How to Specify Position Tolerance for Hole Patterns in CNC Machining

Position tolerance (symbol: ⌖), often called true position, is one of the most powerful GD&T controls for ensuring that hole patterns locate correctly in an assembly. However, incorrect specification is a frequent cause of rejected parts, additional inspection costs, and unnecessary machining complexity. This guide explains how to specify position tolerance for hole patterns on CNC machined parts, focusing on practical engineering decisions that affect manufacturability, inspection, and cost.

Quick Answer

Position tolerance for a hole pattern is specified by placing a feature control frame below the hole size dimension, referencing one or more datums, and stating the tolerance zone diameter (e.g., ∅0.2 M). For a pattern of holes, you typically need to decide between a single‑segment position tolerance (controlling location relative to datums) and a composite position tolerance (controlling pattern location and hole‑to‑hole spacing separately). Always define datums that are accessible and repeatable during inspection. Use material condition modifiers (MMC or LMC) when function allows, as they can reduce scrap and inspection cost.

Key Takeaways

• Position tolerance controls the center of a hole to a cylindrical tolerance zone; the diameter value is the total allowable deviation.
• Always specify datums in a logical order (primary, secondary, tertiary) based on how the part is located in the assembly.
• For multiple holes, use composite position tolerance if you need tight hole‑to‑hole spacing but looser location relative to the part edges.
• Apply MMC (Maximum Material Condition) modifier to the tolerance and/or datum references to allow bonus tolerance and ease inspection with functional gages.
• Inspect position tolerance with a CMM or hard gage; ensure the inspection method matches the datum referencing scheme.
• Common mistakes: missing datums, improper datum order, over‑constraining the part, and using position tolerance unnecessarily when simpler tolerances suffice.

What Is Position Tolerance?

Position tolerance defines a cylindrical (or sometimes square) tolerance zone within which the center axis of a feature (e.g., a hole) must lie. Unlike coordinate tolerancing (±X, ±Y), which creates a square tolerance zone, position tolerance provides a uniform cylindrical zone that better matches functional requirements such as bolt clearance. The tolerance is specified as a diameter value, e.g., ∅0.1, meaning the actual axis must fall within a cylinder of that diameter centered at the true position.

Why Use Position Tolerance Instead of ± Tolerances?

Coordinate tolerances (e.g., 10±0.1) define a square tolerance zone of 0.2 × 0.2. The diagonal corners of that square are 0.283 from true center, which is 41% larger than the stated 0.1 tolerance. Position tolerance eliminates this ambiguity and creates a uniform acceptance zone. It also allows material condition modifiers that can reduce cost by accepting slightly mislocated holes when the part is at its worst‑case condition.

Basic Elements of a Position Tolerance Callout

A typical position tolerance feature control frame on a drawing looks like this:

⌖ ∅0.2 M | A | B | C

• ⌖ – Position symbol
• ∅0.2 M – Diameter of tolerance zone, with MMC modifier (M)
• A – Primary datum (usually a plane)
• B – Secondary datum (often a width or edge)
• C – Tertiary datum (a hole or another planar surface)

The order of datums is critical: the primary datum constrains three degrees of freedom (two rotations and one translation), the secondary constrains two, and the tertiary constrains one.

Datums for Hole Patterns

Selecting correct datums is the most common source of confusion and error. For a part with a hole pattern that must locate relative to other features, follow these guidelines:

• Choose datums that correspond to mounting surfaces or mating features in the final assembly.
• Primary datum should be a plane that contacts the mating part (often the surface that holds the part flat).
• Secondary datum should be a feature that aligns the part in one direction (e.g., a side edge or a slot).
• Tertiary datum should be a feature that provides final rotational alignment (e.g., a dowel pin hole or another edge).
• Avoid using datum features that are themselves produced by the same setup as the holes unless they are independent (e.g., machined in the same setup but used as reference).

Example: Bracket with Four Mounting Holes

In the example above, the bottom surface is the primary datum (plane A), the left edge is datum B, and the rear edge is datum C. All four holes are controlled with a single position tolerance referencing A|B|C. This ensures the hole pattern is correctly located relative to the edges that will mate with the assembly.

Single‑Segment vs. Composite Position Tolerance

When you have multiple holes in a pattern, you must decide how tightly their positions are controlled relative to the datums and relative to each other.

Single‑Segment Position Tolerance

One line in the feature control frame: ⌖ ∅0.5 M | A | B | C. This controls the entire pattern location and the spacing between holes with the same tolerance. Inspector will check each hole’s position relative to the datum system. If the requirement is that the pattern as a whole can shift but the holes must remain precisely spaced, single‑segment may over‑constrain and drive cost.

