CNC Machining Tolerance Cost: IT Grades, H7 Routes and Inspection

A bracket drawing calls a ⌀20 mm H7 bore and a title-block note of “general tolerance ±0.05 mm”. One shop costs the bore as drill and ream, another as boring; the drawing does not say which. The quote gap is not margin but process, pass count and inspection routine behind the same two characters.

After reading this, you will know which tolerance decisions reach a CNC quote, and you can estimate the price delta before release.

The answer up front: tolerance reaches the quote through the machining line only. IT11–12 takes 1.0, IT8–9 1.2 and IT6–7 1.5 on cutting time. Boring rows use 1.3 and 1.8. Roughness is a separate row coefficient; first-article inspection a separate order-level line. Material and post-processing do not move. The five-line structure is in the CNC machining cost breakdown; the CNC quote calculator applies the coefficients below, and this article covers one line.

Change on the drawing	Line that moves	New coefficient
IT11–12 to IT8–9	Cutting time on the affected rows	1.2 (from 1.0)
IT8–9 to IT6–7	Cutting time on the affected rows	1.5 (from 1.0)
Bored hole at IT8–9 or IT6–7	Boring row only	1.3 / 1.8
Ra 3.2 to Ra 1.6	Row time on the finished faces	1.3
Ra 1.6 to Ra 0.8	Row time on the finished faces	2.0
First-article report added	Order-level inspection line	Entered per order

Multipliers on time, not a price list: the currency value depends on the machine rate.

Four Sources of Tolerance Cost

A tighter tolerance changes how the part is cut, held and measured.

Slower feed and speed. A narrower band leaves less room for tool deflection, spindle growth and thermal movement, so the finishing pass runs lighter.

More passes. A callout finished in one pass often becomes rough, semi-finish and finish. Each pass carries a tool change and a scrapping risk.

Fixturing and setup. A tight feature must sit in the same position from first cut to last: soft jaws, a dedicated fixture, a temperature soak or an in-process check.

Inspection. The tighter the callout, the more of the batch is measured, and the more likely a bore gauge, pin gauge or CMM replaces a caliper. Inspection is a separate line because the order drives it, not cutting time.

Why Published Multipliers Mislead

Tormach’s tolerance-cost chart puts a 0.005 in part at roughly twice the cost of rough machining at 0.030 in, a 0.001 in part at four times, and a 0.0001 in part at 24 times. Criterion Precision reports that precision parts typically cost 30–50% more than standard-tolerance parts, and that a blanket ±0.0005 in callout can double machining time and add 40% to inspection.

Both are sanity checks, not a pricing table. The Tormach curve is relative to rough machining, not the previous step, and is in inches. The Criterion figures compare whole classes of parts, not one changed callout. A buyer who reads 4× as “the cost of 0.001 in” will overprice a part with one tight bore.

This model prices each feature as a row, applies the factor to that row’s cutting time, and leaves material and post-processing alone. The coefficients are estimates from project experience in our CNC quote calculator (2026-10), not a survey of shops, and should be calibrated against won jobs.

row cost=cutting time (min)×roughness coefficient÷60×machine rate×material difficulty×tolerance coefficient

Change the tolerance coefficient and only the row cost moves; change the machine rate and every row on that machine moves.

The IT Grade Coefficient Table

IT grades classify the width of a dimension tolerance, from IT01 to IT18; a smaller number is a narrower band. A drawing may state the grade, inherit it from a general-tolerance note, or imply it through a fit callout such as H7.

General tolerances are covered by GB/T 1804-2000, equivalent to ISO 2768-1:1989, which defines four classes, f, m, c and v, for dimensions without individual tolerance. IT grades and fit letters come from GB/T 1800.1-2020, a modified adoption of ISO 286-1:2010. The general note fills untoleranced dimensions; H7 sets a fit. Neither tells the shop which process to use.

Drawing basis	Precision key	Coefficient on cutting time
IT11–12	it11_12	1.0
IT8–9	it8_9	1.2
IT6–7	it6_7	1.5
Not stated or not confirmed	unknown	1.0

The factor is applied per row, not to the part total. A part with one IT6–7 bore and twenty general faces does not carry 1.5 on everything. Assign the grade to the rows that carry the callout and leave the rest at 1.0.

A turning row with 12 minutes of baseline time at ¥80/h costs ¥16.00 at IT11–12. At IT8–9 it is 14.4 minutes and ¥19.20; at IT6–7, 18 minutes and ¥24.00. Across 100 pieces the row moves by ¥320 or ¥800. The tolerance change moves that per-piece line, not the one-off block; cost per part by quantity separates the two.

