CNC True Position Inspection: Hole Location, Datums, MMC and CMM Checks

A hole can be within its diameter limits and still prevent an assembly from fitting. The size may be correct, but the hole axis may be shifted, tilted or related incorrectly to the mounting datums. Coordinate tolerances alone can also create square acceptance zones that do not match the circular clearance available to a fastener.

Position tolerance—often called “true position” in shop language—solves this problem by defining the allowable location of a feature relative to basic dimensions and a datum reference frame. It is one of the most useful and most misunderstood controls on CNC machined parts.

This guide explains position tolerance for holes, pins, slots and patterns; datum setup; RFS, MMC and LMC; bonus tolerance; virtual condition; composite position; CMM and functional-gauge inspection; reporting; common mistakes; and what buyers should include in an RFQ.

What Is True Position in CNC Machining?

The formal geometric characteristic is position. “True position” is a widely used informal phrase for the theoretically exact location established by basic dimensions.

For a cylindrical hole or pin, a position feature control frame commonly defines a cylindrical tolerance zone. The derived axis of the actual feature must satisfy that zone relative to the specified datum reference frame and any stated material-condition modifiers.

Position can control more than center location. Depending on the callout and feature geometry, it can also control orientation of the feature axis relative to the datums. That makes it more functionally useful than checking separate plus-or-minus X and Y coordinates without considering the complete datum system.

The drawing standard and edition matter. ASME Y14.5-2018 establishes symbols, rules and practices for GD&T in ASME-based drawings. ISO 1101:2017 defines the ISO GPS symbol language and interpretation rules for geometrical tolerances including location. Use the standard invoked by the product definition; do not combine defaults from the two systems casually.

Why Plus-or-Minus Coordinates Can Be Misleading

Suppose a hole center is toleranced ±0.10 mm in X and ±0.10 mm in Y. This creates a square coordinate acceptance area. A hole located near a corner of that square can be farther from nominal than a hole at the midpoint of a side, even though both coordinates pass.

A diametrical position zone treats every radial direction consistently. The available location error is described by a cylinder rather than separate rectangular limits. This often matches the functional clearance of a round fastener and round hole more directly.

Position tolerancing can also:

• Reference the surfaces that locate the part in assembly

• Control a complete bolt-hole pattern

• Apply material-condition modifiers

• Allow bonus tolerance as feature size departs from MMC

• Permit datum feature shift when specified

• Support functional fixed or floating fastener calculations

• Define composite pattern requirements

• Be verified with a CMM or functional gauge

The goal is not to make the drawing more complicated. It is to communicate assembly function and acceptance boundaries more accurately.

The Elements of a Position Callout

A complete position requirement normally includes several connected elements.

The position symbol

The feature control frame begins with the position symbol. It identifies the geometric characteristic being controlled.

The tolerance value and zone shape

For a hole or pin axis, a diameter symbol before the tolerance value commonly establishes a cylindrical zone. If the zone is not cylindrical, the drawing must communicate the applicable shape and direction correctly.

Material-condition modifier

The tolerance may apply at maximum material condition (MMC), least material condition (LMC), or regardless of feature size (RFS), depending on the standard and notation.

Datum references

Primary, secondary and tertiary datum references establish the coordinate system and constrain the necessary degrees of freedom. Datum feature modifiers may also affect how the datum reference frame is established.

Basic dimensions

Basic dimensions locate or orient the theoretically exact feature position. They are shown as theoretically exact values under the applicable drawing convention and do not carry a direct plus-or-minus tolerance of their own.

Feature and pattern scope

The leader, dimensioning scheme and surrounding notes identify which hole, pin, slot or pattern the control applies to. An inspector must know whether one feature or the full pattern is being evaluated.

Datum Reference Frames for Position Inspection

A reported position value is meaningless unless the datum reference frame is correct. The primary datum typically removes three degrees of freedom, the secondary removes two more and the tertiary removes the final degree, although cylindrical and specialized datum schemes can behave differently.

