GD&T for CNC Machined Parts: What to Call Out & What It Costs
Not all GD&T callouts cost the same to machine and inspect. This guide maps every geometric control to its CNC achievability, cost impact, and inspection method so you can specify exactly what your part needs and nothing more.
Quick Answer
CNC machining holds position on holes, flatness on milled faces, and perpendicularity on square features well These are baseline-cost callouts at standard tolerance ranges. Callouts that get expensive include tight profile on freeform surfaces (requires 5-axis + CMM), cylindricity below 0.001 in. (requires grinding or honing), and concentricity (requires median-point CMM measurement). The cost impact of any GD&T callout flows through three channels: machining strategy, fixturing complexity, and inspection method. In metric terms, the tight form-control threshold is about 0.025 mm.
Why GD&T Costs What It Does on CNC Parts
Every GD&T callout on a drawing affects three cost drivers. Understanding these drivers lets you make informed tolerance-for-cost trade-offs before your drawing hits the shop floor.
Machining strategy
Tighter tolerances require slower feed rates, finer step-overs, spring passes (a final light cut with no radial engagement to remove tool deflection), and sometimes secondary operations like grinding or honing. A flatness callout of 0.005 in. is a normal milling operation; 0.001 in. may require a light skim cut on stress-relieved material. In metric terms, that is about 0.13 mm versus 0.025 mm.
Fixturing complexity
Position tolerance references datums, which define how the part is held and located in the fixture. Tight position with a 3-datum scheme may require a custom fixture with hardened locating pins and clamping, often costing $500–2,000 per fixture. Standard bolt patterns at ⌀0.014 in. can use a standard vise with edge stops. In metric terms, that is about 0.36 mm for the standard bolt-pattern position window.
Inspection method and frequency
Each GD&T callout must be verified. Manual methods (surface plate + indicator, pin gages) are fast and cheap. CMM inspection runs $75–150/hr and takes 1–5 min per feature. Functional gaging (for position at MMC) is a one-pass check. The inspection method is determined by the GD&T control type and tolerance magnitude.
The 80/20 rule of GD&T cost
On a typical CNC part, 20% of the GD&T callouts drive 80% of the inspection cost. Identifying which callouts are functional (must be tight) versus cosmetic or non-critical (can use block tolerance) is the single largest lever for reducing part cost. For broader cost reduction strategies, see our guide to reducing CNC machining cost.
GD&T Controls That CNC Holds Well
These callouts fall within normal CNC process capability and add minimal cost above standard machining. They are the callouts you should default to when specifying GD&T on machined parts.
Position on holes (at MMC)
A 3-axis CNC with a standard vise holds hole position to ⌀0.010 in. without special fixturing. Specifying MMC enables functional gaging with a hardened gage that places pins at the virtual condition locations. One pass gives one decision, with no CMM operator required. In metric terms, that is about 0.25 mm at the tight end and 0.36 mm at the looser end.
Flatness on milled faces
Fly-cutting or face-milling in aluminum or steel routinely produces flatness within 0.002 in. over surfaces up to roughly 6 × 6 in. (150 × 150 mm). Larger surfaces or thinner cross-sections may need a finishing pass on stress-relieved stock.
Perpendicularity on machined faces
CNC spindles are aligned perpendicular to the table within 0.0002 in. per foot. Any face milled in a single setup is inherently perpendicular to the datum face sitting on the vise jaws. Cost risk comes from thin walls that deflect during cutting. In metric terms, the machine alignment is about 0.005 mm per foot.
Circular runout on turned diameters
CNC lathes hold runout to 0.001 in. on features machined in a single chucking. This is the natural process output, so there is no extra cost. Re-chucking or transferring between chuck and collet introduces concentricity error. In metric terms, that is about 0.025 mm at the tight end.
GD&T Controls That Get Expensive on CNC
These callouts require special fixturing, secondary operations, or extensive CMM verification. Apply them only when the feature genuinely requires the control.
Profile on freeform surfaces
Freeform profile with datums typically requires 5-axis machining (ball-end mill with continuous tool-path contouring), though 3-axis can work if the profile and datums are accessible in a single setup. Full CMM 3D surface scan is required. The combination of high machine-hour rate ($150–250/hr for 5-axis) and extended CMM time makes this the most expensive GD&T callout category. In metric terms, the tight end is about 0.025 mm.
Cylindricity below 0.001 in. (0.025 mm)
Turning and boring can achieve 0.002 in. cylindricity. Below 0.001 in. typically requires ID/OD grinding or honing, which is a secondary operation that adds $20–50+ per bore. The CMM must do a multi-section scan to verify. In metric terms, that is about 0.05 mm at the achievable end and 0.025 mm when it gets expensive.
