Position Tolerance: From Confusion to Control

What Position Tolerance Really Is

In GD&T, position tolerance (symbol: ⌖) controls the location of a feature—usually a hole, pin, slot, or boss. It defines a zone where the feature's axis or center plane must lie.

The key is that the tolerance zone is a circle (or cylinder in 3D), not a square. A position tolerance of 0.1mm means the center of the hole must be inside a circle with a diameter of 0.1mm. Not 0.1mm in X and 0.1mm in Y separately. A circle.

Why does that matter? Because the diagonal of a 0.1mm square is about 0.14mm. If you treat position as a square tolerance, you're allowing 40% more error in the diagonal direction. A part that passes a square tolerance might fail a true position tolerance. And vice versa.

Let me give you an example. Suppose you have a hole with a position tolerance of 0.1mm. If the hole center is 0.08mm off in X and 0.08mm off in Y, it's within a ±0.1mm square tolerance (since 0.08 < 0.1). But the distance from the true center is sqrt(0.08² + 0.08²) = 0.113mm. That's outside the 0.1mm diameter circle. The part fails position tolerance even though it would pass a standard ± tolerance.

This is why you can't just treat position like X and Y limits. You have to think about the diagonal.

The Datum Framework

Position tolerance always references datums. Usually three: primary (A), secondary (B), and tertiary (C). These datums create a coordinate system. The basic dimensions (the ones in boxes) tell you where the feature should be in theory. The position tolerance tells you how much it can deviate.

For example: ⌖ ⌀0.1 A B C

• Datum A is usually a flat surface (the primary reference)

• Datum B is usually an edge or hole (secondary)

• Datum C is another edge or hole (tertiary)

When you measure the part, you set it up on these datums. Then you locate the hole's actual center. Then you check if it falls within a 0.1mm diameter circle around the basic location.

If you ignore the datums, you can measure the same hole and get different results. I've seen parts pass inspection in one fixture and fail in another because the fixture used different datums. Always follow the drawing.

MMC and Bonus Tolerance

Once you understand basic position, you'll see a little "M" inside a circle next to the tolerance. That's Maximum Material Condition (MMC). It means you get bonus tolerance if the feature is not at its largest material condition.

For a hole, the largest material condition is the smallest allowable hole diameter (because more material is present). If the hole is drilled larger than the MMC size, you get bonus tolerance. The bonus equals the difference between the actual hole size and the MMC size.

Example: A hole is dimensioned as 10.00 ±0.10. The MMC is 9.90mm (smallest hole). The position tolerance is 0.1mm at MMC. If you drill the hole to 9.95mm, you get 0.05mm bonus tolerance. Your total position tolerance becomes 0.15mm.

Why does this matter? Because a larger hole is easier to position correctly—the mating pin or fastener has more clearance. So the standard gives you a break. It's a smart way to reduce scrap.

If you see the MMC modifier, you can relax a little on position if the hole size is favorable. But don't rely on it too much. I aim to hit the basic tolerance without bonus, then use bonus as a safety margin.

How to Control Position on the Machine

Holding position tolerance is about three things: machine accuracy, workholding, and tooling.

Machine Accuracy

Your machine needs to be able to position accurately. A 0.1mm position tolerance is easy for most modern CNC machines. A 0.02mm tolerance requires a good machine in good condition. A 0.005mm tolerance is grinding or jig boring territory.

Before you run a tight position job, check your machine's positioning accuracy. Run a test: drill a few holes at known coordinates, then measure the actual locations. If the machine is off by 0.02mm, you need to compensate or use a different machine.

Workholding

If the part moves during machining, your position tolerance is gone. Use a rigid setup. For multiple parts, use a fixture that locates the part consistently. Soft jaws cut to the part shape work well.

The biggest mistake I see is using a vise without indicating the part. For position-critical jobs, I indicate the part edges to establish the datum reference frame. I might spend an extra five minutes setting up, but it saves me from scrapping parts.

Tooling

For holes, use a drill with a split point to reduce walking. For better position accuracy, use a center drill first, then a stub drill, then the full-length drill. Or better yet, use a boring operation or interpolation with an end mill for final size.

Drills tend to walk, especially on uneven surfaces or angled entries. If position is tight, I always spot drill first, then drill undersize, then bore or interpolate to final size and position. Boring is the most accurate because the tool is rigid and the spindle determines the position.

For milling features (slots, pockets, bosses), use a finishing pass with a small end mill. Climb milling for better accuracy. And always take a light finish pass—0.1mm or less—to minimize tool deflection.

Inspection: How to Check Position

You need a CMM or a height gauge with a dial indicator, plus a way to establish the datums.

The basic method for a hole:

1. Set up the part on a surface plate using the datum features.

2. Find the center of the hole (use a probe or a dial indicator in a spindle).

3. Measure the X and Y deviation from the basic dimensions.

4. Calculate the true position: 2 * sqrt(ΔX² + ΔY²). (Multiply by 2 because the tolerance is a diameter, not a radius.)

If that value is less than or equal to the position tolerance (including any bonus), the part is good.

For production, I use a CMM. It's faster and less error-prone. But for a quick check on the shop floor, a height gauge and a coaxial indicator work.

Common Mistakes

Treating position as plus/minus. I've seen engineers convert position tolerance to X and Y limits. That's wrong. You're either using the GD&T correctly or you're not. If you want plus/minus, use plus/minus.

Ignoring the datums. The part must be measured in the datum reference frame. If you set it up differently, your measurement is meaningless.

Forgetting MMC bonus. If you have MMC, you can sometimes accept a slightly off-position hole if the hole size is larger. But you have to calculate it. Don't just guess.

Not controlling the process. Position tolerance is not something you check only at the end. You need to control the machine, the workholding, and the tooling. If you only measure the first part and then assume the rest are good, you're going to scrap a batch when something drifts.

A Real Example

I had a job with an aluminum plate, 4 holes, position tolerance of 0.05mm at MMC. The holes were 6.00 ±0.05mm. Datums: A (bottom face), B (left edge), C (back edge).

My approach:

• Used a fixture with a ground base (datum A) and fixed pins for B and C.

• Spot drilled with a 3mm center drill.

• Drilled undersize to 5.8mm with a stub drill.

• Finished with a 6mm end mill interpolating the hole to final size. This gave me perfect position because the interpolation is controlled by the machine's ballscrews, not by drill walking.

The first part measured position within 0.02mm. I ran 200 parts, checking every 20th part. All were within tolerance. No scrap.

What I Tell Customers

When a customer asks for a tight position tolerance, I ask them: "Do you really need it? And do you understand that it's a circle, not a square?"

Most engineers appreciate the explanation. Some loosen the tolerance. Some keep it. Either way, they know I know what I'm doing.

And that trust is worth more than any single job.

The Bottom Line

Position tolerance is a powerful tool, but only if you understand it. It's not plus/minus. It's a circle. It references datums. It can include bonus from MMC.

To hold it, control your machine, your workholding, and your tooling. Use spot drilling, boring, or interpolation for critical holes. And always measure in the correct datum reference frame.

Once you get it, it's not that hard. But until you get it, it will cost you parts.

What's the tightest position tolerance you've ever held? And how did you do it? I'd like to hear your stories.