True Position Tolerance: Calculation, MMC Bonus & Worked Examples
True position is the most common GD&T location control per ASME Y14.5-2018. This guide covers the formula, a worked example on a 4-hole bolt pattern in 6061-T6 aluminum, MMC bonus tolerance, functional gaging, and how position tolerance affects CNC machining cost.
Quick Answer
True position is the GD&T location control that defines how far a feature’s actual center can deviate from its nominal (basic) location. Calculate it as P = 2√(dx² + dy²), where dx and dy are the measured deviations in X and Y from the basic dimensions. The result is a diameter. When specified at MMC, the tolerance grows as the feature departs from its maximum material size—a bonus that reflects assembly reality and reduces rejection rates.
What Is True Position?
True position (also called “position” or “GD&T position tolerance”) is the most frequently used location control in ASME Y14.5-2018. It defines the allowable deviation of a feature’s center point, axis, or center plane from its theoretically exact (basic) location, as established by datum references.
Unlike ± dimensions that create a square tolerance zone, true position uses a cylindrical tolerance zone for holes and pins (or a rectangular zone when explicitly noted). The zone is centered on the basic location, and the feature axis must fall entirely within it. This cylindrical zone is functionally significant: round holes mate with round pins, so the allowable deviation is naturally radial—not independent in X and Y.
Position always references datums (the feature control frame includes datum letters A, B, C) to establish the measurement coordinate system. For a deeper overview of datums and all 14 GD&T symbols, see the GD&T guide.
The True Position Formula
The position deviation for a feature in a 2D plane (the typical case for through-holes) is calculated as:
Position deviation (diameter of the zone containing the measured axis)
Deviation from the basic X coordinate: actual X − nominal X
Deviation from the basic Y coordinate: actual Y − nominal Y
Why the ×2?
The √(dx² + dy²) term gives the radial distance from the nominal center to the actual center. Per ASME Y14.5-2018, position tolerance is expressed as a diameter, not a radius. Multiplying by 2 converts the radial deviation to the diametral value that appears in the feature control frame.
3D Extension
For features with position controlled in three dimensions (e.g., a blind hole with depth location), the formula extends to P = 2√(dx² + dy² + dz²), where dz is the Z-axis deviation. The tolerance zone becomes a sphere instead of a cylinder.
Cylindrical Zone vs Square Zone: 57% More Area
The single largest cost advantage of true position over ± tolerancing is the tolerance zone shape. With ±0.005 in. (0.13 mm) in X and ±0.005 in. in Y, you create a 0.010 × 0.010 in. square zone. True position uses a cylindrical (circular) zone. The circle that circumscribes the same square has a diameter of 0.010 × √2 ≈ ø0.014 in. (0.36 mm)—and that circle contains 57% more area than the square.
| Property | ± Square Zone | Position Cylindrical Zone |
|---|---|---|
| Zone shape | Rectangle (0.010 × 0.010 in.) | Cylinder (⌀0.014 in.) |
| Zone area | 0.000100 sq in. (0.0645 mm²) | 0.000154 sq in. (0.0993 mm²) |
| Area advantage | Baseline | +57% |
| Max deviation on-axis | 0.005 in. (0.13 mm) | 0.007 in. (0.18 mm) |
| Max deviation at 45° | 0.007 in. (0.18 mm) — same as circle | 0.007 in. (0.18 mm) |
| Datum reference | No (implied from dim chain) | Yes (explicit A|B|C) |
| Functional relevance | Rectangular — poor match for round features | Circular — matches hole/pin geometry |
What this means in practice
Converting from ± to true position does not loosen the tolerance—it uses a zone shape that matches the function. A round hole mates with a round pin; the relevant deviation is radial distance from center, not independent X/Y limits. The 57% area gain means more parts pass inspection for the same functional requirement. On a typical production run in 6061-T6 aluminum, this can reduce scrap rate by 3–8% for hole-pattern features compared to equivalent ± callouts.
