A minus 0.003 mm tolerance means one thing: the tool measures at or below nominal, never above. If the catalogue says 0.500 mm, the drill is between 0.497 mm and 0.500 mm.
That single sentence carries a lot of engineering.
What the tolerance is, and what it is not
It is a statement about the tool. It is not a statement about the hole.
A drilled hole is larger than the drill that made it, by roughly 0.5-3% of diameter in ductile materials. The difference comes from runout, from wander on entry, from built-up edge and from elastic recovery of the work material.
A -0.003 mm tool therefore does not produce a -0.003 mm hole. What it does is remove one source of error from the stack.
Where the stack-up matters
Take a 0.5 mm hole with a +/-0.02 mm requirement. The error budget looks roughly like this:
| Source | Typical contribution |
|---|---|
| Tool diameter | -0.003 to 0 mm |
| Holder runout | 0.002-0.010 mm |
| Wander on entry | 0.005-0.020 mm |
| Built-up edge | 0.005-0.015 mm |
| Thermal growth | 0.001-0.005 mm |
The tool tolerance is the smallest line in that table. That is the point: it is the only line the toolmaker controls, so it should not consume the budget.
Runout is usually the largest line and the easiest to fix. For a drill below 1 mm, keep total indicated runout under 0.005 mm. Above that the drill behaves as a single-flute cutter and cuts oversize.
Why negative rather than plus-minus
A symmetric tolerance would allow a tool above nominal. In most drilling operations an oversized tool is the worse error:
- A hole that will be reamed needs the drilled hole below the reaming allowance.
- A hole that takes a press-fit pin needs the top of the hole tolerance to hold.
- A hole that will be tapped needs material left for the thread.
A one-sided tolerance makes the failure direction the recoverable one.
How it is held in production
The tolerance comes from grinding to the minus side of nominal and then measuring. At 0.5 mm the window is 6 µm, comparable to the resolution of a good optical measuring system. Every part number is measured, not sampled.
Two things can destroy the tolerance after it leaves the grinder:
- Coating. A 3 µm PVD layer on each flank adds up to 6 µm to the diameter. Coated series therefore carry their own diameter record, and the uncoated series is the one quoted at -0.003 mm.
- Regrinding. A reground drill is smaller, not larger. If a re-sharpened tool is used where the tolerance matters, it has to be re-measured.
What it does not fix
The tolerance does not compensate for a worn collet, a dirty shank or a spindle with 0.01 mm of play. Those errors are larger than the tolerance itself.
It also does not turn a drill into a reamer. A drilled hole typically lands in IT9-IT11. A reamed hole reaches IT7-IT8. If the drawing asks for IT7, the answer is a reamer such as CM326, not a tighter drill.
FAQ
Is -0.003 mm the same as h6?
No. A shaft tolerance class is defined per diameter band and includes both sides of nominal. This is a unilateral catalogue tolerance expressed in absolute millimetres.
Which series carry this tolerance?
The uncoated DC326 record is quoted at -0.003 mm, across 0.04-3.175 mm and 542 part numbers.
Does the tolerance hold after coating?
Coated series are ground and then coated, and their diameter is specified as coated. Do not apply the -0.003 mm figure to a coated part number.
How should I measure it?
A micrometer with 0.001 mm resolution at three positions along the margin, or an optical comparator. A caliper is not adequate at 0.5 mm.