Every CNC machinist has seen the drawing. A hole is located with a simple ±0.005″ linear dimension from two edges. The part comes off the machine. The hole measures in spec per the print. It doesn’t fit.
Why? Because the linear tolerance created a square tolerance zone, but the mating part required a round one. The hole was within 0.005″ in X and Y, but 0.007″ diagonally—and that’s where the pin bound up.
This is precisely the problem that True Position in GD&T (Geometric Dimensioning and Tolerancing) is designed to solve. It defines a cylindrical tolerance zone centered on the exact nominal location, reflecting how parts actually assemble.
But specifying True Position correctly isn’t just about picking a number and putting a box on the drawing. The choice of datums, the use of material condition modifiers like MMC, and the way the tolerance is applied directly affect how the part is set up, machined, and inspected—and ultimately, whether it works and what it costs.
In this guide, we’ll walk through how to specify True Position for CNC machined parts so your intent is clear to the machinist, your part passes inspection, and your assembly works the first time. We’ll draw from real experience at Baosheng Industry, where we machine parts with position tolerances as tight as 0.0008″ for aerospace and medical components.
Explore our precision CNC machining services with expert GD&T interpretation →
What Is True Position GD&T? (And Why It’s Different From ± Tolerances)
True Position is defined in the ASME Y14.5 standard and represented by the symbol ⌖. It specifies a zone—usually cylindrical—within which the center, axis, or center plane of a feature must lie relative to specified datums.
The Fundamental Difference
| Characteristic | Linear ± Tolerance | True Position (⌖) |
|---|---|---|
| Tolerance Zone Shape | Square or rectangular | Cylindrical (or width, for some applications) |
| Corner Effect | Accepts parts that are further out diagonally (up to ~1.4× the stated tolerance) | Rejects parts that exceed the radial tolerance in any direction |
| Datum Reference | Usually implied by dimensioning edges | Explicitly stated; defines the coordinate system |
| Material Modifiers | Not applicable | MMC, LMC, RFS modifiers can be applied to adjust tolerance with feature size |
| Inspection | Measured linearly | Measured as a radial deviation from true center |
A Simple Example:
A hole located at X=2.000″, Y=1.500″.
- ±0.005″ linear tolerance: The hole center must lie within a 0.010″ × 0.010″ square. The diagonal is 0.014″. A hole at X=2.005″, Y=1.505″ is 0.007″ off true center but passes.
- ⌖ 0.010″ diameter tolerance: The hole center must lie within a cylindrical zone 0.010″ in diameter at true position. That same 0.007″ off-center hole passes here too, but a hole at X=2.005″, Y=1.505″ (0.007″ radial) would also pass. Wait—let’s recalculate: a hole at (2.005, 1.505) is off by (0.005, 0.005) vector, radial error = √(0.005²+0.005²) = 0.00707″. So it passes a 0.010″ diameter zone. But the key is that any point at exactly 0.005″ in X and Y is still inside the circle (radius 0.005″ = diameter 0.010″). However, if the hole were at X=2.007″, Y=0, that’s 0.007″ radial, still passes. The advantage is that the entire 0.010″ diameter zone is functionally driven—matching a round pin or fastener—rather than the artificial square.
For cylindrical mating features, True Position ensures a functional assembly where linear tolerances might not.
Read more about how manual DFM review catches GD&T issues before machining →
Why True Position Matters for CNC Machined Parts
Specifying True Position correctly does three things for the CNC machining process:
1. It Defines the Setup Datums Clearly.
A True Position callout includes explicit datums—typically a primary plane, a secondary plane, and a tertiary point or plane. These datums tell the machinist exactly how to fixture the part. The primary datum is the first surface to contact the fixture. The secondary constrains the next degree of freedom. The tertiary completes the 3-2-1 location.
Without explicit datums, the machinist assumes the datums from whatever edges the dimensions originate from. If those edges aren’t machined square in the same setup, or if they have significant surface variation, the assumed coordinate system may not match what the designer intended.
2. It Creates a Common Coordinate System for Multiple Features.
When dowel pins, bearing bores, and mounting holes on different faces of a part must align to each other, True Position with a common datum reference frame ensures they all relate to the same origin. Without this, tolerance stackup between features on different faces can cause misalignment that’s difficult to diagnose.
3. It Enables Functional Inspection.
With True Position, inspection directly verifies the assembly condition. The CMM or functional gauge checks whether the feature fits, not just whether it’s within arbitrary linear limits. For features with MMC applied, a fixed functional gauge can be used—the hole must accept a pin of a specific size at the true position. This is faster and more reliable than measuring linear deviations and calculating radial error.