Common examples include:

• A mounting face as primary datum A

• A locating bore or pilot as secondary datum B

• A clocking hole, slot or side face as tertiary datum C

• A primary cylindrical shaft datum with a shoulder face for axial location

• A hole pattern used as a datum feature pattern

• Datum targets on an irregular casting or thin structure

The inspection setup must simulate the specified datums in their stated order. Measuring hole coordinates from an arbitrary edge, machining origin or vise jaw does not prove a position tolerance unless that reference represents the required datum system.

The GD&T datums for CNC machining guide explains datum features, datum simulators, precedence, datum shift and CMM alignment in more detail.

Position Tolerance at RFS

When a position tolerance applies regardless of feature size, the geometric tolerance is independent of the actual feature size within its size limits. An acceptable large hole does not automatically gain extra position tolerance unless the drawing and governing standard provide a material-condition modifier that creates it.

RFS is useful when location accuracy must remain consistent throughout the allowed size range. Examples may include:

• Precision dowel holes

• Bearing or bushing locations

• Hydraulic passages that must align with ports

• Features controlled for wall thickness or edge distance

• Holes located for measurement or optical alignment

RFS inspection frequently uses variable measurement such as a CMM, vision system or carefully designed open setup. A simple fixed functional pin gauge may not independently reveal the actual size and axis location needed for the evaluation.

Maximum Material Condition and Bonus Tolerance

Maximum material condition is the feature size containing the greatest amount of material:

• For an internal feature such as a hole, MMC is the smallest permitted diameter

• For an external feature such as a pin, MMC is the largest permitted diameter

When position is specified at MMC, the stated geometric tolerance applies when the feature is at MMC. As the actual feature departs from MMC toward less material, additional geometric tolerance—commonly called bonus tolerance—becomes available.

For an internal hole:

Bonus tolerance = actual hole size − MMC hole size

For an external pin:

Bonus tolerance = MMC pin size − actual pin size

The total available position tolerance is the stated MMC position tolerance plus the applicable bonus tolerance, subject to the full drawing requirements.

Simple hole example

Assume a hole size is 10.00–10.20 mm and the position tolerance is diameter 0.20 mm at MMC.

• Hole MMC = 10.00 mm

• Actual hole = 10.12 mm

• Bonus tolerance = 0.12 mm

• Total available position tolerance = 0.20 + 0.12 = 0.32 mm

This example is intentionally simple. The inspection must still consider datum modifiers, feature form, projected tolerance zones, composite controls and the governing standard.

MMC is especially useful for clearance-hole assemblies because a larger hole provides more assembly clearance and can tolerate more location error without preventing fit.

Least Material Condition

Least material condition is the feature size containing the least material:

• For a hole, LMC is the largest permitted diameter

• For a pin, LMC is the smallest permitted diameter

Position at LMC can help protect minimum wall thickness, minimum edge distance or remaining material around a feature. As the actual feature departs from LMC toward more material, additional tolerance may become available under the applicable rule.

LMC is less common than MMC in general machining drawings, but it is valuable when material preservation is the primary function rather than assembly clearance.

Virtual Condition and Functional Boundaries

Virtual condition is a constant worst-case boundary created by the combined effect of feature size at a material condition and the geometric tolerance at that condition.

For a simple internal feature controlled at MMC:

Virtual condition = hole MMC size − position tolerance at MMC

For a simple external feature controlled at MMC:

Virtual condition = pin MMC size + position tolerance at MMC

Using the 10.00–10.20 mm hole with diameter 0.20 mm position at MMC:

Hole virtual condition = 10.00 − 0.20 = 9.80 mm

A correctly designed fixed functional gauge can represent this boundary for assembly verification. Virtual condition is also useful when checking the relationship between mating hole and fastener requirements.

Do not use these simple equations without confirming feature type, modifiers and the applicable standard. Non-cylindrical features, projected zones, datum mobility and complex assemblies may require additional analysis.

Bonus Tolerance and Datum Shift Are Different

These two allowances are often confused.

Bonus tolerance comes from the controlled feature departing from its specified material condition. For example, a clearance hole larger than its MMC size may receive additional position tolerance.

Datum shift comes from a datum feature of size departing from the material boundary specified in the datum reference. It can allow the datum reference frame to translate or rotate within the permitted clearance, depending on the datum scheme and standard.