Composite Position Tolerance

Two lines in the feature control frame. The top line controls the pattern location relative to datums (larger tolerance). The bottom line controls the spacing between holes within the pattern (smaller tolerance) and references only a datum(s) that restrict degrees of freedom relevant to the pattern.

⌖ ∅0.8 M | A | B | C
   ⌖ ∅0.2 M | A

Here, the top line allows the pattern to shift up to ∅0.8 from true position, while the bottom line ensures any two holes are within ∅0.2 of their basic relative positions. Composite tolerance is very common for PCB mounting holes, flanges, and multi‑bolt patterns where alignment to the mating part is less critical than the fit of the bolts through the holes.

Material Condition Modifiers: MMC, LMC, RFS

Applying MMC (Maximum Material Condition) allows bonus tolerance — as the hole size deviates from MMC (smallest hole), the allowable position tolerance increases. This is extremely beneficial because it reduces scrap and allows functional gaging (e.g., a go/no‑go pin gage). Use the MMC modifier (M) after the tolerance value and optionally after datum references.

LMC (Least Material Condition) is less common but used when wall thickness is critical. RFS (Regardless of Feature Size) is default; no modifier means no bonus tolerance. In practice, use MMC for clearance holes whenever possible.

Inspection of Position Tolerance

Inspection depends on the chosen modifiers and the availability of equipment.

• Coordinate Measuring Machine (CMM): Most flexible; can evaluate position with or without MMC. Requires a full definition of datums and alignment routine.
• Functional Gage (Hard Gage): A go gage with pins sized at the worst‑case MMC condition. Extremely fast and repeatable but requires dedicated gage per part. Only works with MMC specification.
• Pin Measurements: For small quantities, inspectors may use a height gage or indicator on a surface plate, but this is prone to error.

When requesting a CNC machining quote for parts with position tolerances, provide the full GD&T definition (drawing with datum targets, basic dimensions, and feature control frames). Without this, the supplier cannot correctly plan the machining sequence and inspection method, leading to miscommunication and possible rejection.

Common Mistakes When Specifying Position Tolerance

• Missing datums: Not specifying any datums, or only referencing one datum when the part has a planar base. A hole pattern without a datum system is ambiguous — the inspector must guess which surface to use.
• Wrong datum order: Placing a narrow surface as primary and a large plane as secondary. The primary datum should be the most functionally important and provide the largest contact area.
• Over‑constraining with too many datums: Using three datums when two or even one suffice for the pattern. This makes the tolerance unnecessarily tight and increases inspection variability.
• Using zero tolerance at MMC incorrectly: ∅0 M | A|B|C means holes must be perfectly centered if at MMC; any size deviation allows bonus. While valid, this can be difficult to interpret and inspect without functional gages.
• Not specifying basic dimensions: Position tolerance must be accompanied by basic dimensions (enclosed in a box) that define the true position. Without basic dims, the tolerance has no target.
• Applying position tolerance to a single hole without datums: A single hole can still need datums; otherwise, its location is unconstrained.

How Position Tolerance Affects CNC Machining Cost

Tighter position tolerances (e.g., ∅0.05 vs. ∅0.5) require more setup stability, better tooling, and often additional inspection time. If the tolerance is specified at MMC, the supplier may use a functional gage and avoid CMM inspection, lowering costs. Composite tolerances can also reduce cost by allowing a larger pattern shift tolerance. When designing, analyze the assembly function: does the pattern need to align to the part edges, or just to itself? Choosing composite tolerance can save significant machining and inspection cost.

What This Means for Your Part

Before releasing your drawing, review the following:

• Have you defined a clear datum system that mimics how the part mounts? If you cannot physically measure from those datums, the supplier will struggle.
• Are basic dimensions clearly indicated for each hole’s true position? They should be dimensioned from the datums.
• Can you use MMC? For clearance holes, the answer is almost always yes. This can eliminate the need for CMM inspection and reduce the risk of scrap.
• Is the tolerance value realistic for your machining process? Discuss with your CNC machining supplier early. Position tolerances of ∅0.1 are routinely achievable in 3‑axis machining; ∅0.025 is possible but requires extra care and may increase cost.
• Consider composite position tolerance if the pattern spacing is critical but pattern shift can be relaxed.

When sending your RFQ to a CNC machining manufacturer, include the 2D drawing with full GD&T callouts and a 3D model. Confirm that the supplier has experience with position tolerance inspection (CMM or gage). Properly specified position tolerance reduces lead time, improves part quality, and prevents costly misunderstandings.

References & Further Reading

• ASME Y14.5-2018 – Dimensioning and Tolerancing
• Related Technical Guides: CNC Machining Tolerances, Preparing a 2D Drawing