What the Coefficient Multiplies

Cost line	Moves with the tolerance grade?	Why
Material	No	Blank weight and unit price are set by the drawing and the purchase lot
Programming and setup	Not automatically	A proving cut can be added by hand; the coefficient does not inflate setup
Machining	Yes	Cutting time on the rows assigned that grade
Post-processing	No	Priced per kg, per piece or per area
First-article inspection	Separate line	Order-level, entered from the customer’s inspection requirement

If a quote moves when you relax a tolerance, and material and finish are unchanged, the difference should be traceable to the machining rows or to inspection. Ask for those two lines. If the whole quote moves by the same percentage, you are looking at margin, not tolerance cost. The material line has its own basis — blank weight, loss factor and grade price — covered in material cost.

Exception: a tight feature can force an extra proving cut, and a shop may add setup hours. Our model does not add them. If your shop does, enter them in the setup line.

H7 Holes: Three Routes, Three Prices

H7 is a hole tolerance class, not a process. It can be made by drill and ream, precision drilling, or boring, each with a different time base, tool cost and inspection need. A drawing that says H7 alone is under-specified.

The table prices one ⌀20 mm through hole, 25 mm deep, in 45# steel at ¥80/h, Ra 3.2, difficulty 1.0. Base times are calculator estimates: 3 minutes for the 13–30 mm band plus 1 minute per 25 mm, ream at 1.15 over drill time, boring at 6 minutes times the depth-to-diameter ratio.

Route	Row type	Time estimate	Effective minutes per hole	Cost per hole at ¥80/h
Drill and ream	Ream, composite	(3 + 25/25 × 1) × 1.15 × 1.5	6.9	¥9.20
Precision drilling	Drill	(3 + 25/25 × 1) × 1.5	6.0	¥8.00
Boring	Bore	6 × (25/20) × 1.8	13.5	¥18.00

For four holes the feature costs ¥36.80, ¥32.00 or ¥72.00. The spread is the price of not naming the route.

• The ream row is composite: a pilot drill and the ream, at 15% over drill time before the precision factor.
• The drill row is cheapest, but a drilled hole is not automatically H7. Whether the route holds the callout depends on diameter, depth, material and tooling. The row prices time; it does not certify the process.
• The boring row is 6 minutes times the depth-to-diameter ratio, then the bore factor. At small diameters its base time is large compared with drilling.

A fourth variant is drill plus a separate boring row: two rows, so the total differs from a single boring row at the same rate.

It is a pricing comparison, not a capability ranking. The H7 callout can be quoted three ways, and the drawing does not choose. Put the route on the RFQ. The CNC quote calculator can reproduce the line you intend to buy.

Boring Has Its Own Table

Boring and precision-turned holes use a dedicated set: IT8–9 at 1.3 and IT6–7 at 1.8, applied once. Do not also apply the general table; 1.2 × 1.3 = 1.56 and 1.5 × 1.8 = 2.7 would count the same decision twice. The model chooses one table per row.

The factors are higher because a boring bar is a single-point finishing operation, set, checked and often adjusted between passes. On a lathe, a bore row uses the lathe rate; the coefficient does not change. A precision-turned outside diameter uses the general table on the turning row.

Deep bores are the limit of the model: time scales with the depth-to-diameter ratio, but bar deflection is not modelled. Beyond the shop’s comfort, override the row with trial-cut minutes.

A ⌀50 × 100 mm bore is 12 minutes of base time. At IT8–9 it becomes 15.6 minutes (¥20.80 at ¥80/h); at IT6–7, 21.6 minutes (¥28.80).

Tolerance and Ra Compound

Tolerance and roughness are separate callouts acting on the same row time. Both are multipliers, so they compound rather than add.

Surface callout	Coefficient	12-minute row	Cost at ¥80/h
Ra 3.2	1.0	12.0 min	¥16.00
Ra 1.6	1.3	15.6 min	¥20.80
Ra 0.8	2.0	24.0 min	¥32.00
Ra 0.4	2.0 provisional cap, range only	Not a grinding price	Range output

A row at IT6–7 and Ra 0.8 carries both: 12 × 1.5 × 2.0 = 36 minutes, or ¥48.00. The multipliers are sequential, not additive. That combination is the expensive pattern, and a blanket note costs more than a local one.

Ra 0.4 usually needs grinding. The model suppresses the single-point price when a Ra 0.4 row has no grinding row, returning a range. The 2.0 provisional cap is not a grinding price; a grinding row is priced separately at the grinder rate.

Relaxing finish on non-functional faces is the cheapest saving. Move Ra 0.8 from every face to the sealing or sliding faces; leave the rest at Ra 3.2.

Inspection Is an Order-Level Line

First-article inspection is charged once per order and spread across the batch. The calculator defaults the line to zero; the requirement belongs to the customer and drawing, not the machining template.

It does not reset on repeat orders. Programming may be reused, but if the customer requires a first-article report every time, the cost stays. What drives the amount is the requirement: how many dimensions are critical, which gauge is used, and what report is required. At one piece that order-level line falls entirely on the single part, which is why CNC prototyping cost is dominated by charges paid once per order.