They arise from different features and must be calculated and applied separately. A CMM program or manual report that combines them without explanation can produce results that are difficult to audit.

True Position Calculation from X and Y Coordinates

For a simple two-dimensional case with a cylindrical diametrical zone, the radial coordinate deviations may be converted into a diametrical position value:

Position error = 2 × √(ΔX² + ΔY²)

If the measured hole center is +0.05 mm in X and −0.08 mm in Y from the basic location:

Position error = 2 × √(0.05² + 0.08²) ≈ 0.189 mm

This formula is useful for understanding a straightforward planar hole pattern, but it is not a universal inspection method. It can be insufficient when:

• The hole axis is tilted through material thickness

• A three-dimensional datum alignment is required

• The tolerance zone is not diametrical

• MMC, LMC, datum shift or projected tolerance applies

• A composite position control is used

• Surface data and feature fitting affect the derived axis

• The standard defines additional requirements

A validated CMM program or functional gauge may be more appropriate for complex cases.

Position of a Hole Axis Through Thickness

Checking one center point at the top of a hole can miss axis tilt. A hole can enter near nominal and exit significantly displaced on the opposite face.

Inspection methods may evaluate:

• A derived axis from multiple measured circles

• A scanned cylinder fitted to the hole surface

• Separate entry and exit circles

• A projected axis beyond the part surface

• Functional engagement using a long gauge pin

The measurement strategy must reflect the tolerance zone and functional engagement. Thick plates, bearing bores, long dowel holes and stacked assemblies generally require more than a single two-dimensional center measurement.

Projected Tolerance Zones

A projected tolerance zone extends the controlled axis beyond the part surface by a specified height. It is useful when a threaded hole or press-in stud must align with a mating hole located some distance above the mounting face.

Without projection, a tilted threaded hole might satisfy position within the threaded depth yet cause the fastener to interfere with a remote bracket or cover.

The drawing should clearly state:

• Projected zone height

• Direction of projection

• Applicable feature control

• Mating-part or functional requirement

• Inspection method and any gauge length

An inspector should not infer a projected zone merely because a long bolt is used in assembly.

Position Tolerance for Hole Patterns

Bolt circles, rectangular hole arrays and multiple dowel holes require control of both pattern location and feature-to-feature relationships.

Important questions include:

• Where is the pattern located relative to the datum reference frame?

• How closely must holes relate to one another?

• Does pattern rotation matter?

• Are holes used for floating fasteners or fixed fasteners?

• Do dowel holes require tighter relationship than clearance holes?

• Is the pattern itself used as a datum in a later requirement?

A single-segment position control can locate each feature relative to the datums under one requirement. When pattern refinement is needed, a composite position tolerance or separate controls may be appropriate.

Composite Position Tolerance

A composite position feature control frame uses multiple segments to control different aspects of a feature pattern. In general, the upper segment locates and orients the pattern relative to the referenced datums, while the lower segment refines the feature-to-feature relationship and any datum relationship stated in that segment.

Composite tolerancing is useful when the entire pattern may have a relatively generous location tolerance but the spacing between holes must remain tight for assembly with a rigid mating pattern.

It is not the same as two unrelated single-segment position callouts. The frame structure, repeated datum references and governing standard affect interpretation. Designers, machinists and CMM programmers should review the requirement together before production.

Position for Slots, Tabs and Non-Cylindrical Features

Position is not limited to round holes and pins. It may control features of size such as slots, tabs and widths when the drawing defines the applicable tolerance zone and feature representation.

Inspection may require:

• Derived median plane of a slot or tab

• Bidirectional position controls

• Separate control of length and width directions

• Profile tolerance when the full boundary is functionally important

• Custom functional gauges for mating features

The CNC slot machining guide covers slot width, depth, end geometry, position, inspection and design-for-manufacturing considerations.

CMM Inspection of Position Tolerance

A coordinate measuring machine is the most common variable method for complex position verification.

1. Review the drawing

Confirm the standard, feature control frame, basic dimensions, datum order, material-condition modifiers, pattern scope and any projected or composite requirement.

2. Qualify the probe

Use a stylus and qualification routine suitable for the hole diameter, depth, surface finish and access. A large stylus may not enter a small bore; a long stylus can increase uncertainty.