Tight position at RFS
RFS means no bonus tolerance and no functional gaging. Every hole on every part must be CMM-verified. Precision fixturing with hardened located pins is required. Combined fixturing + 100% CMM drives the cost premium. In metric terms, that is about 0.05–0.13 mm.
Concentricity (avoid on new designs)
Requires median-point CMM measurement. The method is computationally intensive and slow. ASME Y14.5-2018 recommends position or runout for coaxial features. Use runout for rotating parts and position for static coaxiality. In metric terms, that is about 0.025–0.05 mm.
GD&T Control vs CNC Cost & Inspection Method
Cost impacts are relative to baseline (standard 3-axis CNC with first-article CMM) on aluminum and steel alloys at current US job shop rates. “Easy range” is achievable without special setup; “tight range” requires precision fixturing, secondary operations, or 100% inspection.
| Control | Sym. | Easy Range | Tight Range | Cost (Easy) | Cost (Tight) | Inspection |
|---|---|---|---|---|---|---|
| Position (holes/pins) | ⌖ | ⌀0.010–0.014 in. (0.25–0.36 mm) | ⌀0.002–0.005 in. (0.05–0.13 mm) | Baseline | +40–100% | Functional gage (MMC) or CMM |
| Flatness | ⏥ | 0.002–0.005 in. (0.05–0.13 mm) | 0.0005–0.001 in. (0.013–0.025 mm) | Baseline | +30–60% | Surface plate + indicator or CMM |
| Perpendicularity | ⟂ | 0.002–0.005 in. (0.05–0.13 mm) | 0.0005–0.001 in. (0.013–0.025 mm) | Baseline | +25–50% | Square + indicator or CMM |
| Parallelism | // | 0.002–0.005 in. (0.05–0.13 mm) | 0.0005–0.001 in. (0.013–0.025 mm) | Baseline | +25–50% | Surface plate + indicator or CMM |
| Angularity | ∠ | 0.003–0.005 in. (0.08–0.13 mm) | 0.001–0.002 in. (0.025–0.05 mm) | +5–10% | +30–60% | Sine bar + indicator or CMM |
| Profile of a Surface | ⌓ | 0.005–0.010 in. (0.13–0.25 mm) | 0.001–0.003 in. (0.025–0.08 mm) | +10–20% | +60–150% | CMM (3D surface scan) or structured light |
| Circular Runout | ↗ | 0.002–0.005 in. (0.05–0.13 mm) | 0.0005–0.001 in. (0.013–0.025 mm) | Baseline (turning) | +30–60% | V-block + dial indicator (one rotation) |
| Total Runout | ⌰ | 0.003–0.008 in. (0.08–0.20 mm) | 0.001–0.002 in. (0.025–0.05 mm) | +5–15% | +40–80% | V-block + indicator (traverse full length) |
| Cylindricity | ⌭ | 0.002–0.005 in. (0.05–0.13 mm) | 0.0005–0.001 in. (0.013–0.025 mm) | +5–10% | +50–100% | CMM (multi-section scan) or roundness tester |
| Circularity | ◯ | 0.001–0.003 in. (0.025–0.08 mm) | 0.0003–0.0005 in. (0.008–0.013 mm) | Baseline (turning) | +40–80% | V-block + indicator or roundness tester |
| Straightness | ⏤ | 0.002–0.005 in. (0.05–0.13 mm) | 0.0005–0.001 in. (0.013–0.025 mm) | Baseline | +20–40% | V-block + indicator or CMM |
| Concentricity | ◎ | 0.003–0.005 in. (0.08–0.13 mm) | 0.001–0.002 in. (0.025–0.05 mm) | +15–25% | +60–120% | CMM (median-point algorithm) |
Not Sure Which Callouts Drive Cost on Your Part?
Upload your drawing and get a free DFM review from MakerStage engineers. We will flag GD&T callouts that drive unnecessary cost, suggest tolerance-for-cost trade-offs, and recommend the inspection approach that matches your volume, whether that is functional gaging, first-article CMM, or sampling.
Get a Quote with Free DFM ReviewInspection Method per GD&T Control
The inspection method determines the per-part verification cost. As a rule: if you can inspect with a manual tool (indicator, pin gage, functional gage), the cost is low. If the callout requires a CMM, cost scales with the number of features and the scan density. For a detailed inspection process reference, see our inspection processes guide.
