Most of the price difference between two quotes for the same part comes from a handful of features: the bearing seats, the bores that must line up, and the hole patterns that bolt the part to the rest of the machine. This guide looks at those three features specifically, shows how their tolerances change the machining and inspection route, and explains how to specify them so the part works without paying for precision it does not need.
Short answer.
- Bearing seats need a fit from the bearing maker’s table (commonly H7 or J7 in housings), plus roundness and perpendicularity to the shoulder. Making them tighter than the bearing needs adds boring, temperature control and CMM time without improving the bearing.
- Bore positions are cheaper and clearer when controlled with a position tolerance from functional datums than with tight ± coordinates. In a simple geometric comparison, a round zone that encloses the square of a ± tolerance covers about 57% more area; whether that is acceptable depends on the function and datums.
- Hole patterns for bolts can usually take much more tolerance than drawings give them. With clearance holes, the allowable position tolerance follows directly from hole size minus bolt size.
How a tolerance changes the machining route
Cost does not rise smoothly as a tolerance gets smaller. It rises in steps, each time the tighter limit forces a different process, a different inspection method or more scrap risk.
| Tolerance on a feature | Typical route | Typical inspection | Relative effort |
|---|---|---|---|
| General, for example ISO 2768-m (±0.1 mm up to 6 mm, rising to ±0.5 mm at 400 mm) | Standard milling or turning | Calipers, height gauge | Baseline |
| ±0.02 to ±0.05 mm | Separate finishing pass, stable fixturing | Micrometers, bore gauges, plug gauges | Moderate |
| About ±0.01 mm, or a bearing fit such as H7 on a bore | Boring or reaming, tool wear compensation, controlled part temperature | Bore gauge or CMM | Significant |
| ±0.005 mm and tighter | Grinding, honing or wire EDM after machining | CMM in a temperature controlled room | Highest; scrap risk rises |
Effort grows further when the tolerance links features machined in different setups, because the datum has to be transferred between fixtures.
Bearing seats: specify the fit the bearing needs
A bearing seat is the feature most worth controlling tightly, and also the one most often over or under specified. Four things define it:
- Diameter and fit. Use the bearing maker’s recommendations for your load and rotation. For housings with a stationary outer ring under normal load, these tables commonly give H7 or J7; rotating inner rings usually sit on k5 or k6 shafts. For example, a Ø32 H7 bore is 32.000 to 32.025 mm.
- Form. Roundness or cylindricity matters as much as size, because an oval bore distorts a thin bearing ring. Specify it when the bearing maker does.
- Orientation to the shoulder. The shoulder that locates the bearing should be perpendicular to the bore axis. A tight diameter with no perpendicularity control can still tilt the bearing.
- Surface finish. Bearing makers commonly call for Ra 0.8 to 1.6 µm in housing bores. A rougher bore wears in and loosens the fit.
In aluminum housings, check the effect of temperature: aluminum expands about twice as much as bearing steel, so a fit that is correct at room temperature loosens as the housing warms. That is a design decision for the engineer responsible for the assembly, and it is worth stating the operating temperature on the drawing or in the RFQ.
If the housing is anodized, the bore shrinks. Either mask the bearing seat or state that the fit applies after finishing; see the anodizing allowance guide.
Bore positions: use position tolerance from functional datums
Two common ways to locate a bore give very different results for the same intent.
± coordinates, for example 50.00 ±0.05 in X and Y, create a square tolerance zone 0.1 mm wide. The worst acceptable point is in the corner of that square, about 0.0707 mm from the true position.
A position tolerance can use the circle that just encloses that square. Its diameter is 0.1√2 mm, about Ø0.1414 mm, and the round zone it creates around the true position contains the whole square. Every bore inside the original square is also inside the circle, and bores close to the true position but slightly outside the square in X or Y are accepted too. That circumscribed circle is about 57% larger in area than the square (a ratio of π/2). This is an illustrative geometric comparison: it shows why position tolerance usually wastes less of the available tolerance. Converting an existing ± requirement to a position tolerance still needs the design owner to check the function, the datum scheme and any related orientation or form controls.
Position tolerance also forces the drawing to say which datums the bore is measured from. That removes a frequent source of disputes: when the datums are not stated, the shop and the inspector can measure from different edges and both be right.
Coaxial bores on opposite faces
Two bearing bores that must share an axis, such as the two sides of a joint housing, are the most demanding positional requirement on most robot parts. Coaxiality is easiest to hold when both bores are machined in one clamping, by 5-axis machining, a rotary table or line boring through both. When the part must be flipped, the second bore depends on how accurately the datum is picked up again. If coaxiality is critical, say so on the drawing and identify which bore is the datum.