A process-sequence cost often travels with a tight part. When a heat-treatment fee is priced and any row is IT6–7 or Ra 0.8 or finer, the calculator raises a two-stage warning: heat treatment distorts the part, so the finishing cut follows it. The price covers one stage unless the second is added. This is not inspection; it is a second machining stage.

Put the inspection requirement on the RFQ: if 40 dimensions exist and six are critical, say which six and which gauge.

Relaxing Tolerance Without Losing Fit

The cost lever is not “loosen everything”. It is to separate faces that perform a function from faces that merely exist.

• Review the tolerance callout
• Locates or seals
• Yes→keep it and change the process
• Clearance only→check the fit before relaxing
• No→relax to the general tolerance
• Sets the assembly
• Yes→run a stack-up before changing
• No→relax, then re-check the stack
• Global or local
• Global note→move it to the critical faces
• Already local→leave it
• Can the shop prove it
• Yes→keep it and name the gauge
• No→change route or redesign the fit

Functional and mating faces keep their callout. If the face locates a bearing or seals a joint, the tolerance is part of the function. Change the process or split the tolerance.

Non-functional faces go to the general tolerance first. A face that only clears a casting or carries a nameplate does not need a callout. Removing it is free.

A local callout beats a blanket note. Six tight faces cost less than the same note on sixty, and the shop sees which faces matter. A callout the shop cannot measure is not enforceable.

What the Standards Fix and Do Not

GB/T 1804-2000 covers general tolerances for linear and angular dimensions without individual tolerance indication. It is equivalent to ISO 2768-1:1989 and defines four classes: fine (f), medium (m), coarse © and very coarse (v). It fills in the dimensions the drawing left blank. It does not set process capability.

GB/T 1800.1-2020 is the GPS standard for the ISO code system of tolerances on linear sizes, a modified adoption of ISO 286-1:2010. It defines IT grades and fit letters. H7 is a hole tolerance class: the H fundamental deviation with grade 7. The width still depends on the nominal size band.

We do not reproduce the standard tables. Use the standard or your shop’s table for the micrometre values; the coefficients here are costing multipliers. A drawing needs both the general-tolerance note and the individual fit callouts, and neither chooses the route.

Frequently Asked Questions

How much does a tighter tolerance add to a CNC quote?

It depends on the row. Moving a row from IT11–12 to IT8–9 multiplies cutting time by 1.2; to IT6–7, by 1.5. A 12-minute turning row at ¥80/h goes from ¥16.00 to ¥19.20 to ¥24.00.

Is ±0.01 mm too tight for CNC machining?

The number alone cannot answer that. Nominal size, feature, material, depth and the shop’s process decide whether a callout is routine or needs a second operation. Ask which route will hold it and which gauge will prove it. If either answer is vague, it is not yet priced.

What is the difference between H7 and IT7?

H7 is a hole tolerance class: the H fundamental deviation with grade 7. IT7 is the grade itself. The H7 width equals the IT7 width for the same size band, with the hole’s lower deviation at zero.

Why do two quotes for the same H7 hole differ?

Usually because the route differs. Drill-ream, precision drilling and boring have different time bases and inspection needs. The same ⌀20 × 25 mm hole at IT6–7 runs 6.9, 6.0 and 13.5 effective minutes before the rate. Ask each shop to name the route and the setups.

Does a tighter tolerance make a better part?

Only if the function needs it. A tight tolerance narrows the permitted variation; it does not improve the material, fit design or surface if those are wrong. On a non-functional face it adds cost without adding function.

How is inspection cost quoted?

As an order-level line: charged once per order and spread across the batch. The driver is the requirement, not the grade: how many dimensions are critical, which gauge is used, and what report the customer wants. Our calculator defaults it to zero.

Before You Release the Drawing

Three sentences to carry away. First, tolerance cost is a machining-line cost: the grade multiplies cutting time, and material and finish do not move with it. Second, an H7 callout without a route is not a comparable quote; name the route and inspection method. Third, put the tight callout on functional faces and let the general tolerance carry the rest.

References

• ISO 2768-1:1989 — General tolerances — Part 1: Tolerances for linear and angular dimensions without individual tolerance indications
• ISO 286-1:2010 — Geometrical product specifications (GPS) — ISO code system for tolerances on linear sizes — Part 1
• GB/T 1804-2000 — General tolerances: tolerances for linear and angular dimensions without individual tolerance indications
• GB/T 1800.1-2020 — GPS — ISO code system for tolerances on linear sizes — Part 1
• Tormach — The High Cost of Tight Tolerances
• Criterion Precision — How to Reduce Cost on Precision Machined Parts Without Sacrificing Quality

To see the multipliers on your own part, open the CNC quote calculator, set the precision key on the rows that carry the callout, and compare with the same rows a grade down. The difference is the tolerance cost. To have the route and inspection line checked before you send the RFQ, send the drawing and report requirement to our engineering contact. We will check which rows carry the callout, whether the route matches the gauge, and which inspection line belongs on the order. The six-step walk-through is in the calculator guide.