Tolerance levels that can be achieved by various machine tool processing methods
A working reference for engineers who need to pick a process before they draw the GD&T. Each method below comes with the range it holds every day, the range it can hold when everything is dialed in, and the surface finish that ships with it. Use it to set realistic callouts instead of arguing with a supplier after the first article.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
- 8
Key takeaways
What tolerance levels that can be achieved actually depend on
When someone asks about tolerance levels that can be achieved, the honest answer starts with the machine, then immediately moves to the part. A machine tool quoted at ±0.002 mm positioning accuracy will not deliver ±0.002 mm on a 300 mm aluminum bracket with four setups. Setup error, thermal drift, tool wear and clamping distortion each add their own share, and they add up faster than most people expect.
A practical rule we use on the floor: the achievable tolerance on a real part is roughly 2 to 3 times the machine's positioning spec, once you account for workholding and material. That is why a shop can hold ±0.005 mm on a small stainless fitting and still quote ±0.02 mm on a large plate from the same machine.
Material matters as much as the machine. Aluminum 6061 and 7075 cut clean and let you push a light finishing pass without chatter. Austenitic stainless 304 and 316 work-harden at the cutting edge, so the last pass has to remove enough material to get under the hardened skin. Titanium Ti-6Al-4V and Inconel move the other way: they deflect, they hold heat, and they punish any tool that rubs instead of cuts.
So before choosing a process, answer three questions. How rigid is the part? How many setups does it need? Which feature actually carries the function? Then match the process to the tightest functional feature, not to the whole drawing. Everything else can stay loose and save money.
- 1Rigid part, one setupYou can plan close to the machine's capability.
- 2Thin wall or long overhangExpect 2–3× the error from deflection alone.
- 3Multiple setupsEach re-datum adds its own stack-up contribution.
- 4Heat-treated materialDistortion shows up after machining, not during it.
Turning, milling, drilling and boring: the everyday ranges
Turning handles cylindrical features better than anything else on a lathe. On a rigid shaft with a supported end, OD and ID turning holds ±0.01 mm routinely and ±0.005 mm on diameter when you use a finish pass and control the insert wear. Concentricity between two turned diameters in the same chucking typically lands within 0.005–0.01 mm. Move the same feature to a second operation and that number opens up to 0.02–0.03 mm unless you use a collet and a soft jaw set cut in place.
Milling is where most parts live, and it is also where tolerance claims get optimistic. A 3-axis mill cutting a pocket in 6061 holds ±0.025 mm on position and ±0.01 mm on a reamed hole. Tighten to ±0.01 mm and you need a finishing pass with a sharp tool, a warm machine and a stable fixture. Five-axis simultaneous work adds rotary axis error, so ±0.02 mm across a contoured surface is a realistic production number, not ±0.005 mm.
Drilling is a locating operation, not a finishing one. A twist drill wanders, so a drilled hole alone is typically ±0.1 mm on position and H12 on diameter. Reaming takes it to H7 and ±0.025 mm. Boring is the precision answer: a single-point boring head on a rigid setup holds ±0.005 mm on diameter and 0.005 mm on roundness, and it can correct a hole that was drilled slightly off-center.
Planing and shaping are rarely the right answer for tight work today. They still make sense for long flat ways and for surfaces where tool marks are acceptable, but the flatness they hold, around 0.02–0.05 mm over 300 mm, is beaten by a surface grinder.
Grinding, lapping and when to stop chasing numbers
Grinding is the process that changes the conversation. A surface grinder with a dressed wheel holds ±0.005 mm on thickness and 0.002–0.005 mm on flatness over a 100 mm face, and it does it repeatedly. Cylindrical grinding on a hardened shaft reaches ±0.002 mm on diameter with 0.002 mm roundness. That is the practical ceiling for most production parts, and it is where the cost curve turns steep.
Below that, you are in lapping and honing territory. Lapping brings flatness to 0.001 mm and finish to Ra 0.05 μm, but it is slow, it needs a dedicated plate, and it is usually reserved for sealing faces, gauge blocks and valve seats. Honing does the same job inside a bore. Both are finishing operations: the geometry has to be correct before the part reaches them.