Worked Example: 4-Hole Bolt Pattern
A CNC-machined mounting bracket in 6061-T6 aluminum has four clearance holes for ¼-20 fasteners. Each hole is specified as:
Feature Control Frame
⌖ | ø 0.010 Ⓜ | A | B | C
Measure actual hole center
Use CMM or optical comparator to record the X and Y coordinates of each hole’s center, relative to the datum reference frame (A|B|C).
Calculate deviations
For each hole: dx = actual X − nominal X, dy = actual Y − nominal Y. Sign doesn’t matter because we square both terms.
Apply the formula
P = 2 × √(dx² + dy²). This gives the diameter of the smallest cylinder centered on the basic location that contains the actual hole axis.
Calculate allowed tolerance
Allowed = stated position (0.010) + bonus. Bonus = actual hole diameter − MMC (0.266). If the hole is at MMC, bonus = 0 and the allowed tolerance equals the stated value.
Inspection Results
| Hole | Actual ø (in.) | dx (in.) | dy (in.) | P (in.) | Bonus (in.) | Allowed (in.) | Result |
|---|---|---|---|---|---|---|---|
| 1 | 0.268 | +0.003 | −0.002 | 0.0072 | 0.002 | 0.012 | PASS |
| 2 | 0.267 | +0.004 | +0.001 | 0.0082 | 0.001 | 0.011 | PASS |
| 3 | 0.270 | −0.002 | +0.003 | 0.0072 | 0.004 | 0.014 | PASS |
| 4 | 0.270 | −0.003 | +0.004 | 0.0100 | 0.004 | 0.014 | PASS |
Hole 4 — the MMC advantage
Hole 4 has a position deviation of exactly ø0.010 in.—equal to the stated tolerance. At RFS (no bonus), this hole would be borderline. But the actual diameter is ø0.270 in. (LMC), yielding a bonus of 0.004 in. The allowed tolerance grows to ø0.014 in., and the hole passes comfortably. This is why specifying position at MMC accepts more parts without sacrificing assembly function.
CNC Parts to GD&T Position Specs — Free DFM Review
MakerStage machines hole patterns to ASME Y14.5 position tolerances as tight as ø0.002 in. (0.05 mm) with CMM verification. Upload your drawing with GD&T callouts and get a quote with engineer-reviewed DFM feedback—we will flag any position callouts that drive unnecessary cost and suggest tolerance-for-cost trade-offs before you commit.
Get a Quote with Free DFM ReviewMMC Bonus Tolerance — How It Works
When a position callout includes the MMC modifier (“circled M” in the feature control frame), the stated tolerance applies only when the feature is at its Maximum Material Condition. As the feature departs from MMC—a hole gets larger, or a pin gets smaller—the position tolerance increases by the same amount. This increase is called bonus tolerance.
The physical logic is straightforward: a larger hole can accept more position error and still assemble with the mating fastener. ASME Y14.5-2018 captures this reality with a simple rule:
Bonus Tolerance Table for the Worked Example
| Actual Hole ø (in.) | Bonus (in.) | Allowed Position (in.) | Allowed Position (mm) |
|---|---|---|---|
| 0.266 (MMC) | +0.000 | ø0.010 | ø0.25 |
| 0.267 | +0.001 | ø0.011 | ø0.28 |
| 0.268 | +0.002 | ø0.012 | ø0.30 |
| 0.269 | +0.003 | ø0.013 | ø0.33 |
| 0.270 (LMC) | +0.004 | ø0.014 | ø0.36 |
When to specify MMC
Use MMC when assembly clearance is the primary concern: bolt patterns, dowel-pin fits, connector pin arrays. MMC enables functional gaging and accepts more parts. Typical use: clearance holes for fasteners where the hole must clear the bolt regardless of where the hole center lands within the position zone.
