What Are Tolerances?
Here's the reality of manufacturing: no part is ever made perfectly. Every machine, every tool, every process introduces small variations. A shaft drawn at Ø1.000 in might come off the lathe at 0.9994 or 1.0005.
A tolerance is the amount of variation you're willing to accept on a dimension. It's your way of telling the shop: "I need this to be close to 1.000 in, but here's how much wiggle room you have."
Let's look at how tolerances are written on a drawing.
Reading a Tolerance Callout
The most common format is bilateral tolerance — a nominal size with equal variation in both directions:
This means the actual part can be anywhere from 0.998 to 1.002 in. Both are acceptable. Anything outside that range gets scrapped or reworked.
The tolerance band is the total range: 1.002 − 0.998 = 0.004 in.
Your Turn — Calculate Min & Max
A drawing calls out this pin diameter:
Two Parts, Two Drawings
Now we have a real assembly problem. You've got two parts, each from a different drawing:
Drawing A — The Hole (Housing)
Min: 0.998 | Max: 1.002 in
Drawing B — The Pin (Shaft)
Min: 0.988 | Max: 0.992 in
Look at the cross-section on the right. The purple ring is the hole, the blue circle is the pin, and the gap between them is your clearance.
Think About the Extremes
For a pin-in-hole, the tightest fit happens when:
- The hole is at its smallest (0.998)
- The pin is at its largest (0.992)
And the loosest fit happens when:
- The hole is at its largest (1.002)
- The pin is at its smallest (0.988)
Building a Tolerance Stack
What you just did — calculating worst-case clearance — is the core of a tolerance stack analysis. Let's formalize the process so you can apply it to any assembly, not just a simple two-part problem.
Step 1: Identify the critical gap.
What are you trying to control? In our case, it's the diametral clearance between pin and hole.
Step 2: List every dimension in the chain.
Walk from one side of the gap, through the parts, to the other side. Each dimension that contributes gets listed.
Step 3: Assign direction.
Dimensions that increase the gap are positive (+). Dimensions that decrease the gap are negative (−).
Step 4: Stack them up.
| Dimension | Nominal | Tol | Min | Max | Dir |
|---|---|---|---|---|---|
| Hole Ø | 1.000 | ±0.002 | 0.998 | 1.002 | + |
| Pin Ø | 0.990 | ±0.002 | 0.988 | 0.992 | − |
| Clearance | 0.010 | ±0.004 | 0.006 | 0.014 |
What If the Tolerances Were Tighter?
Let's say the pin tolerance was ±0.004 instead of ±0.002. Now the pin could be as large as 0.994 in.
Worst-case clearance: 0.998 − 0.994 = 0.004 in. Still fits, but barely.
And if the pin nominal was 1.000 ±0.004? Max pin = 1.004. Min clearance = 0.998 − 1.004 = −0.006 in.
This is exactly why you do a tolerance stack before releasing drawings — not after parts arrive.
Position Tolerance — It's Not Just About Size
So far we've only looked at how big the pin and hole are. But there's another problem: where is the hole?
Even if the hole is perfectly sized, if it's drilled 0.008 in off-center, the pin might not fit. This is where GD&T position tolerance comes in.
On a drawing, a position callout looks like this:
Position | Ø0.008 tolerance zone | at MMC
This means the center of the hole must fall within a circular zone of Ø0.008 in, centered on the true position from the drawing.
Adding Position to the Stack
When the hole is off-position, you lose clearance on one side. In a worst-case stack, you subtract the position tolerance from the available clearance.
For a position of Ø0.008, the worst-case shift is 0.004 in radial (half the diametral zone). But since we're doing a diametral stack, we use the full Ø0.008.
| Dimension | Nominal | Tol | Worst Min | Worst Max | Dir |
|---|---|---|---|---|---|
| Hole Ø | 1.000 | ±0.002 | 0.998 | 1.002 | + |
| Pin Ø | 0.990 | ±0.002 | 0.988 | 0.992 | − |
| Hole Position | 0.000 | Ø0.008 | shift up to 0.008 | − | |
| Clearance | 0.010 | −0.002 | 0.014 | ||
MMC Bonus Tolerance — Free Real Estate
Remember that Ⓜ symbol in the position callout? That's the Maximum Material Condition (MMC) modifier, and it's your best friend in tolerance stacking.
MMC for a hole = the smallest the hole can be (most material remaining) = 0.998 in
MMC for a pin = the largest the pin can be (most material) = 0.992 in
How Bonus Tolerance Works
If the hole is produced at Ø1.000 (its nominal), that's 0.002 larger than MMC (0.998). You get 0.002 in of bonus added to your position tolerance:
Actual position tolerance = stated (0.008) + bonus (0.002) = Ø0.010
Instead of thinking about size and position separately, MMC lets you combine them into one concept: the Virtual Condition.
Virtual Condition (hole) = MMC − position tol = 0.998 − 0.008 = Ø0.990
Virtual Condition (pin) = MMC + position tol = 0.992 + 0.000 = Ø0.992
Worst-case clearance with MMC: 0.990 − 0.992 = −0.002 in... unless we also put position tolerance on the pin.
In our case, if the pin also has a position of Ø0.004 at MMC:
Pin VC = 0.992 + 0.004 = Ø0.996
Hole VC = 0.998 − 0.008 = Ø0.990
Worst-case clearance = 0.990 − 0.996 = −0.006 in — interference!
Hmm, still doesn't work. The fix? Either loosen the tolerances, increase the nominal gap, or reduce position tolerances. That's what the sandbox is for.
You've Completed the Lessons!
You now understand the building blocks:
- Bilateral tolerances define the size range of each feature
- Worst-case stacking answers "will it always assemble?"
- Position tolerance accounts for location error
- MMC bonus gives you extra position tolerance as features depart from MMC
Experiment Freely
Adjust any value below and watch the cross-section and results update live.