---
title: "True Position in GD&T: Hole Position Tolerance Explained for Buyers"
description: "Tight hole position tolerances often drive cost and inspection disputes in molded and machined parts. Learn how true position, GDT position tolerance, datum setup, bonus tolerance, and practical verification help buyers judge capability before release."
url: "https://www.hyneu.com/insights/true-position-gdt-hole-tolerance-guide.html"
language: "en"
type: "Article"
category: "Insights"
datePublished: "2026-10-31"
dateModified: "2026-10-31"
brand: "HYNEU"
manufacturer: "HYNEU"
image: "https://static.hyneu.com/uploads/industries/default/T4HDyZrT1ZKs4.webp"
---

# True Position in GD&T: Hole Position Tolerance Explained for Buyers

## Why True Position Is Not a Tighter Center-to-Center Tolerance

Most misunderstandings about true position start with a simple assumption: that it is just a stricter way to control the center-to-center distance between two holes. In production, that assumption creates two expensive errors. A buyer may tighten a position tolerance that does not need to be tight, or an inspector may reject a part that satisfies the drawing because the measurement was reduced to separate X and Y distances.

![How to Calculate True Position for Hole Position in Manufacturing](https://static.hyneu.com/uploads/industries/default/T4HDyZrT1ZKs4.webp)
True position is not a linear distance between centers. It is a GD&T position control that defines a tolerance zone around the exact theoretical location of a feature, measured from a specified datum reference frame. For a round hole, that zone is normally a cylinder. The question is not how far the hole center is from another center in a straight line, but whether the hole center lies inside the allowed cylindrical zone. That distinction matters because it connects inspection to assembly function and to the actual manufacturing process.

On an injection-molded part or a machined hardware component, a hole can be off in X and Y and still assemble perfectly if the offset stays inside the cylindrical zone. Conversely, a hole can pass a simple center-to-center check and still fail the drawing if the datum scheme or the zone shape is ignored. The practical value of true position is not extra strictness. It is a clearer link between design intent, tooling adjustment, inspection, and assembly fit.

## What True Position Actually Controls

True position is the exact theoretical location of a feature. On a controlled drawing, that location is defined by basic dimensions, usually shown in boxes. Basic dimensions carry no tolerance of their own because the position tolerance in the feature control frame supplies the allowed variation. The feature control frame also names the datums that establish the measurement reference.

The term “true position” is often used in two related ways. Strictly, it is the theoretical location. In daily inspection language, it also refers to the calculated deviation of the actual feature from that theoretical location. The drawing callout itself is a position tolerance, and the GD&T position control is the system that defines the zone, datums, and modifiers.

A typical hole callout may state a position tolerance of diameter 0.30 mm at maximum material condition to datums A, B, and C. The basic dimensions locate the hole. The datum reference frame establishes the coordinate system. The position tolerance defines the cylindrical zone. The maximum material condition modifier, when used, allows additional tolerance as the hole departs from its smallest permitted size. All four pieces must be read together. Reading only the number 0.30 mm is a common source of false rejection and supplier disagreement.

### A practical calculation

![True Position in GD&T: Hole Position Tolerance Explained for Buyers](https://static.hyneu.com/uploads/industries/default/EfxQ1dXaRnpwJ.webp)
For a hole controlled in two axes, the inspector records the actual center relative to the true position. If the deviation in X is dx and the deviation in Y is dy, the reported true position diameter is **2 × square root of (dx² + dy²)**. A single-axis offset of 0.10 mm does not produce a true position result of 0.10 mm. It produces a diametrical result of 0.20 mm if the other axis is zero.

This calculation matters during first article inspection and capability review. Two suppliers can report the same X deviation but very different true position results because one has a Y offset and the other does not. The buyer should see the measured coordinates, the calculated diametrical result, and the tolerance basis. A bare pass or fail statement is not enough to judge process capability.