3. Establish the datum reference frame

Measure the primary, secondary and tertiary datum features with sufficient coverage. Apply the correct fitting, constraint and material-boundary rules.

4. Measure the controlled feature

Collect enough points or scanning data to represent the feature. Deep, tapered, lobed or interrupted holes may require multiple levels or specialized strategies.

5. Construct the evaluated feature

Create the measured circle, cylinder, axis or median plane according to the approved method and software implementation.

6. Apply size and modifier effects

Use actual feature size and the specified material-condition rules. Keep bonus tolerance and datum shift traceable in the report.

7. Evaluate the feature or pattern

Calculate the position result, then review individual features, pattern behavior and any composite segments separately.

8. Save a reproducible report

Record datum results, actual sizes, position values, allowed tolerance, modifiers, measurement strategy and part orientation.

A CMM output is not automatically correct because it displays a green pass. The program, datum alignment, sampling density, fitting method and standard interpretation must be validated.

Manual and Optical Inspection Methods

Not every position check requires a CMM.

Surface plate and height gauge

On simple prismatic parts, an inspector can establish datums on a surface plate and measure feature centers with a height gauge, indicator, test pin or bore device. The method needs sufficient accuracy and a calculation consistent with the tolerance zone.

Vision measuring system

Optical systems can measure small holes, slots and two-dimensional patterns quickly. Edge detection, lighting, burrs, surface contrast and focus affect the result. A 2D system may not reveal axis tilt through a thick part.

Coordinate measuring arm

A portable arm can inspect large structures and accessible features. Its uncertainty, operator technique and datum setup must be suitable for the specified tolerance.

Pin gauges plus coordinate setup

Gauge pins can establish hole size or provide a measurable center reference. Clearance between the pin and hole, pin straightness and seating depth affect the inferred location.

Functional gauge

A fixed gauge can simulate a worst-case mating boundary and check many features quickly. It often provides an attribute pass or fail result rather than an actual numerical position value.

Functional Gauging at MMC

Functional gauges are especially effective for repetitive clearance-hole or pin patterns controlled at MMC. Gauge elements represent the applicable virtual conditions, while datum simulators establish the allowed reference frame.

Advantages include:

• Rapid production inspection

• Simultaneous check of feature pattern assembly

• Direct relationship to worst-case fit

• Reduced calculation by the operator

• Clear attribute acceptance

Limitations include:

• Gauge design and manufacturing cost

• Need for calibration and wear control

• Limited information about actual error or process direction

• Possible inability to isolate which feature caused failure

• Complexity when datum shift, projection or multiple levels are involved

A functional gauge should be designed from the complete drawing, not only the position value. Its datum simulators, pin sizes, tolerances and sequence of engagement must follow the governing requirements.

Dowel Holes vs Clearance Holes

Dowel holes and bolt-clearance holes often need different position strategies.

Dowel holes locate components precisely and may have tight size, position, perpendicularity and depth requirements. Two dowel holes can overconstrain an assembly if fit and location are not coordinated. A round-and-diamond pin arrangement or one round hole plus one relieved locating feature may be used to manage tolerance buildup.

Clearance holes usually allow more positional variation because the fastener shank does not locate the part as precisely. MMC position can convert available clearance into functional tolerance.

The CNC dowel pin holes guide explains fits, reaming, edge distance, hole spacing and assembly strategies.

Position Tolerance and Threaded Holes

The functional axis of a threaded hole is not always represented adequately by probing only the countersink or tap-drill opening. Thread form, pitch diameter, axis angle and engagement length influence the assembly.

Possible inspection approaches include:

• Threaded functional gauge pins

• Threaded mandrels measured on a CMM

• Dedicated projected-zone gauges

• Thread scanning or specialized metrology

• Process control of tap or thread-mill alignment

The gauge should engage consistently without excessive force. Any play between the gauge and thread must be addressed by the approved method. The CNC thread inspection guide explains GO/NO-GO gauges, pitch diameter and usable engagement.

Common Machining Causes of Position Error

Incorrect work offset or datum pickup

Probe calibration errors, edge-finder technique and wrong offset selection can shift an entire pattern.