See how we combine 5-axis machining with tight GD&T tolerances →
How to Properly Specify True Position on Your Drawing
Here is a step-by-step approach to creating a clear, manufacturable True Position callout.
Step 1: Select a Functional Primary Datum
The primary datum should be the surface that establishes the part orientation in the assembly. For most CNC parts, this is a large, machined flat face. The machinist will put this face down on the fixture.
Good practice: Machine the primary datum face first, then use it to locate the part for all subsequent operations. If possible, make this the first machining operation on the part.
Step 2: Choose Secondary and Tertiary Datums That Are Accessible and Repeatable
- Secondary datum: A surface perpendicular to the primary. Typically a long edge or machined side. It constrains rotation.
- Tertiary datum: A point or surface that constrains the last degree of freedom. Often a shorter edge or a machined boss.
The datums must be features the machinist can actually touch off on or probe. Avoid using cast surfaces, rough stock edges, or features that will be machined away in an intermediate operation as datums.
Step 3: Define the True Position Tolerance Value
The value is the diameter of the cylindrical tolerance zone. It should be based on the functional clearance between the feature and its mating component.
Rule of thumb for fixed fasteners:
Tolerance Zone Diameter = Minimum Clearance Hole Diameter − Maximum Fastener Diameter.
For a 0.250″ bolt in a 0.266″ clearance hole, the available tolerance budget is 0.016″ for all sources of position error (the hole’s position, the threaded hole’s position, and any fastener float). This budget must be allocated.
Step 4: Apply MMC, LMC, or RFS
- MMC (Maximum Material Condition): The tolerance increases as the feature departs from MMC. This is the most common for clearance holes because it takes advantage of the additional clearance from larger holes. If a hole is made larger, its position can be looser and still accept the fastener.
- LMC (Least Material Condition): Tolerance increases as the feature departs from LMC. Used for edge distances or minimum wall thickness control.
- RFS (Regardless of Feature Size): Tolerance stays constant. Used for press fits, precision bearing bores, or when size isn’t meant to compensate.
For CNC machining: MMC is preferred for clearance holes because it gives the machinist more tolerance to work with, reducing cost. RFS is used when the position is critical regardless of size.
Step 5: Compose the Feature Control Frame
A complete True Position callout includes:
⌖ | Ø 0.010 Ⓜ | A | B | C
- ⌖ : True Position symbol
- Ø : Diametral zone (if omitted, it’s generally a width in a specific direction)
- 0.010 : Tolerance value
- Ⓜ : MMC modifier (if applicable; could be L, or omitted for RFS)
- A | B | C : Datum references in order of precedence
Upload your CAD with GD&T for a free DFM review—we’ll check your datums and tolerances →
Common True Position Mistakes and How to Avoid Them
Mistake 1: Using ± Tolerances Where True Position Is Needed
The Error: Locating a hole with ±0.005″ from two edges, then wondering why dowel pins bind on some parts.
The Fix: Use True Position with a cylindrical tolerance zone. The datum reference frame makes the coordinate system explicit.
Mistake 2: Datums That Aren’t Machined or Aren’t Accessible
The Error: Selecting a datum that is a cast surface, a rough saw-cut edge, or an internal feature that can’t be probed without first machining something else.
The Fix: Choose machined, accessible surfaces for datums. The primary datum should be a face large enough to rest stably on the fixture. The secondary should be a long enough edge to orient the part repeatably.
Mistake 3: Not Applying MMC to Clearance Holes
The Error: Specifying RFS on clearance holes for bolts or screws. This forces the machinist to hold a tight position regardless of hole size, driving up cost for no functional benefit.
The Fix: Apply MMC to all clearance holes for fasteners. This gives the machinist additional tolerance when the hole is made toward the upper size limit, which happens naturally as drills wear.
Mistake 4: Forgetting That Position Tolerance Also Controls Orientation
The Error: Adding a separate perpendicularity callout to a hole that already has a position tolerance relative to the same primary datum.
The Fix: True Position inherently controls perpendicularity to the primary datum within the same tolerance zone. A separate perpendicularity callout is redundant and may create conflicting requirements.
Mistake 5: Specifying a Composite Tolerance Incorrectly
The Error: Using a composite position tolerance with two tolerance values without understanding that the lower segment only controls feature-to-feature relationship, not location relative to datums.
