, not one
Separate the drawing into four groups before deciding what is achievable. Formed dimensions are made by the tool. Wall thickness is made either by the strip or by the ironing gap. Form and position characteristics are made by tool alignment across the stages. Machined features are made after the part is formed, and are the only place a fine band belongs.
| Feature | What sets it | Where the tolerance comes from |
|---|---|---|
| Outside diameter, drawn | Final draw or sizing die | Die bore less the elastic recovery of the material |
| Inside diameter or bore | Punch diameter, plus any ironing pass | The punch, or the ironing ring where the wall is thinned |
| Height and overall length | Last forming stage, plus coining or trimming | Springback, and whether the end is trimmed after forming |
| Wall thickness, drawn only | The incoming blank | Strip thickness tolerance is the wall tolerance |
| Wall thickness, ironed | The punch-to-die gap | A tool dimension, not a process accident |
| Concentricity and runout | Tooling axis across every stage | How well the stages share one axis |
| Roundness and straightness | Number of stages and the sizing pass | Improves down the draw sequence |
| Sealing face, thread, bearing seat | Machining after drawing | The only group where a fine callout is realistic |
The ranges you will see quoted, and the conditions attached
Trade tolerance charts quote ranges for drawn features. They are useful as a starting point and dangerous as a promise, because every figure in them carries conditions. These are the ranges that appear in published drawings and supplier charts, with the condition that has to be true for each to hold.
| Feature | Ranges quoted in trade charts | Condition attached |
|---|---|---|
| Drawn outside diameter, small shells | plus or minus 0.05 to 0.15 mm | Sizing stage included; measured on the sizing face; material and thickness fixed |
| Drawn outside diameter, larger parts | plus or minus 0.15 to 0.3 mm | Same, at a larger diameter where elastic recovery is a bigger share of the band |
| Height or overall length | plus or minus 0.1 to 0.5 mm | The end is trimmed or coined after forming, not left as drawn |
| Wall thickness, drawn only | roughly 5 to 10 per cent of nominal | The blank thickness tolerance is the wall tolerance |
| Wall thickness, ironed | commonly 0.3 to 1.5 mm wall | An ironing ring is in the tool; the wall is a tool dimension |
| Concentricity or coaxiality | 0.05 to 0.2 mm | All stages share one tool axis |
| Roundness | 0.03 to 0.1 mm | A sizing pass follows the main reduction |
| Perpendicularity of a trimmed face | 0.05 to 0.2 mm | The end is cut, not torn |
| Flatness of a coined bottom | 0.05 to 0.15 mm | The bottom is coined after drawing |
| Surface roughness on ironed faces | Ra in the region of 0.4 to 1.6 micrometres | Set by tooling finish and lubricant, not by the press |
None of these is a commitment. On a specific part the achievable figure depends on the items in the next section, and on any part the drawing decides. Where a dimension has to be tighter than forming can hold economically, the honest engineering answer is to machine that face after drawing rather than to ask the die for it.
Why a formed wall is a different class from a machined one
A machined surface is produced by a tool moving relative to a rigid workpiece, so its tolerance is largely a machine and fixturing question. A drawn wall is produced by material flowing, and it changes thickness and hardness as it flows. The wall thickness varies around the circumference and along the height because the blank did not arrive uniform and because the material at the bottom of the cup did not travel as far as the material at the rim. A single nominal wall value on a drawing is a starting point, and it needs a measurement point before it is enforceable. This is why our own guidance is to name where the wall is measured, not only what it should be.
What sets the achievable tolerance
- The number of forming stages and their sequence. More stages mean more consolidation, but also more chances for the axis to drift.
- The annealing schedule between stages. Forming raises yield strength and reduces ductility, and a part that has work hardened will not follow the die the same way.
- Material grade and temper. The same nominal grade supplied full hard and annealed behaves like two different materials. See temper selection for drawn parts.
- Whether functional surfaces are finished after drawing. Coining, trimming, sizing, turning or grinding after forming is usually cheaper than tightening the die.
- Tooling alignment across the stages. Concentricity is a property of the tooling axis, not of how firmly the part was held.
What the drawing should actually state
Define the functional datums first, then mark the dimensions the assembly genuinely depends on, and leave the rest general. For a drawn housing that is usually the bore or a locating diameter, concentricity, overall height and any sealing face. Say where the wall thickness is measured. Name the acceptance method, whether that is a drawing dimension, a gauge, a first article report or a functional check. An ambiguous tolerance is what turns an acceptable part into a rejected lot. Our guide to specifying a drawn part and the drawing requirements checklist cover the same ground from the buyer side.
What applies when the drawing says nothing
Dimensions that carry no individual tolerance are governed by the general tolerance stated in the drawing's title block. Our default, where a drawing does not state otherwise, is ISO 2768-m. That is the medium class, and it is the right default for a formed part: it is loose enough not to over-constrain a drawn wall and tight enough to keep the part in line with the machining that follows. What each class actually contains is set out in our ISO 2768 general tolerances page.
How the tolerances are held and verified
Capability is demonstrated rather than asserted. The gauging lives in-house: a 2.5D optical measuring projector, an instant vision measuring system, a digital height gauge with 0.001 mm resolution, a portable surface roughness tester, a Rockwell hardness tester and a model 20 salt spray chamber, supported by outside micrometers, three-point bore micrometers, plug and go-no-go gauges and a concentricity gauge. The full list is on the inspection lab page. Capability studies are run on the characteristics the control plan marks as significant, and batch heat treatment, slow wire cutting, passivation, electropolishing, plating, phosphating and coating are placed with qualified external processors and disclosed on the inspection plan.
Key point
Ask for the four zones separately: formed dimensions, wall thickness, form and position, and machined features. Tighten only what the assembly uses, state where the wall is measured, and let formed surfaces carry ISO 2768-m unless the function says otherwise. Anything tighter than forming can hold belongs on a machined face after drawing.
Frequently asked questions
Can you hold 0.05 mm on a drawn diameter?
Often, yes, on a small drawn shell where a sizing stage is included and the material and thickness are fixed, but it is not a blanket figure and it widens with diameter. It also matters whether the diameter is formed or machined. On a drawn housing a 0.05 mm band is realistic on a sizing diameter or a machined bore, and less realistic on a large as-drawn diameter.
Why is the wall thickness on my drawing not being met when the diameters are?
Because in a drawn wall the thickness is produced by different things at different heights. Where the wall is only drawn, its thickness follows the strip tolerance and thins as material stretches. Where the wall is ironed, thickness is set by the punch-to-die gap and is far more uniform. Adding a measurement point and, if needed, an ironing or sizing pass is usually the fix rather than tightening the blank.
Should I tolerance a deep drawn part like a machined part?
No. A drawn surface is a formed surface, and asking forming to hold a machining class raises tooling cost and inspection time without improving the part. Split the drawing: fine bands on the features that are machined after drawing, forming-class tolerances on the features the die produces, and the general class everywhere the assembly does not care.
What tolerance applies if I do not put one on the drawing?
The general tolerance named in the title block. Where a drawing does not state one, our default is ISO 2768-m, the medium class. It is deliberately chosen for formed parts, because a formed wall should not be constrained to the fine class by accident.