Part movement in the fixture

Insufficient clamping, chips under the part or unstable contact points can change the datum relationship during machining.

Tool deflection

Long drills, end mills and boring tools can wander. The problem increases with deep holes, angled entry surfaces and hard or layered materials.

Drill walking

A drill may follow surface irregularity or deflect on a curved face. Spotting, pilot operations or milling the entry can improve location.

Multiple setups

Features machined in separate operations can accumulate alignment error. A common datum strategy and in-process probing help maintain relationships.

Thermal drift

Machine, tool and part temperature can shift positions over a long cycle or large work envelope.

Tool wear and chip packing

Wear changes cutting forces, while packed chips can push a tool off line or damage the bore.

Post-machining distortion

Heat treatment, stress relief, unclamping and surface finishing can move thin or unbalanced parts after the holes were initially correct.

Designing Parts for Reliable Position Control

Choose functional datums

Reference the faces, pilots, bores or locating features that constrain the part in assembly. Avoid selecting a convenient but functionally unrelated edge.

Use a complete datum scheme

Provide enough datums to stabilize the required degrees of freedom without unnecessary overconstraint.

Define basic dimensions clearly

Every controlled feature must have an unambiguous theoretically exact location and orientation.

Match modifiers to function

Use MMC when assembly clearance supports bonus tolerance and functional gauging. Use RFS when location must remain constant independent of size. Use LMC when protecting remaining material is the key requirement.

Consider hole depth and projection

Long engagement and remote mating parts may require axis control through thickness or a projected tolerance zone.

Avoid unnecessary tight tolerances

Tight position values can require reaming, boring, interpolation, probing, more stable fixtures and detailed CMM inspection. Set the tolerance from functional stack-up rather than habit.

Coordinate size and position

Hole-size limits determine clearance and available bonus tolerance. Size and position should be selected as one functional system.

Provide inspection access

Allow room for probes, gauge pins, fixture locators and functional gauges. Deep counterbores and obstructed holes may limit measurement choices.

The CNC machining tolerances guide explains how tolerance choices affect process, inspection, cost and quotation.

Example Position Inspection Plan

Inspection frequency should reflect part risk, process capability, quantity and customer requirements. The CNC inspection sampling plan guide explains sample size, defect classification, AQL and 100% inspection decisions.

What a Position Inspection Report Should Include

A useful report may contain:

• Part number and drawing revision

• Drawing standard and edition

• Characteristic or balloon number

• Feature size limits and actual measured size

• Position tolerance value and modifier

• Actual position result

• Bonus tolerance, when applicable

• Datum feature references and modifiers

• Applied datum shift, if reported separately

• Basic feature location

• Upper and lower composite-segment results

• Projected-zone evaluation when required

• Measurement method and program revision

• Instrument, fixture or gauge identification

• Calibration status

• Sample quantity or serial number

• Inspection condition before or after finish

• Inspector and date

• Nonconformance and disposition reference

For new or changed processes, include the requirement in the CNC first article inspection report and ensure the ballooned drawing matches the report characteristic.

ASME Y14.45-2021 provides uniform practices for reporting attribute or variable measurement data associated with ASME Y14.5 requirements.

Common True Position Inspection Mistakes

Reporting X and Y only

Coordinate deviations help diagnose the process but may not directly state compliance with a diametrical position tolerance.

Using the wrong datum order

Changing primary, secondary and tertiary precedence changes the alignment and can change the result.

Ignoring feature size

MMC or LMC controls require the actual feature size to determine available tolerance.

Combining bonus tolerance and datum shift

They are separate effects from different features. Reports should make their use traceable.

Measuring only the hole entrance

This can miss axis tilt, taper or exit-location error.

Allowing best-fit alignment when the drawing fixes the datums

An unconstrained best fit may reduce reported error while failing to represent the functional assembly reference.

Under-sampling a CMM feature

Too few points can produce an unstable axis or miss lobing and local form error.

Treating a functional gauge as an actual-value measurement

A gauge pass proves its designed boundary condition; it does not necessarily provide the numerical position of each feature.

Misreading composite position

The lower segment is not simply an extra independent tolerance. Its relationship to the pattern and repeated datums must be interpreted correctly.