The Fix: If you need to tightly control the pattern of holes relative to each other but allow the whole pattern to shift relative to the datums, use a composite frame. The upper segment controls location to datums; the lower segment controls spacing within the pattern. Ensure both segments and their datums are correctly specified for your functional intent.
See how our manual DFM catches GD&T issues before metal is cut →
True Position and Datum Selection: The Key to Accurate Machining
Datum selection is where the theoretical world of GD&T meets the physical world of CNC machining. The datums you specify on the drawing directly translate into how the part is fixtured.
The 3-2-1 Principle in CNC Machining
| Datum | Constrains | Machining Equivalent |
|---|---|---|
| Primary | 3 points of contact (plane) | Part face seated flat on the fixture table or vise bed |
| Secondary | 2 points of contact (line) | Part edge pushed against a fixed jaw or locating rail |
| Tertiary | 1 point of contact (point) | Part end stop or button |
Datum Selection Guidelines for CNC Machinability
| Guideline | Why It Matters |
|---|---|
| Make the primary datum a large, flat machined surface | Ensures stable seating on the fixture. Avoid curved or interrupted surfaces. |
| Make secondary and tertiary datums orthogonal to each other and to the primary | Simplifies vise and fixture setups. Angled datums require custom fixturing. |
| Specify datums in the order you want them contacted | The machinist will locate the part in datum precedence order. |
| Avoid using features on different setups as datums for each other | A datum on Face B shouldn’t be the reference for a True Position on Face A if Face A is machined first. This creates a chicken-and-egg problem. |
| Don’t use centerlines or theoretical planes as the sole datum | Unless they are derived from physical features with defined tolerances. The machinist can’t align to a centerline that isn’t established by a physical part feature. |
A Practical Example
Bad datum selection:
Primary datum A is the bottom face. Secondary datum B is the centerline of a small hole. The machinist must probe a tiny hole and then align the entire part to it—introducing angular error from probe uncertainty.
Good datum selection:
Primary datum A is the bottom face. Secondary datum B is the long machined side edge. Tertiary datum C is a short machined end face. All three are flat, accessible, and machinable in a single setup.
Learn more about designing parts for efficient CNC setups →
True Position with MMC and LMC: When and Why
Material condition modifiers are the most powerful—and most misunderstood—aspect of True Position for CNC parts.
MMC (Maximum Material Condition): The Manufacturer’s Friend
MMC means the specified tolerance applies when the feature contains the maximum amount of material (smallest hole, largest shaft). As the feature departs from MMC, bonus tolerance is added to the position tolerance.
Example: A hole specified as ⌖ Ø 0.010 Ⓜ | A | B | C, with size 0.250–0.260″.
- At 0.250″ (MMC), position tolerance = 0.010″.
- At 0.255″, bonus = 0.005″. Total position tolerance = 0.015″.
- At 0.260″ (LMC), bonus = 0.010″. Total position tolerance = 0.020″.
Why this helps the machinist:
As a drill wears or a reamer cuts slightly larger, the hole size naturally drifts toward the upper limit. With MMC, the additional tolerance absorbs the position error that may accompany tool wear. The machinist isn’t forced to change tools prematurely to hold an unnecessarily tight position on a hole that will still accept the fastener.
Functional gauge for MMC: A fixed gauge pin at the virtual condition size can be used: Virtual Condition = MMC size − Position tolerance at MMC. If the pin fits, the part passes. This is very fast for inspection.
LMC (Least Material Condition): Edge Distance and Wall Thickness
LMC applies the tolerance at the feature’s smallest material condition (largest hole, smallest shaft). Bonus is added as the feature gets smaller (more material). This is relevant for minimum wall thickness or edge distance.
Example: A hole must maintain 0.030″ minimum edge distance. Specifying the hole position with LMC ensures that as the hole gets larger (approaching LMC), the position tolerance tightens to protect the remaining wall.
When to Use Which Modifier
| Application | Recommended Modifier |
|---|---|
| Clearance holes for bolts/screws | MMC |
| Threaded holes | MMC or RFS (depending on floating/fixed fastener formula) |
| Press-fit dowel holes | RFS (size doesn’t help position deviation) |
| Bearing bores | RFS |
| Features where minimum wall must be maintained | LMC |
| Alignment pins | RFS |
See how our tight-tolerance CNC machining handles MMC, LMC, and RFS parts →
How Baosheng’s Manual DFM Review Helps Get GD&T Right
Automated quoting platforms interpret GD&T through pattern-matching algorithms that often ignore material condition modifiers, misinterpret composite frames, or flag valid callouts as errors because they deviate from standard templates.
