Drawing and RFQ Guide for Machined Parts
CNC Machining Tolerance Cost: How Drawing Requirements Change a Quote
Tight tolerances do not carry one universal price premium. Cost changes when a requirement alters the manufacturing route, setup stability, tooling, cycle time, scrap risk, finishing sequence or inspection plan. A clear drawing helps a supplier price the features that matter instead of adding contingency for ambiguity.
Use this guide to separate functional requirements from defaults, state the correct standard edition and prepare a feature-level tolerance review before ordering custom machined parts.
Before Requesting a CNC Quote
- Identify the dimensions and geometric relationships that control fit, function, sealing, motion or interchangeability.
- Define datums from functional interfaces rather than convenient raw-stock edges.
- State the governing dimensioning and tolerancing standard with its edition.
- Use individual tolerances or GD&T for critical features; do not depend on a general tolerance note to communicate a special fit.
- State whether requirements apply before or after coating, heat treatment, polishing or another secondary process.
- Define the inspection method or acceptance intent when it affects the result.
- Send the matching CAD model and controlled drawing revision.
For manufacturing and inspection capabilities, review services d’usinage CNC sur mesure et CNC inspection planning.
What Makes a CNC Tolerance More Expensive?
| Facteur de coût | Why it changes the process | Useful drawing or RFQ action |
|---|---|---|
| Tolerance relative to feature size | A small permissible variation may require a more stable finishing step, additional offsets, environmental control or a different process. | State the functional limit on the individual feature instead of applying it across the drawing. |
| Relationship across setups | Position, profile, runout or orientation between faces cut in different setups adds datum-transfer and workholding risk. | Define functional datums and allow the supplier to review whether features can be completed in one setup. |
| Thin, long or flexible geometry | Cutting and clamping forces, residual stress and temperature can change the free-state result. | Define wall/floor thickness, restraint condition, free-state requirement and acceptable inspection setup. |
| Deep or inaccessible feature | Long tools, small bores, undercuts and deep pockets reduce rigidity and complicate chip removal and measurement. | Increase access or radius where function permits; identify which hidden features are critical. |
| Material and condition | Machinability, hardness, thermal behavior, internal stress and lot condition influence stability and tool wear. | Specify exact grade, temper/condition, form, heat treatment and substitution rules. |
| Secondary processing | Heat treatment, coating, plating or polishing may change size, form or surface and require allowance or post-process machining. | State the final-condition requirement and the governing process specification. |
| Inspection and reporting | A difficult characteristic may require special fixturing, programming, calibrated gauges or a detailed report. | Define sampling, report format, ballooning, FAI and any customer-specific measurement method. |
| Quantity and repeatability | One prototype, a pilot lot and repeat production justify different fixture, tool-control and inspection strategies. | Provide current quantity, forecast and expected repeat-order cadence. |
Because these factors interact, a credible supplier cannot quote a fixed percentage increase from tolerance alone. Two features with the same numerical tolerance can require very different manufacturing and verification routes.
ISO 2768 Status: State the Exact Part and Edition
ISO 2768-1:1989 addresses general tolerances for linear and angular dimensions without individual tolerance indications. ISO lists that edition as published and current, while its stage is “to be revised” and a replacement is under development. Check the official ISO 2768-1 record immediately before issuing or quoting a drawing.
ISO 2768-2:1989, previously used for general geometrical tolerances, is withdrawn. ISO identifies ISO 22081:2021 as its replacement. The old combined shorthand found on legacy drawings may still be contractually relevant, but a buyer and supplier must agree which dated documents govern. See the withdrawn ISO 2768-2 record.
A title-block note does not authorize either party to silently substitute a newer, older or “equivalent” standard. Resolve legacy callouts, customer specifications and drawing notes during contract review.
Do not copy a tolerance table from a blog
Use the licensed standard named by the drawing. Online summaries can omit scope, exclusions, definitions, revision changes and rules that determine whether a table entry applies.
General Tolerances Are Not a Substitute for Functional Requirements
A general tolerance controls eligible dimensions that do not have an individual indication, within the scope and rules of the specified standard. It does not automatically define surface texture, edge condition, thread class, fits, free-state behavior, coating allowance or every geometric relationship.
Use a General Tolerance For
Eligible noncritical dimensions where a common drawing default reflects design intent and the governing standard is clearly identified.
Use an Individual Size Tolerance For
Fits, thicknesses, diameters, depths or clearances whose limits directly affect assembly or function.
Use GD&T For
Form, orientation, location, profile or runout relationships that need to be evaluated from defined datums and according to a stated standard.
ASME describes Y14.5 as establishing symbols, rules, definitions and practices for stating and interpreting GD&T and related requirements. If this system governs the drawing, specify its edition rather than mixing rules from an ISO GPS standard. Review the ASME Y14.5 record.
Match the Control to the Functional Question
| Functional question | Requirements to consider | Quotation risk if unclear |
|---|---|---|
| Will the shaft and bore assemble? | Fit system or explicit limits, material condition, temperature, coating and inspection method. | The supplier may price a needlessly narrow symmetric tolerance or miss the final-condition fit. |
| Will holes align with the mating part? | Datum scheme, basic dimensions, position requirement, material-condition modifier and fastener clearance. | Coordinate tolerances may obscure functional allowance and create an inefficient inspection plan. |
| Will a rotating feature run correctly? | Bearing datums, runout or coaxial relationship, surface, balance and operating condition. | Independent diameters may pass size checks while the functional relationship remains undefined. |
| Will a face seal? | Seal design authority requirements, flatness/profile, surface texture parameter, direction and defect criteria. | A generic “smooth finish” note cannot define leakage performance or acceptance. |
| Will a flexible part fit when released? | Free-state or restrained condition, fixture method, datum targets and permitted deformation. | Manufacturing and inspection fixtures may force different shapes without a common evaluation condition. |
| Will coated parts remain within limits? | Masking, coating thickness, pre/post-process dimensions and final inspection stage. | Machining may meet the drawing before finishing but fail the intended final assembly. |
Datum Strategy Can Reduce Ambiguity and Setup Cost
Datums should represent the interfaces that locate or orient the part in its assembly. When critical features reference unrelated or unstable surfaces, the machining fixture and inspection alignment may struggle to reproduce the intended relationship.
