How to Set Geometric Tolerance on Drawings

• 1
  Key takeaways
• 2
  Why set geometric tolerance on drawings at all
• 3
  Choose datums before you write any frame
• 4
  Build the feature control frame correctly
• 5
  Use material modifiers and basic dimensions with care
• 6
  Match the tolerance zone to what the process can hold
• 7
  Step-by-step: set geometric tolerance on drawings
• 8
  Which control to use for which feature

A plus/minus tolerance controls size. It says nothing about whether a hole is straight, whether a face is flat, or whether two bores share an axis. On a bracket with three mating surfaces, those are the dimensions that decide whether the part assembles. Geometric tolerance closes that gap by tying each feature to a datum and giving it a measurable zone.

The practical reason to set geometric tolerance on drawings is inspection. A callout like flatness 0.05 defines a zone an inspector can verify with a surface plate and indicator. A note that says "must be flat" does not. When the drawing is measurable, the first article report is meaningful and the production run stays consistent.

There is a cost side too. Every geometric control adds inspection time. A true position callout at Ø0.1 mm on a deep bore may need a CMM program, while the same feature at Ø0.25 mm can often be checked with a pin gauge. Good drawings keep the tight controls where function demands them and leave the rest open.

• 1
  Size vs. geometrySize tolerance sets the limit; geometric tolerance sets the form and location.
• 2
  Measurable beats descriptiveIf the shop cannot check it, the callout is decoration.
• 3
  Cost follows inspectionTighter zones mean slower checking and higher piece price.

Datums are the reference frame for everything else. Start with the primary datum: the largest, flattest surface that seats in the assembly. On a machined housing, that is usually the mounting face. Mark it as datum A and make it the first feature the machinist prepares, because every later cut references it.

The secondary datum B should remove one more degree of freedom. A dowel hole or a slot edge works well. The tertiary datum C locks the last rotation. Three datums are enough for most prismatic parts. If you find yourself adding a fourth, the part probably needs a functional gauge instead of a CMM setup.

Order matters. If datum A is a rough cast surface and datum B is a finished bore, the machinist has to flip the setup or add an operation. On the parts we run, a datum scheme that follows the machining sequence typically saves one setup and 15 to 30 minutes of cycle time per lot.

• 1
  A is the seating faceLargest flat surface touching the assembly.
• 2
  B removes a translationA hole or slot that constrains one axis.
• 3
  C removes rotationThe final lock, often a second hole or an edge.
• 4
  Avoid datum conflictsDo not reference a surface the part never touches in use.

A feature control frame reads left to right: symbol, tolerance value, material modifier if needed, then datum references in order. The symbol sets the type of control. Flatness, straightness, roundness, and cylindricity control form. Parallelism, perpendicularity, and angularity control orientation. Position, concentricity, and symmetry control location. Runout controls rotation.

For a bolt hole pattern, the common choice is position with a diameter zone, for example Ø0.25 mm MMC, referenced to A, B, C. The diameter symbol tells the inspector the zone is cylindrical, which matches how the hole functions. Leaving the diameter symbol off turns the zone into two parallel planes and changes the acceptance math.

Keep one control per frame unless two controls genuinely share the same zone. Perpendicularity and position on the same hole are different requirements and belong in separate frames. Stacked frames are a frequent source of measurement disputes because the inspector has to guess which one governs a borderline part.

• 1
  Symbol firstIt defines the zone shape and the check method.
• 2
  Include Ø for holesA cylindrical zone reflects how a pin or bolt fits.
• 3
  Datums in orderA, then B, then C, matching the setup sequence.
• 4
  One idea per frameSplit unrelated controls into separate frames.

The maximum material modifier, MMC, allows bonus tolerance as a feature departs from its maximum size. A hole at Ø10.0 +0.2 with position Ø0.2 MMC gains extra position tolerance when the hole is drilled oversize. That is good for cost, because the shop can accept parts that still assemble. It only works when the mating part is fixed, such as a bolt in a clearance hole.

Least material modifier, LMC, is used when minimum wall thickness matters more than assembly. Think of a bushing pressed into a bore where a thin wall could crack. In that case the callout protects the wall, not the fit.

Basic dimensions are boxed values with no tolerance. They locate a feature relative to the datums and work with the position frame to define the true position. Never leave a basic dimension without a corresponding geometric control, and never tolerance a basic dimension directly. That combination creates an unresolved requirement on the shop floor.

• 1
  MMC for clearance holesBonus tolerance helps assembly without scrapping parts.
• 2
  LMC for wall thicknessProtects minimum material conditions.
• 3
  Basic dimensions need a frameA boxed value alone is not inspectable.
• 4
  RFS is the defaultIf no modifier is shown, the tolerance applies regardless of size.

A drawing can ask for anything. The shop can only hold what the machine and setup allow. On our 5-axis centers, position tolerances around Ø0.02 to Ø0.05 mm are routine on features cut in one setup. When the feature requires a second setup, the stack-up of two fixtures usually pushes the realistic limit to Ø0.05 to Ø0.1 mm.

Surface finish interacts with form tolerance. A face machined to Ra 1.6–3.2 μm will not hold a flatness of 0.005 mm across 200 mm, because the tool marks themselves sit in that range. If you need flatness below 0.01 mm, specify a finer finish such as Ra 0.8–1.6 μm and plan a finishing pass with a sharp tool and light depth of cut.

Material matters as well. Aluminum 6061 and 7075 hold tight geometric zones well. Stainless 316 and 17-4PH move more after machining, so a flatness callout on a thin stainless plate may require stress relief or a second finishing cut. Titanium and Inconel add tool wear, which shows up as drift across a production run.

• 1
  One setup, tight zonesØ0.02 to Ø0.05 mm position is realistic.
• 2
  Two setups, looserAllow Ø0.05 to Ø0.1 mm for fixture stack-up.
• 3
  Finish limits formVery fine flatness needs a fine surface finish.
• 4
  Thin walls moveAdd stock or stress relief for stainless and titanium.