Hole patterns: let the fastener decide the tolerance
Bolt hole patterns are where drawings most often ask for more precision than the assembly needs. When parts are joined with bolts through clearance holes, the position tolerance that still guarantees assembly can be calculated directly, using the fastener formulas from ASME Y14.5:
- Floating fastener (bolt through clearance holes in both parts, nut on the other side): position tolerance = clearance hole diameter minus bolt diameter. For M6 bolts in Ø6.6 mm holes, that is Ø0.6 mm on each part.
- Fixed fastener (bolt through a clearance hole into a tapped hole): position tolerance on each part = (clearance hole diameter minus bolt diameter) divided by two. For the same M6 bolt and Ø6.6 mm hole, Ø0.3 mm on each part.
These formulas rest on stated assumptions: the holes and fasteners are at maximum material condition, the position tolerance is applied at MMC, the fastener is straight, and the total tolerance is split equally between the two parts. For a fixed fastener, any tilt of the tapped hole is carried through the thickness of the mating part, so ASME Y14.5 recommends a projected tolerance zone on the tapped hole; without one, less tolerance is really available. Counterbored holes, thick parts, press-fit pins and unequal splits need their own calculation. The figures above are worked examples, not drawing values: the final tolerance comes from the designer’s tolerance analysis.
Compare that with a drawing that gives every hole ±0.02 mm. The pattern then needs a finishing route and CMM inspection, and the bolts fit no better. Where location really matters, use dowel pins for location and let the bolts only clamp. The dowel holes get the tight tolerance; the bolt holes do not.
When the pattern must sit accurately relative to other features but the holes need to be accurate mainly to each other, composite position tolerancing can control both levels separately. It is worth discussing during drawing review rather than defaulting to one tight value for every hole.

Size tolerance and geometric tolerance are separate controls
A hole’s diameter and its position are separate requirements. A thickness tolerance does not control flatness. A tight diameter on a bearing seat does not control its roundness or its squareness to the shoulder. Specify the requirement that represents the function, then agree how it will be checked.
A checklist before you send the drawing
- Bearing seats: fit from the bearing maker, form, perpendicularity to the shoulder, surface finish, operating temperature.
- Bores that must align: datums identified, position or coaxiality tolerance, which bore is the reference.
- Bolt patterns: position tolerance from the fastener formula, dowels where location matters.
- Everything else: a general tolerance note such as ISO 2768-m.
- Finishing: whether dimensions apply before or after anodizing or plating, and which surfaces are masked.
Make the cost comparison useful
Ask for two versions of the quotation: one with the present drawing and one with clearly identified relaxations on noncritical features. Keep material, quantity, finish and inspection scope the same. Any relaxation should be reviewed and approved by the engineer responsible for the assembly before it becomes the production requirement.
In drawing review we flag tolerances that will drive a grinding or CMM route, bores that cannot be held coaxial in the proposed setup, and hole patterns that look tighter than their fasteners need. We do not change tolerances on our own; the design owner decides.
Frequently asked questions
What tolerance should a bearing bore in an aluminum housing have?
Use the bearing maker’s recommended fit for your load and rotation, commonly H7 or J7 for a stationary outer ring, and add roundness, perpendicularity to the shoulder and a surface finish around Ra 0.8 to 1.6 micrometers. Consider the operating temperature, because aluminum expands about twice as much as bearing steel.
Is position tolerance more expensive than plus or minus tolerances?
Often it is not. In a simple geometric comparison, a round zone that encloses the plus or minus square covers about 57% more area, and a position tolerance makes the measuring datums explicit. Whether an existing drawing can be converted depends on the function and datums, so the design owner should confirm it.
How much position tolerance do bolt holes need?
Assuming maximum material condition and an equal split between the parts: for bolts through clearance holes in both parts, the position tolerance on each part can equal clearance hole diameter minus bolt diameter, for example 0.6 mm for M6 bolts in 6.6 mm holes. For a bolt into a tapped hole, use half of that on each part, and consider a projected tolerance zone on the tapped hole. These are worked examples; the final value comes from the tolerance analysis.
Which tolerances drive CNC machining cost the most?
Tolerances that force a change of process, such as boring, grinding or honing, and tolerances that link features machined in different setups. Inspection by CMM in a controlled room adds further time.
Explore precision machining for critical fits, use the RFQ drawing checklist, or send your drawing for a tolerance review.
References
- ISO 286-1 and ISO 286-2, Geometrical product specifications: ISO code system for tolerances on linear sizes.
- ISO 2768-1, General tolerances for linear and angular dimensions.
- ASME Y14.5, Dimensioning and Tolerancing (position tolerance and fastener formulas).
- Bearing manufacturers’ catalogs on shaft and housing fits, for example SKF and Schaeffler.