Applying the wrong standard defaults

ASME and ISO terminology, notation and default rules are not identical. Always identify the governing standard and edition.

RFQ Checklist for Position-Toleranced CNC Parts

Include the following with a request for quotation:

1. Controlled 3D CAD model and 2D drawing

2. Part number and revision

3. Drawing standard and edition

4. Basic dimensions for every controlled feature

5. Complete position feature control frames

6. Datum feature symbols, sequence and modifiers

7. Feature-size limits and fits

8. MMC, LMC or RFS requirements

9. Pattern, composite and projected-zone details

10. Material and heat-treatment condition

11. Surface treatment and final inspection stage

12. Required CMM, vision, manual or functional-gauge method

13. Measurement uncertainty or decision rule if required

14. Sampling or 100% inspection scope

15. First article, capability and final report requirements

16. Production quantity, delivery and traceability needs

The broader CNC machining RFQ checklist helps organize CAD files, materials, finishes, tolerances, documentation and delivery information.

CNC Position Inspection RFQ Template

Please quote CNC machining for part [part number], revision [revision], quantity [quantity]. The drawing follows [ASME Y14.5-2018 / ISO 1101:2017 / other standard]. Features [IDs] require position of [tolerance and units] at [RFS/MMC/LMC] relative to datum reference frame [A|B|C with applicable modifiers]. Evaluate [single feature/pattern/composite/projected zone] in the [before/after finish] condition using [CMM/functional gauge/approved method]. Report actual feature size, position result, allowed tolerance, any bonus tolerance and datum-shift treatment. Include [FAI/capability/final inspection] documentation and notify us before changing the inspection method or proposing a deviation.

Clear requirements allow the supplier to plan the fixture, machining sequence, probing, inspection time and functional gauge needs before pricing.

Frequently Asked Questions

Is “true position” the correct GD&T term?

The formal geometric characteristic is position. “True position” is commonly used in shops to describe the theoretically exact location established by basic dimensions.

Does position control hole size?

No. Feature size is controlled by its size limits. Position controls the allowable location and, depending on the application, orientation of the feature relative to the datum system.

What is bonus tolerance?

When position is specified at MMC or LMC, departure of the actual feature size from that stated material condition can provide additional geometric tolerance according to the applicable rules.

Is bonus tolerance the same as datum shift?

No. Bonus tolerance comes from the controlled feature's size departure. Datum shift comes from permissible movement associated with a datum feature of size and its referenced material boundary.

Can position be checked with calipers?

Calipers alone are rarely sufficient for a precise datum-related position requirement. Simple layouts may use height gauges, gauge pins and surface plates, while complex parts generally require a CMM, vision system or functional gauge.

Why does the CMM result change with a different alignment?

The datum reference frame defines the coordinate system. Changing datum features, order, fitting, constraints or material-boundary treatment changes the alignment and therefore the position result.

Can a functional gauge replace a CMM?

For suitable MMC applications, a functional gauge can efficiently verify the required worst-case boundary and pattern assembly. It normally provides pass or fail information rather than detailed actual values, so it may not replace required variable reports.

How many CMM points are needed for a hole?

There is no universal number. It depends on diameter, depth, form, surface finish, tolerance and required uncertainty. Deep or imperfect holes may require multiple circles or scanning.

Does a larger hole always get bonus tolerance?

Only when the position requirement includes the applicable material-condition modifier and all governing rules are satisfied. A position tolerance at RFS does not automatically gain bonus tolerance from a larger hole.

What is the difference between position and runout?

Position commonly controls the location of a feature axis or median plane relative to datums and basic dimensions. Runout controls surface variation during rotation about a datum axis. See the CNC runout inspection guide for circular and total runout applications.

Request a CNC Machining Quote with Position Inspection

Reliable position control begins with functional datums, clear basic dimensions and a feature control frame that matches assembly needs. Define material-condition modifiers, projected or composite requirements, inspection method and reporting expectations before machining begins.

Send your CAD files, controlled drawing, material, quantity, finish and inspection requirements through the Aluprototype request-a-quote page. The team can review datum strategy, hole-making sequence, CMM access, functional gauging and documentation for custom CNC machined parts.