Here is the trade most engineers miss. Going from ±0.02 mm to ±0.005 mm on a milled feature might triple the cycle time, because you add a semi-finish pass, a finishing pass and a temperature soak. Going from Ra 1.6 μm to Ra 0.4 μm on the same feature is a separate cost, and it may need a different tool or a different machine entirely. Specify them independently.
Ask one question before you add a tight callout: does this feature need to be tight, or does it need to be consistent? A bearing bore needs a tight diameter and a controlled fit. A mounting face needs flatness and a good finish. Confusing the two is how drawings get expensive without getting better.
Part geometry, setup count and the error nobody budgets for
Every additional setup adds a datum transfer. On a part with three setups, the stack-up from fixture location alone can reach 0.02–0.03 mm before the machine contributes anything. This is why we push hard for features that can be cut in one orientation, and why a 5-axis machine often pays for itself on parts that look simple on paper.
Thin walls, deep pockets and long slender features behave differently. A 1 mm wall on an aluminum housing will spring under clamping pressure and then relax after unclamping, so the measured dimension changes between the machine and the CMM. Rough the part, stress relieve it if the material allows, then take a light finishing pass with reduced clamping force.
Heat treatment is the other silent variable. A 4140 part that is quenched and tempered after roughing will move. Leave 0.3–0.5 mm of stock for the finishing operation, and expect to re-establish datums after heat treat rather than trusting the ones from the soft state.
Tool wear is a slow drift, not a step change. On a long run, an unmanaged finishing tool will walk 0.005–0.01 mm over a few hundred parts. That is manageable if you have in-process checks and a tool-life plan, and unmanageable if the first article is the only measurement anyone takes.
- 1One setup beats threeFewer datums, less stack-up, lower cost.
- 2Clamp light on thin wallsReduce force and take two light passes.
- 3Leave stock for heat treat0.3–0.5 mm on critical faces.
- 4Plan tool lifeLog the finishing tool and change it on count, not on feel.
Step by step: choosing and holding a tolerance
Run these in order. Skipping step 2 is the most common reason a first article fails.
- 1List the functional features onlyMark the surfaces that mate, seal, slide or locate. Everything else gets a general profile tolerance of ±0.1 mm or looser. This alone removes most of the cost from a typical drawing.
- 2Match each feature to a processHoles that locate get reamed or bored. Round bearing seats get turned or ground. Flat sealing faces get milled then ground if flatness matters. Do not assign a tolerance before you assign a process.
- 3Check the setup countCount how many orientations the part needs. If the tight feature is on the opposite side of a loose feature, consider a 5-axis machine or a redesign. Each extra setup adds 0.01–0.03 mm of uncertainty.
- 4Set the finishing allowanceLeave 0.2–0.4 mm on surfaces that will be finish-milled, 0.3–0.5 mm before heat treat, and 0.02–0.05 mm for a grind. Too little stock causes rubbing and work hardening; too much causes deflection.
- 5Define the inspection methodState the instrument and the datum. Micrometer for diameters, CMM for position, surface tester for Ra. If the drawing does not say, the shop will pick the fastest method and the numbers will not match yours.
- 6Run a capability check on the first articleMeasure the critical features on the first part and on the tenth. If the spread is more than a third of the tolerance band, the process is not stable yet. Adjust the finishing parameters before releasing the run.
- 7Lock the process and monitorOnce the first article passes, freeze the tool paths, the fixture and the finishing parameters. Add in-process checks at a fixed interval, and log tool changes against measured drift.
Tolerance and finish by machining method
Routine values are what we quote without special discussion. Achievable values need a stable setup, a finishing pass and an inspection plan.