- Choose a primary datum that establishes a stable functional orientation.
- Use secondary and tertiary references to constrain the remaining degrees of freedom in a way that matches assembly.
- Avoid dimension chains when the end relationship is what matters; dimension important features from a shared functional reference where appropriate.
- Identify datum features that are interrupted, very small, flexible, inaccessible or modified by finishing.
- Agree how datum simulators, targets or constrained conditions will be established during inspection.
This is design-authority work. A manufacturer can identify ambiguity and propose a manufacturable alternative, but should not change the datum scheme without documented customer approval.
Material, Geometry and Final Condition Affect Achievable Results
A tolerance is not independent of the part. Thin aluminum plates can move when released from a fixture; heat-treated steel can change after thermal processing; engineering plastics can respond to moisture, temperature and residual stress; slender turned parts can deflect during cutting and measurement.
Tell the supplier the exact material specification, grade, temper or condition, product form and any stability treatment. For thin walls, long overhangs, deep bores or large material removal, define the inspection state and functional priority. If a surface will be anodized, plated, painted, polished, ground or heat treated, say which dimensions and geometric requirements apply in the final condition.
Inspection Requirements Belong in the Quote
The same manufacturing requirement can create different total costs depending on how it must be verified and documented. Inspection planning should consider access, equipment range, resolution, uncertainty, fixture, program development, sample size and report format.
- Specify critical characteristics and their required coverage.
- State whether variable measurement data or a functional go/no-go result is needed.
- Identify first-off, first-article, in-process and final-report requirements separately.
- Define whether a ballooned drawing, customer template, material certificate or special-process certificate is required.
- Do not demand one instrument by name unless the measurement method itself is a contractual requirement.
- Confirm whether results apply before or after unclamping, conditioning or finishing.
What a Tolerance DFM Review Should Return
A useful review does not simply ask the buyer to loosen every tolerance. It identifies the specific requirement, explains the manufacturing or measurement risk and proposes an option that preserves the functional intent.
| Review output | Example of useful detail |
|---|---|
| Ambiguity list | Conflicting CAD/drawing dimensions, missing standard edition, undefined datum, incomplete thread or finish callout. |
| Feature risk | Deep bore, thin wall, cross-setup relationship, post-treatment movement or inaccessible inspection point. |
| Process option | Change setup sequence, add finishing allowance, use a dedicated fixture, change tool access or evaluate another process. |
| Design option | Increase an internal radius, shorten a deep pocket, relocate a datum or change tolerance form while preserving function. |
| Inspection proposal | Characteristic, method, stage, sample, report and final-condition definition. |
| Commercial impact | Identify which option changes setup, tooling, inspection, lead time or risk; price the actual drawing instead of using a generic multiplier. |
RFQ Checklist for Tight-Tolerance CNC Parts
- matching 3D CAD model and revision-controlled 2D drawing;
- governing tolerancing standard, part number and exact edition;
- functional datums, critical-to-quality features and assembly context;
- size limits, GD&T, fits, threads, surface texture and edge requirements;
- material specification, grade, condition, form and traceability;
- heat treatment, coating, finishing, masking and final-condition requirements;
- quantity, forecast, repeat cadence and approved quantity breaks;
- first-article, sampling, dimensional report and measurement-method requirements;
- approved substitutions, deviation authority and change-control requirements;
- delivery destination and required arrival date.
CNC Machining Tolerance Cost FAQs
How much does a tighter CNC machining tolerance increase cost?
There is no reliable universal percentage. Cost changes only when the tolerance alters the process, setup, tooling, cycle time, scrap risk, finishing or inspection. Send the drawing so the supplier can identify and price the affected features.
Does ISO 2768 define the tolerance for every CNC feature?
No. A specified edition provides general tolerances only within its scope and rules for eligible dimensions without individual indications. It does not replace functional size limits, GD&T, fits, threads, surface texture, edge conditions or final-condition requirements.
Is ISO 2768-2 still current?
No. ISO lists ISO 2768-2:1989 as withdrawn and identifies ISO 22081:2021 as its replacement. Legacy contracts may still name the withdrawn edition, so the buyer and supplier must confirm the exact governing documents rather than silently substituting standards.
Should I apply the tightest tolerance to every drawing dimension?
No. Apply requirements according to function and risk. Overly restrictive noncritical dimensions can add manufacturing and inspection cost without improving the assembly. Critical features still need explicit, unambiguous controls.
What files are needed for a CNC tolerance review?
Send the matching CAD model and controlled drawing with standard edition, datums, critical features, material, final condition, quantity and inspection requirements. Assembly context or a mating-part definition can help explain functional intent.
Get a Drawing-Specific CNC Tolerance Review
Upload your CAD model and controlled drawing. Lauens can review process, material, critical features, finishing and inspection before preparing a quotation. Any tolerance or measurement capability becomes a commitment only when approved for the actual feature and order.
