Calculations of Dimensions and Fit Tolerances
Written for design engineers and buyers who need to turn a functional requirement into numbers a machine shop can hold. We cover IT grades, hole and shaft deviation, clearance and interference fits, and how to tell when a tolerance is tighter than the process can deliver. Read it once and you can check whether a drawing will assemble or jam before it reaches the shop floor.
From a fit requirement to a tolerance value
A fit is a decision about two numbers: how much space you allow, and how much you can afford to lose.
Reading IT grades without a standards library
Tolerance grades run from IT01 to IT18. The number is a quality index, not a size. Move up the grade and the tolerance band gets wider at the same nominal diameter. IT01 is the tightest band in the system, IT18 the loosest, and the value in micrometres depends entirely on the diameter you are working with. A Ø10 mm shaft at IT7 and a Ø200 mm shaft at IT7 are not the same tolerance in micrometres, even though they share a grade.
The grade alone tells you how precise a feature must be. The fundamental deviation letter tells you where the band sits relative to the nominal size. Put the two together and you have a full tolerance callout, for example Ø40 H7 or Ø40 g6. On a drawing this is the part that decides assembly, not the grade on its own.
Grades are chosen by function, not by habit. Slip fits for locating pins usually land around IT6 to IT7 on both members. Press fits need IT6 or tighter on the shaft so the interference range stays predictable. Clearance holes for fasteners rarely need better than IT9 to IT11. If a designer writes IT5 on a bolt clearance hole, the shop will ask why, because the extra cost buys nothing at the joint.
- 1IT01 to IT4Gauge blocks, spindle tooling, reference pins. Rarely used on production parts.
- 2IT5 to IT7Precision fits, hydraulic bores, bearing seats, precision shafts.
- 3IT8 to IT11General machined fits, locating bores, clearance holes for fasteners.
- 4IT12 to IT18Cast, forged or flame-cut surfaces, non-critical spacing.
Hole tolerance, shaft tolerance and fit tolerance
A hole has an upper limit Dmax and a lower limit Dmin. Hole tolerance TD is the difference, Dmax minus Dmin, and it equals the difference between the upper deviation ES and the lower deviation EI. A shaft works the same way: shaft tolerance Td is dmax minus dmin, or the gap between the upper and lower deviation of the shaft. Neither number depends on the other member. Each feature earns its own band from the drawing.
Fit tolerance Tf is different. It is the sum of the two bands, TD plus Td. That sum sets how much the clearance or interference can vary across a production run. A small Tf means tight control of the assembly condition. A large Tf means the joint may swing from loose to tight as parts come off the machine, even when both features are in tolerance.
Maximum clearance Xmax appears when the largest hole meets the smallest shaft: Dmax minus dmin. Minimum clearance Xmin appears when the smallest hole meets the largest shaft: Dmin minus dmax. If Xmin is positive, the fit is always clearance. If Xmax is negative, the fit is always interference. When the range crosses zero, a given pair of parts may assemble with a slight clearance or a slight interference depending on where each part landed in its band.
- 1TD = Dmax − Dmin = ES − EIHole tolerance, independent of the shaft.
- 2Td = dmax − dminShaft tolerance, independent of the hole.
- 3Tf = TD + TdFit tolerance, the variation the joint can see.
- 4Xmax = Dmax − dmin, Xmin = Dmin − dmaxClearance range for the assembly.
Common fit types and when they are used
Values are functional guidance for machined metal parts at the sizes shown. Always check the governing standard for your application.
| Fit type | Typical callout | Assembly | Where it fits |
|---|---|---|---|
| Slip fit | H7 / g6 | Hand assembly, light oil film | Locating pins, sliding sleeves, spigots |
| Close running fit | H7 / f7 | Free rotation, minimal play | Bushings, gearbox shafts, spindles |
| Location clearance | H7 / h6 | Light tap or push, near zero play | Dowelled plates, precision covers |
| Transition fit | H7 / k6 | Light press or light tap | Gear hubs, bearing inner rings |
| Press fit | H7 / p6 | Hydraulic press or shrink | Bushes, valve seats, bearing outer rings |
| Heavy press | H7 / s6 | High force or thermal shrink | Permanent joints, hardened inserts |
What a CNC shop can actually hold
Tolerance math and machining reality meet at the spindle. Our floor holds ±0.005 mm (±0.0002 in) on critical features when the geometry allows it. That is a shop capability, not a promise for every feature on every part. Long slender bores, thin walls and deep pockets push the achievable band wider because tool deflection and thermal growth move the cut.