## Coordinate Tolerance vs GD&T Position

Coordinate tolerances and true position do not describe the same tolerance zone. A plus/minus coordinate callout creates a rectangular or square zone. A position tolerance for a round hole usually creates a cylindrical zone. The difference is not academic; it changes acceptance, inspection effort, and sometimes tooling cost.

| Aspect | Coordinate tolerance (±) | True position / GD&T position |
| --- | --- | --- |
| Tolerance zone shape | Rectangular or square in X and Y | Usually cylindrical around the true center |
| Relationship to function | Depends on how the two axes are interpreted | Tied to datums and assembly requirements |
| Effect of hole size | Normally fixed unless another control applies | May include maximum or least material condition bonus |
| Inspection result | Separate X and Y deviations | Single diametrical deviation compared with the position tolerance |
| Common risk | A part may be rejected in one axis even though the hole still assembles | A misread datum scheme or ignored bonus tolerance can cause false rejection |

A common misconception is that true position always costs more because it sounds more precise. In fact, a position tolerance with a maximum material condition modifier can be more forgiving than a tight plus/minus callout for a hole that only needs clearance for a fastener. The extra forgiveness is controlled by the actual hole size and the virtual condition boundary. The opposite is also possible: a poorly chosen datum scheme can make a reasonable tolerance difficult to verify and expensive to guarantee.

## How to Verify Hole Position Step by Step

- **Confirm the feature control frame and basic dimensions.** Check the position tolerance, the datum order, and any maximum or least material condition modifier. Do not derive the true position from undimensioned geometry or from another hole unless the drawing says so.
- **Lock the datum reference frame.** The primary, secondary, and tertiary datums must be established in the stated order. For plastic parts, agree whether measurement is in free state or restrained condition. A fixture that clamps a flexible part flat can change the result.
- **Measure the actual hole size and center coordinates.** The method may be a coordinate measuring machine, optical system, functional gauge, or another agreed method. The key is that the method can establish the hole center relative to the same datums used by the drawing.
- **Convert the center offset to diametrical true position.** Record dx and dy, calculate the diametrical result, and keep the raw coordinates. This allows a second reviewer to check the result and helps distinguish a real process shift from a calculation error.
- **Apply bonus tolerance only when specified.** If the drawing uses maximum material condition for a hole, the allowed position tolerance increases as the actual hole becomes larger than its smallest permitted size. For example, a hole called out at 10.00 to 10.20 mm with a 0.30 mm position tolerance has a 0.15 mm bonus when produced at 10.15 mm, giving a total allowed position tolerance of 0.45 mm. An inspector who compares the measured result only with 0.30 mm will reject a conforming part.
- **Compare the result with the tolerance and measurement uncertainty.** A result close to the limit deserves a second check. Probe access, datum contact, surface finish, and part temperature can all affect the measured value. Guard banding may be appropriate for critical assemblies or high-cavity molds.
- **Review the trend, not only the first part.** A single good hole does not prove a stable process. Check multiple cavities, production lots, and time-based drift. In injection molding, hole position can move with material lot, moisture, mold temperature, hold pressure, and cooling time. In metal hardware, punch wear, drill walk, and fixture wear can cause gradual drift.

## Where True Position Matters Most in Plastic and Hardware Manufacturing

### Injection-molded components

In plastic parts, hole position is affected by shrinkage, warpage, gate location, cooling balance, and insert movement. A mold can produce a hole at the correct pin location and still produce a part whose hole center falls outside the true position zone after shrinkage and ejection. Differential shrinkage across a long part is especially important. If the drawing datums are on one side of the part and the holes are on another, the measurement may reveal a warp pattern rather than a simple hole location error.

A practical risk is measuring a flexible molded part on a flat fixture without agreeing on the restraint condition. The part may pass on the fixture and fail in free state, or the reverse. For projects where hole position supports assembly, the drawing, the fixture, and the quality plan should state the condition clearly. This is a drawing review issue as much as an inspection issue.

### Hardware and tool accessories

For stamped, drilled, or machined hardware parts, true position often controls mounting holes, pin holes, and assembly interfaces. Punch wear can shift a stamped hole over a production run. Drill walk can affect deep holes. Plating and coating can change hole size and, in some cases, influence measurement if the coating is thick or uneven. The supplier should know whether the stated position tolerance applies before or after surface finishing.

### Assembly interfaces

True position is most useful where a hole must line up with a pin, screw, connector, or mating bracket. In these cases, the tolerance should reflect assembly clearance and the datum scheme should reflect how the part is located in the assembly. A position tolerance copied from a template without checking the functional datum can create a drawing that is easy to inspect but hard to assemble, or the reverse.

