The Price of One Decimal Place: How Tolerances Drive the Cost of CNC Parts

The most expensive characters on a technical drawing are not the diameters or lengths - they are the small annotations next to them: H7, Ra 0.8, tolerance class "f". Most of them get there out of habit, not necessity - and every one of them triggers a specific, measurable chain of costs in the machine shop. This article shows how that chain works and which tolerances you can safely loosen.

Two identical parts, two different prices

In the classic cost estimating handbook published by SME continuously since 1968, there is an example that deserves a place above every design engineer's desk. Two turned pins, identical at first glance - they differ only in the tolerance on the same diameter. The first has a tolerance of ±0.002 in. (±0.05 mm). The second: +0.000/-0.001 in. (+0.000/-0.025 mm).

On the drawing, that is a difference of one annotation. In the shop, the difference looks like this:

• the first pin can be made directly from cold-drawn bar stock as delivered - its natural accuracy is sufficient, and the diameter needs no machining at all;
• the second pin requires larger-diameter stock, turning that diameter with a different, slower method, and two cuts - roughing and finishing - because one cut will hold neither the dimension nor the required surface quality.

Same geometry, same material, same function in the machine - and the cycle time and price jump. That is not the shop being difficult. That is physics and arithmetic.

Where the cost of a tolerance comes from

Tightening a tolerance is never "free", because it always changes how the part must be made. Back in 1972, in his handbook on time norms for machine tools, the Polish author Romuald Wołk stated it plainly: for lower surface quality classes a single pass with the right feed is enough, while higher classes require at least two - a roughing pass and a finishing pass. Fifty years later the machines have changed; the principle has not.

A tighter tolerance raises cost through several channels at once:

• more passes - the material allowance must come off in stages, with decreasing depth of cut;
• slower parameters - finishing passes run at lower feeds;
• additional operations - reaming, fine boring, grinding, honing; often a separate clamping, a separate tool, and sometimes a separate machine;
• more measurement - a toleranced dimension has to be checked, sometimes on every piece;
• higher scrap risk - the narrower the tolerance zone, the easier it is to fall out of it, and the cost of scrap is spread over the good parts.

The SME handbook compresses this into one sentence worth quoting verbatim: keep machining to a minimum and tolerances as loose as the requirements allow.

Designed by Magnific

Level 1: general tolerances to ISO 2768

The "ISO 2768-mK" note in the drawing frame applies to every dimension without an individual tolerance - typically 90% of the dimensions on the part. The letter defines the accuracy class for linear dimensions:

For CNC milling and turning, class m is the natural default - a machine in good condition holds it without special effort. Class f applied to the whole part means every dimension, including those with no functional significance, must be machined and inspected tighter: more careful finishing passes, more measurement, less margin for tool wear. You end up paying for precision on surfaces that nothing will ever touch.

The practical rule: general class m, with tighter callouts only on the specific dimensions that truly need them.

Level 2: hole fits to ISO 286

The symbol next to a hole - H11, H9, H7 - is not cosmetic; it is a choice of manufacturing process. Every step down the ladder means a narrower tolerance zone and usually an additional operation. For a Ø10 mm hole it looks like this:

H7 is justified where the hole mates with a bearing, a bushing, or a dowel pin. But H7 written "on autopilot" on clearance holes for bolts is the classic mark of an expensive drawing: an M8 bolt in a Ø9 hole will never notice the difference between H7 and the general tolerance - the quote will.

Level 3: surface roughness Ra

Roughness works like fits - each threshold means another operation, not just a "nicer surface". In milling and turning practice: Ra 3.2 is the standard result of proper machining; Ra 1.6 takes careful finishing passes; Ra 0.8 means slow feeds and good conditions; Ra 0.4 and below usually means grinding - a separate machine, a separate setup, and an extra cost often larger than all the prior machining of that surface. A low "global" roughness written in the drawing frame acts as a multiplier on the whole part.

The master rule: tolerance only what touches something

Let us reduce all of this to a checklist you can run through before sending a drawing out for quotation:

1. Is the general tolerance class m (not f) - and does it really need to be anything else?
2. Does every individually toleranced dimension describe a surface that works with something - mates, guides, seals, locates?
3. Are fits (H7 etc.) only on functional holes, not on clearance holes for bolts?
4. Is low roughness limited to sliding, sealing, or contact surfaces?
5. Can you say out loud the reason for the tightest tolerance on the drawing?

Among the iron rules of estimating, the SME handbook lists reviewing the required tolerances carefully - and querying the design department when they are missing or doubtful. A good machine shop will do exactly the same: it will ask whether H7 on ten holes is a requirement or a habit. On a mid-size part, loosening two or three unnecessary tolerances can cut the price by tens of percent - with no change in function whatsoever.

The fastest way to see it is live: in MetronQ quoting, the customer clicks a surface on the 3D model, tightens its tolerance, and immediately sees the price change. There is no better lesson in the cost of tolerances than a control that converts them into money in real time.

PS If you want to check what such automated quoting costs a shop - the pricing is here.