Why GD&T Saves Money on Machined Parts
Most prototype drawings we receive use coordinate tolerancing: every dimension carries a plus-minus value, and every hole gets its own ±0.05 mm block. It looks rigorous. In practice it over-constrains the part and inflates the quote. Geometric dimensioning and tolerancing — GD&T — describes function instead of geometry, and in CNC machining that difference shows up directly on the invoice.
Here is the core idea. A ±0.05 mm tolerance on a hole location creates a square tolerance zone. The diagonal of that square is about 1.41 times larger than the side, which means a part can pass inspection at the corner of the square while still failing to assemble. A true position callout of Ø0.14 mm at MMC gives you a circular zone with 57 percent more usable area than the equivalent square — and it actually matches how a pin fits into a hole.
Start With the Datums, Not the Tolerances
The single biggest GD&T mistake on prototype drawings is picking datums after everything else is dimensioned. Datum features should be the surfaces that actually locate the part in its assembly, in the order the assembly touches them.
- Primary datum (A): The largest, flattest, most stable mounting face. Usually the face that bolts to the next assembly.
- Secondary datum (B): A long edge or a pair of dowel holes that stops rotation.
- Tertiary datum (C): A shorter feature that stops the last degree of freedom.
Two rules follow from this. First, datums must be machined, never as-cast or as-extruded. A datum on a raw extrusion surface can shift by ±0.5 mm between batches, and every downstream tolerance inherits that error. Second, datums must be reachable by a probe or a fixture. We have seen drawings where datum A was the far side of a deep pocket that no CMM probe could touch without a custom angled stylus. That adds inspection cost for no functional benefit.
True Position and Maximum Material Condition
True position is the workhorse of GD&T on machined parts, and it is where most cost savings hide. Consider a four-hole bolt pattern on a flange. With coordinate tolerancing you might call each hole at ±0.05 mm from two edges. That is a square zone per hole, and the holes are checked independently, so a pattern that is uniformly shifted can still fail even though it would bolt up fine.
Switch to position: Ø0.2 mm at MMC to datums A, B, C. Now the entire pattern is checked as a group against the datums, and because the tolerance applies at maximum material condition, you get bonus tolerance as the holes drift away from their smallest size. A hole at the large end of its size range might gain another 0.1 mm of positional tolerance. That bonus is real — it is the clearance you actually have — and it lets the machinist hold a looser process without risking assembly.
Typical values we quote against: Ø0.1 mm at MMC for precision bores and bearing seats, Ø0.2 mm for general bolt patterns, Ø0.3–0.5 mm for clearance holes in sheet-metal-style flanges. Anything under Ø0.05 mm starts requiring jig boring or a coordinate-measuring loop mid-process, and the cost curve bends upward sharply.
Cost Curves: Where Tight Tolerances Get Expensive
Tolerance cost is not linear. On 6061-T6 in a three-axis mill, going from ±0.1 mm to ±0.05 mm typically adds 10–20 percent to cycle time because of an extra finishing pass and slower feeds. Going from ±0.05 mm to ±0.01 mm can add 60–100 percent: you now need temperature-stable coolant, a finishing pass with a fresh insert, and in-process measurement. Below ±0.005 mm (±0.0002 in) you are into grinding or jig boring territory on most shops, and the part may need a second setup on different equipment.
The same curve applies to geometric controls. Flatness of 0.05 mm over a 100 mm face is routine. Flatness of 0.01 mm over the same face may require lapping or a carefully sequenced facing pass with stress relief between roughing and finishing. On thin-walled parts, most flatness problems are actually fixturing problems: clamp the wall, machine it flat, release the clamp, and it springs back. Tell your machinist the wall thickness and they will choose vacuum or low-pressure clamping instead.
Common GD&T Mistakes on Prototype Drawings
- Applying position without datums. A true position callout with no datum reference is unmeasurable. Inspection will guess, and the guess usually works against you.
- Tolerancing every surface. Uncontrolled dimensions still have a general tolerance from the title block. Adding explicit ±0.02 mm to a non-functional face only creates rejection risk.
- Confusing concentricity with runout. Concentricity requires measuring the derived median axis and is genuinely expensive. Circular runout or total runout usually captures the functional requirement — a shaft that spins true — at a fraction of the inspection cost.
- Stacking profile and position on the same feature. Pick the control that matches the function. Two controls on one feature means the part must satisfy both, and the tighter one dominates.
- Ignoring projected tolerance zone. For threaded holes or press-fit pins, the axis error at the top of the pin matters, not at the surface. A projected tolerance zone extends the position control above the part surface and prevents a tilted hole that still passes at the surface.
When GD&T Is Not Worth It
If you are making three brackets that bolt together with 1 mm clearance slots, coordinate tolerancing with a sane general tolerance is fine. Do not spend an hour writing datum structures for a part that has no assembly interface. GD&T earns its keep when parts interface, when you have multiple suppliers, or when a design will move from prototype into production and the drawing needs to communicate function unambiguously. For a die casting that will later be machined on critical faces, a clear datum structure on the casting drawing prevents an expensive argument about whose tolerance caused the mismatch.
Practical Takeaway
Before you release the next drawing, do three things. Choose datums from the assembly, not from the modeling origin. Convert hole patterns to true position at MMC. Then walk every tolerance and ask what breaks if it doubles — if the answer is nothing, loosen it. On a typical prototype enclosure this review removes 30 to 50 percent of the tight callouts, and the quote usually follows.