| Method | Typical Rate | Time per Feature | Controls Verified | When to Use |
|---|---|---|---|---|
| Functional gage (go/no-go) | $0.50–2/part (amortized) | 5–15 sec | Position at MMC | Production qty >50 parts with position at MMC. Gage cost $500–2,000. |
| Surface plate + dial indicator | $40–75/hr (manual) | 1–3 min | Flatness, parallelism, runout | First article and sampling. Simple form/orientation checks on flat or round features. |
| Pin gage / plug gage | $0.25–1/feature | 10–30 sec | Hole diameter (go/no-go) | Quick size check before CMM. Verifies diameter only, not position. |
| CMM (touch probe) | $75–150/hr | 1–5 min per feature | All GD&T controls | First article inspection, tight tolerances, complex datum schemes. Required for profile, cylindricity, concentricity. |
| Structured light / laser scanner | $100–200/hr | 5–15 min per surface | Profile of a surface, freeform contours | 5-axis freeform parts where point-by-point CMM is too slow. Captures full surface deviation map. |
GD&T Decision Table for CNC Parts
Match your design scenario to the recommended GD&T callout. Each row explains why that control is the right choice and gives a typical tolerance range for CNC.
| Design Scenario | Recommended Callout | Why | Typical Range |
|---|---|---|---|
| Bolt-pattern clearance holes (4× ¼-20 through) | Position at MMC | Cylindrical zone gives 57% more area than ±. MMC enables functional go/no-go gaging, which is the fastest inspection method for production. In metric terms, the standard zone is about 0.25–0.36 mm. | ⌀0.010–0.014 in. (0.25–0.36 mm) |
| Dowel-pin press-fit holes (locating features) | Position at RFS | Fit is independent of hole size, so the pin must remain concentric regardless of how close the hole is to its limits. RFS prevents bonus tolerance from allowing misalignment. In metric terms, that is about 0.05–0.13 mm. | ⌀0.002–0.005 in. (0.05–0.13 mm) |
| Sealing face (O-ring groove mating surface) | Flatness + Surface Finish (Ra) | O-ring seals require a flat, smooth surface. Flatness controls waviness; Ra spec controls microfinish. No datum is needed because the surface is assessed in isolation. In metric terms, the flatness band is about 0.025–0.05 mm and the surface finish is 0.8–1.6 µm Ra. | 0.001–0.002 in. (0.025–0.05 mm) flat; Ra 32–63 μin. (0.8–1.6 μm) |
| Motor mounting face (perpendicular to bore axis) | Perpendicularity to datum (bore axis) | The face must be square to the bearing bore so the motor shaft runs true. Perpendicularity inherently controls flatness per Rule #1. In metric terms, the typical band is about 0.025–0.08 mm. | 0.001–0.003 in. (0.025–0.08 mm) |
| Bearing bore (press-fit or slip-fit) | Cylindricity (or circularity + straightness) | Bearing seats require uniform bore geometry in all directions. Cylindricity is the single control that captures roundness, straightness, and taper. In metric terms, that is about 0.013–0.025 mm. | 0.0005–0.001 in. (0.013–0.025 mm) |
| Rotating shaft OD (in a bearing) | Circular runout (or total runout for long shafts) | Runout combines coaxiality and roundness in one check. Circular runout for short journals; total runout for full-length shafts where taper matters. In metric terms, that is about 0.025–0.08 mm. | 0.001–0.003 in. (0.025–0.08 mm) |
| Freeform 5-axis surface (complex contour) | Profile of a Surface with datums | Profile is the only control that constrains form, orientation, and location of a non-planar surface in a single FCF. Requires CMM or structured-light scan verification. In metric terms, that is about 0.08–0.25 mm. | 0.003–0.010 in. (0.08–0.25 mm) |
| Non-critical surfaces (cosmetic, non-mating) | Block tolerance (± from title block) | No GD&T needed. Title-block ± tolerances (typically ±0.005–0.010 in.) are sufficient. Adding GD&T to non-functional features increases inspection time without functional benefit. In metric terms, that is about 0.13–0.25 mm. | ±0.005–0.010 in. (±0.13–0.25 mm) |
How to Avoid Over-Tolerancing CNC Parts
Over-tolerancing, meaning adding GD&T to features that do not need it, is the number-one cost driver on engineering drawings sent to CNC shops. Every unnecessary callout adds inspection time and constrains the shop’s process freedom. Here are the patterns to watch for.
Flatness on every face
Position at RFS on clearance holes
Cylindricity on every bore
Form tolerances tighter than the size tolerance
GD&T on non-mating cosmetic surfaces
Too many datum references
The drawing review test
Before releasing a drawing, point to each GD&T callout and ask: “If this feature is at the limit of this tolerance, does the part still assemble and function?” If yes, the tolerance is correct. If you are not sure, loosen it first. You can always tighten later. If the answer is “it doesn’t matter either way,” remove the callout entirely and use the block tolerance. For a deeper look at DFM strategies, see our DFM guidelines.
GD&T for CNC Machining FAQ
Related Resources
Get Your GD&T Drawing Quoted with Free DFM Review
Upload your drawing with GD&T callouts. MakerStage engineers review every feature control frame, flag cost drivers, and suggest tolerance-for-cost trade-offs before you pay for a single part.
Get Free Quote with DFM Review