## Supplier Evaluation and Drawing Review

- **Can the supplier read the datum scheme?** Ask for the first article inspection plan and confirm that datums A, B, and C are established in the correct order. A supplier who measures from a convenient surface rather than the drawing datum may produce a good part and a bad report.
- **Is the inspection method suitable for the tolerance?** A functional gauge may be efficient for high-volume hole location checks, but it may not give coordinate data for capability analysis. A coordinate measuring machine may provide data but may struggle with small holes or flexible plastic parts. The method should match the feature and the decision.
- **Is bonus tolerance handled correctly?** Review a sample inspection report that includes a maximum material condition callout. Confirm that the supplier records actual hole size and applies the bonus only when the drawing allows it. This is a frequent source of false rejection in threaded or clearance holes.
- **Is process capability available?** For repeat production, ask for position capability data by cavity or production cell. A supplier may pass a first article and still drift during mass production. Capability data should be linked to the same datum scheme and measurement method used for acceptance.
- **Is change control clear?** Mold repairs, insert changes, punch replacement, material lot changes, and fixture modifications can all move hole position. The supplier should define when a new first article or layout inspection is required after a change.

For HYNEU, as a Zhejiang-based injection molding and hardware manufacturer serving OEM and ODM projects, the useful supplier question is not whether a position tolerance can be quoted. It is whether the drawing, process, fixture, and inspection report agree on the same datum reference frame and the same acceptance rule. That agreement prevents disputes more effectively than a tighter nominal tolerance.

## Practical Judgment Criteria Before Release

Do not release a project on the basis of a position tolerance number alone. Use three filters: functional fit, process capability, and inspection feasibility. Functional fit tells you whether the hole position tolerance reflects the assembly clearance. Process capability tells you whether the selected molding or metal process can hold it across cavities and production lots. Inspection feasibility tells you whether the supplier can measure the result repeatably with the stated datums and modifiers.

If a drawing uses true position only because it appears in a customer template, challenge whether the control reflects the real assembly requirement. If a tolerance is tight but the datum scheme is weak, the inspection result may be uncertain and the supplier may add cost without improving fit. If the drawing includes maximum material condition, confirm that the inspector understands bonus tolerance and records the actual feature size. If the part is flexible plastic, confirm whether position is verified in free state or restrained condition.

A well-controlled true position requirement is a decision tool. It helps the buyer compare suppliers, helps the engineer connect design intent to manufacturing, and helps the quality team separate real nonconformance from measurement noise. A poorly controlled requirement does the opposite: it creates false rejections, unnecessary tooling changes, and slow project ramp-up. The difference is usually not the tolerance value itself, but whether the datum scheme, feature size, modifier, measurement method, and process capability are all read together before production release.

## Related Resources

- [Insights](https://www.hyneu.com/insights/)
- [Capabilities](https://www.hyneu.com/capabilities/)
- [Custom Manufacturing](https://www.hyneu.com/custom-manufacturing/)
- [Products](https://www.hyneu.com/products/)
- [Buying Guides](https://www.hyneu.com/buying-guides/)
- [Industries](https://www.hyneu.com/industries/)
- [Manufacturing Knowledge](https://www.hyneu.com/knowledge/)
- [Manufacturing Q&A](https://www.hyneu.com/questions/questions/)

## Structured Data

```json
[
  {
    "@context": "https://schema.org",
    "@type": "BreadcrumbList",
    "itemListElement": [
        {"@type": "ListItem", "position": 1, "name": "Home", "item": "https://www.hyneu.com/"},{"@type": "ListItem", "position": 2, "name": "Insights", "item": "https://www.hyneu.com/insights/"}
        ,{"@type": "ListItem", "position": 3, "name": "True Position in GDT: Hole Position Tolerance Explained for Buyers"}
    ]
  },
  {
    "@context": "https://schema.org",
    "@type": "Article",
  	
  	"url": "https://www.hyneu.com/insights/true-position-gdt-hole-tolerance-guide.html",
      "headline": "True Position in GDT: Hole Position Tolerance Explained for Buyers",
      "keywords": "true position,position tolerance,GDT position,hole position",
      "articleSection": "Insights",
      "image": [
  		        "https://static.hyneu.com/uploads/industries/default/T4HDyZrT1ZKs4.webp"
  		],"description": "Tight hole position tolerances often drive cost and inspection disputes in molded and machined parts. Learn how true position, GDT position tolerance, datum setup, bonus tolerance, and practical verification help buyers judge capability before release.",
      "datePublished": "2026-10-31T08:27:43Z",
      "dateModified": "2026-10-31T08:27:43Z"
  	
      ,"isPartOf": {
        "@type": "WebPage",
        "url": "https://www.hyneu.com/insights/",
        "name": "Insights"
      },
      "inLanguage":"en",
      "publisher":{ "@id":"https://www.hyneu.com/#organization" }
  }
]
```