Material matters too. Aluminium 6061 and 7075 cut cleanly and hold a tight band well. Stainless 316L and 17-4PH work-harden, so finishing passes need lighter depths and sharp tooling to avoid pushing the dimension. Titanium TC4 and Inconel move more under heat, which means rough, semi-finish and finish passes are separated by a cool-down. For a bore that must hold an H7 fit, the boring bar and the coolant strategy matter as much as the tolerance callout.
Surface finish and tolerance travel together. A bore at Ra 0.2–0.8 μm usually pairs with a tight diameter band because it needs a fine finishing pass. General milled surfaces at Ra 1.6–3.2 μm sit comfortably with IT8 to IT11 bands. Tightening the finish without a reason adds cycle time and does not improve the fit.
- 1Short, rigid featuresEasiest to hold at ±0.005 mm.
- 2Long bores over 5×DExpect the band to widen; add a reaming or boring pass.
- 3Thin walls under 1.5 mmChatter and springback control the result.
- 4Hardened or gummy alloysTool wear shifts size mid-run; plan for in-process checks.
Checking a drawing before it is released
A fit calculation is only useful if the drawing carries the result. Write the nominal size, the deviation letter and the grade on the feature, for example Ø25 H7, and add the limit dimensions in a table for the shop. If a feature is functionally critical, mark it and state the gauge or method the shop should use. This removes the argument about which dimension matters.
Watch the stack. A single tight fit is manageable. Five tight fits on the same part, spread across different faces, force extra setups and raise the risk of a scrap. On a bore pattern, ask whether position tolerance or diameter tolerance is doing the real work. Often one of them can relax without affecting assembly.
Finally, separate the tolerance from the finish. They are different requirements with different costs. A callout of Ø30 H7 with Ra 1.6 μm describes two things, and the shop will quote them separately. If the design only needs the fit, keep the finish realistic for that fit.
- 1Mark critical featuresSay which diameter, bore or face sets the fit.
- 2Give limit dimensionsSaves the operator from doing standards lookups at the machine.
- 3Check the stackMany tight fits on one part multiply setups and risk.
- 4Do not over-specify finishA finish callout is a separate cost from the diameter band.
Questions engineers ask about fit tolerances
Can the shop hold an H7 bore in stainless steel?
Yes, when the bore is short enough and the wall is thick enough to stay rigid. We hold ±0.005 mm on critical features in stainless 316L and 17-4PH, but a deep bore over five times its diameter needs a boring or reaming pass and a stable setup.
Send the drawing with the limit dimensions and the finishing requirement. We check the geometry during DFM analysis and flag any feature where the requested band is not realistic for the material and tool reach.
How do I calculate the clearance range for a specific fit?
Use the limits, not the nominal size. Maximum clearance is the largest hole minus the smallest shaft. Minimum clearance is the smallest hole minus the largest shaft. Both come straight from the deviation values in the standard.
If the minimum clearance is negative, part of your range is interference. That is fine for a press fit, but it means a given pair of parts may need force or heat to assemble. State the expected assembly method on the drawing so the shop knows the joint is not hand-fit.
Does a tighter IT grade always cost more?
Usually yes. A tighter grade needs finer tooling, slower finishing passes and more inspection. There is also a practical floor. Below a certain band, the process cannot hold it across a run without grinding or lapping, which changes the routing.
The cost jump is not linear. Going from IT9 to IT7 on a bore may be a small change. Going from IT7 to IT5 on a long bore can add a separate finishing operation and a gauge check.
When should I use a transition fit instead of a press fit?
Use a transition fit when the parts must stay concentric but you still want to disassemble them for service. A light press or tap fit locates the parts without permanent deformation.
Use a press fit when the joint carries torque or must never move. That joint depends on the interference to transmit load, so the interference range has to be controlled on both members.
Do I need to specify surface finish with a fit tolerance?
Only if the function needs it. A tight fit is about the diameter band. A fine finish is about friction, sealing or appearance. They are separate requirements and separate cost lines.
For a sliding or rotating fit, finish does affect wear and lubrication. For a static locating fit, a standard machined finish at Ra 1.6–3.2 μm is usually enough.
Can you review a fit before I release the drawing?
Yes. Upload the model or drawing and we return a quotation and a free DFM analysis within 12 hours. We point out features where the tolerance, finish or geometry will be hard to hold and suggest an alternative where one exists.
Uploads stay confidential. An NDA is available on request for programs that need one.
Send us the drawing and the fit callout
We will check the tolerance against the material and geometry, and tell you which features can hold the band and which ones need a change.
12-hour quoteFree DFM analysis100% inspection