| Method | Routine tolerance | Achievable tolerance | Typical finish |
|---|---|---|---|
| CNC turning (OD/ID) | ±0.01 mm | ±0.005 mm | Ra 0.8–1.6 μm |
| CNC milling (3-axis) | ±0.025 mm | ±0.01 mm | Ra 0.8–1.6 μm |
| 5-axis milling (contour) | ±0.02 mm | ±0.01 mm | Ra 0.8–1.6 μm |
| Drilling (twist drill) | ±0.1 mm | ±0.05 mm | Ra 3.2–6.3 μm |
| Reaming | ±0.025 mm | ±0.01 mm | Ra 0.8–1.6 μm |
| Boring | ±0.01 mm | ±0.005 mm | Ra 0.4–0.8 μm |
| Surface grinding | ±0.005 mm | ±0.002 mm | Ra 0.2–0.8 μm |
| Cylindrical grinding | ±0.005 mm | ±0.002 mm | Ra 0.2–0.4 μm |
Which process to pick for a given callout
| If the drawing says | Pick this | Why |
|---|---|---|
| ±0.05 mm or looser on a milled face | 3-axis milling, one pass | No finishing operation needed |
| ±0.01 mm on a bore that locates | Bore or ream, then verify | Single-point boring corrects position |
| ±0.005 mm on a shaft diameter | Cylindrical grinding | Turning alone drifts with tool wear |
| Flatness 0.005 mm over 100 mm | Surface grinding | Milling leaves cutter marks and bow |
| Ra 0.4 μm on a sealing face | Fine grind or lap | Milling cannot reach this finish |
| ±0.02 mm across a contoured surface | 5-axis simultaneous | Fewer setups beats tighter machines |
| H7 fit on 20 mm holes, 500 pcs | Ream with a floating holder | Repeatable and fast per hole |
| Thin wall 1 mm, ±0.05 mm | Rough, relieve, light finish | Clamping and spring dominate error |
Set the tolerance to the function, then pick the process
Tolerance levels that can be achieved are decided by the feature, the setup count and the material long before they are decided by the machine spec. Send us the drawing and we will tell you which callouts are realistic, which ones need a process change, and which ones you can loosen without losing function.
Questions engineers ask before releasing a drawing
Can one shop hold ±0.005 mm on every feature of a part?
Not on every feature, and any supplier who says yes without looking at the part is guessing. The limit is a property of the feature, not the shop. A short, rigid, round feature on a stable material can be ground to ±0.002 mm. A long, thin, unsupported wall on the same part may only be good to ±0.05 mm.
The practical approach is to keep the tight callout on the features that carry function and let the rest run loose. That keeps the part manufacturable and the price reasonable.
Does a 5-axis machine give tighter tolerances than a 3-axis machine?
Not automatically. A 5-axis machine adds rotary axis error, so its single-feature accuracy can be slightly worse than a well-set 3-axis machine. What it improves is the number of setups, and that is usually where the real error comes from.
On a part that would need four orientations on a 3-axis machine, a 5-axis machine holding ±0.02 mm will beat the same part made in four setups at ±0.05 mm stack-up.
How do I translate a tolerance into a surface finish callout?
They are linked but not interchangeable. A turned or milled surface at ±0.01 mm usually lands at Ra 0.8–1.6 μm. If you need Ra 0.4 μm or better, plan a grinding or lapping operation, and expect the tolerance to tighten along with it.
Do not specify Ra 0.2 μm on a milled face unless the function truly needs it. It adds a whole operation for a number nobody will measure after assembly.
Why does my part measure in tolerance at the shop and out of tolerance at incoming inspection?
Different instrument, different datum, different temperature. A part measured on a CMM at 20 °C and on a caliper in a warm inspection room can differ by 0.01 mm on a 100 mm feature from thermal expansion alone.
Agree on the measurement method in the drawing or the PO. If the feature is critical, ask for the inspection report with the instrument and the temperature noted.
What is the tightest tolerance available on a turned part without grinding?
On a rigid shaft with a supported end and a controlled finishing pass, ±0.005 mm on diameter is repeatable. Below that, tool wear and thermal drift take over and you need cylindrical grinding.
If the part is long or slender, expect the deflection to dominate and plan for ±0.02 mm or looser, or add a steady rest and reduce the depth of cut.
How much does tightening a tolerance add to the cost?
It depends on the step, not the number. Going from ±0.1 mm to ±0.025 mm on a milled feature is often free, because the same finishing pass covers it. Going from ±0.025 mm to ±0.005 mm usually adds a grinding operation and a separate inspection.
Send the drawing and we will flag which callouts are driving the cost. That conversation takes less time than reworking the first article.
Send a drawing, get a DFM review in 12 hours
Upload the model and we will return a quotation with a free DFM analysis, flagging any tolerance that will drive cost or risk. No minimum order quantity, from one prototype to 10,000+ parts.
12-hour quoteFree DFM analysis100% inspection before shipment
More process notes from GreatLight
We publish setup notes, tooling trials and inspection data from the factory floor.