When to use RFS (no modifier)
Use RFS when position accuracy is required independent of feature size: fluid port alignment, optical bore centerlines, or datum-qualifying features where the tolerance must hold at any produced diameter. RFS is the default per ASME Y14.5-2018 when no modifier appears in the FCF.
Functional Gaging for True Position at MMC
When true position is specified at MMC, the tolerance defines a fixed boundary called the virtual condition (VC). For internal features (holes), the virtual condition is:
What the gage looks like
A hardened steel plate with 4× ⌀0.256 in. (6.50 mm) pins press-fit at the exact nominal hole positions. The pin diameter equals the virtual condition. Pin locations are held to a gage-maker tolerance of typically ±0.0001 in. (0.003 mm), which is 10× tighter than the part tolerance.
How to use it
Set the part against the primary datum (flat plate for A), secondary and tertiary locators (for B and C). Drop the gage onto the part. If all 4 pins enter all 4 holes simultaneously, every hole passes position at MMC. One pass, one decision — no coordinate data, no operator interpretation.
Why it works
The VC boundary is the smallest cylinder that a ⌀0.256 pin can pass through. If a hole at MMC (⌀0.266) is perfectly centered, the clearance is (0.266−0.256)/2 = 0.005 in. per side — exactly the radial position tolerance. As the hole gets larger, more clearance is available, matching the MMC bonus concept exactly.
When functional gaging saves money
Functional gaging is typically 5–10× faster than CMM per part. For production quantities above 50–100 parts, the gage cost ($500–2,000 for a simple plate gage) is recouped in reduced inspection time. Below 50 parts, CMM first-article + sampling is typically more cost-effective.
CNC Cost Impact of Position Tolerance
The position tolerance you specify directly affects fixturing complexity, machining strategy, and inspection method. The table below shows typical cost impact for CNC-machined holes in aluminum and steel alloys, based on current US job shop rates.
| Position Tolerance | Inspection Method | Cost Impact | Typical Application |
|---|---|---|---|
| ⌀0.002–0.005 in. (0.05–0.13 mm) | CMM, 100% inspection | +50–100% | Precision bearing fits, optical alignment bores |
| ⌀0.005–0.010 in. (0.13–0.25 mm) | CMM first article + sampling | +15–40% | Dowel pin locations, mating hole patterns |
| ⌀0.010–0.014 in. (0.25–0.36 mm) | Functional gage (if MMC) or CMM FAI | Baseline | Standard bolt patterns, clearance holes |
| ⌀0.014–0.020 in. (0.36–0.51 mm) | Pin gage or caliper check | −5–15% | Non-critical access holes, wire routing |
Where the money goes
Tight position tolerance increases cost through three channels: (1) slower feed rates and finer tool strategies to hold location, (2) precision fixturing with located pins instead of edge clamps, and (3) CMM time at $75–150/hr for verification. On a typical 4-hole aluminum bracket, moving from ø0.014 to ø0.005 position can add $15–40 per part in combined machining and inspection cost.
Cost reduction strategy
Before tightening position, ask: does this hole need to be within ø0.005, or does the bolt just need to clear? For most clearance-hole patterns, ø0.010–0.014 at MMC is sufficient and keeps parts in the baseline cost tier. Reserve tight position for features where fit or alignment genuinely requires it. For tolerance strategy guidance, see our CNC tolerances guide.
True Position FAQ
How do you calculate true position?
What is the true position formula?
What is MMC bonus tolerance in GD&T?
What is the difference between position at MMC and RFS?
Why is a cylindrical tolerance zone larger than a square zone?
How does true position tolerance affect CNC machining cost?
What is a functional gage for true position?
Related Resources
Need Parts Machined to GD&T Position Specs?
Upload your drawings with GD&T callouts. We machine to ASME Y14.5 with position tolerances as tight as ø0.002 in. (0.05 mm) and provide CMM inspection reports on request. Free DFM review on every order.
Get Free Quote Fast