At Baosheng, our manual DFM review includes a specific GD&T check:
- We verify that your datums are machinable. If a datum is inaccessible or would require a non-standard setup, we flag it and suggest alternatives—before any metal is cut.
- We check for conflicting or redundant callouts. If your True Position already controls perpendicularity, we note it so you can clean up the drawing.
- We evaluate MMC/LMC/RFS decisions. If a clearance hole is missing MMC, we let you know—and explain how it can reduce machining cost.
- We confirm inspectability. Every callout must be measurable with our CMM or functional gauges. If a tolerance isn’t inspectable, it isn’t manufacturable.
A few minutes of GD&T review before machining can prevent days of rework and hundreds in scrapped parts.
Upload your CAD and GD&T drawing now for a free DFM analysis within 24 hours.
True Position Quick Reference Checklist
Before releasing a drawing with True Position callouts, check:
- True Position (⌖) used instead of ± tolerances for all features that must align with mating components (holes, pins, bores).
- Datum features are physical, machined, and accessible in the intended setup orientation.
- Datum precedence order reflects fixturing order: Primary (3 points), Secondary (2 points), Tertiary (1 point).
- MMC applied to all clearance holes for fasteners.
- LMC applied where minimum edge distance or wall thickness must be maintained.
- Composite tolerance used correctly when feature-to-feature spacing must be tighter than location to datums.
- Redundant orientation controls avoided if position already covers them (e.g., no separate perpendicularity on same datum).
- Tolerance values are based on functional fit calculations, not blanket defaults.
- All callouts are inspectable with available CMM or functional gauge capability.
Get Your GD&T Reviewed Before Machining
At Baosheng Industry, we’ve machined tens of thousands of parts with GD&T requirements ranging from ±0.005″ to ±0.0005″. Our engineers and machinists read Feature Control Frames like a language—and we’ll translate yours into a stable, efficient manufacturing process.
Upload your CAD and drawing for a free DFM review within 24 hours, including specific feedback on your True Position callouts, datum selections, and material condition modifiers.
Free DFM Analysis • GD&T Review Included • 24-Hour Engineer Response • AS9100D / ISO 13485 / IATF Certified • ITAR Registered
Frequently Asked Questions (FAQ)
Q1: What is the difference between True Position and coordinate tolerances for CNC parts?
Answer: Coordinate (linear ±) tolerances create a square tolerance zone, which can accept parts that are further off diagonally than the intended limit. True Position uses a cylindrical tolerance zone that equally limits deviation in all directions. True Position also ties the measurement to explicit datums, reducing ambiguity in setup and inspection.
Q2: When should I use True Position instead of linear ±0.005″?
Answer: Use True Position when a feature must align with a mating part (dowel pins, bolt holes, bearing bores). Linear tolerances are adequate for features that don’t have a critical assembly relationship, such as the overall length of a bracket or the depth of a non-critical pocket.
Q3: What does MMC mean in a True Position callout, and why should I use it?
Answer: MMC (Maximum Material Condition) adds bonus tolerance to the position as the feature departs from its smallest size (for holes). This means if a clearance hole is drilled slightly larger, its position tolerance automatically increases, reducing cost. It’s appropriate for all clearance holes for fasteners.
Q4: How do I choose the right datums for my CNC part?
Answer: Choose datums that are large, flat, machined, and accessible. The primary datum should be the face that rests on the fixture. The secondary should be a long edge. The tertiary should be a point or short edge. All must be features the machinist can touch off on or probe in the first setup.
Q5: Can a CMM measure True Position correctly?
Answer: Yes, a CMM is the standard instrument for measuring True Position. It probes the feature, establishes the datum reference frame mathematically, and calculates the radial deviation from the true position. For MMC callouts, the CMM also measures the feature size and computes the available bonus tolerance.
Q6: What is the most common GD&T mistake on CNC part drawings?
Answer: The most common mistake is using ± tolerances where True Position is functionally appropriate, or selecting datums that aren’t machinable in the intended setup. Both lead to parts that measure in spec but don’t assemble correctly.
Q7: Do I need to specify True Position on threaded holes?
Answer: Yes, if the location of the threaded hole is critical to assembly. Typically, True Position is specified for threaded holes with MMC or RFS, following the fixed-fastener or floating-fastener formula to determine the tolerance value.
Q8: How does Baosheng’s DFM review handle GD&T?
Answer: Our manual DFM review includes a specific GD&T check: we verify datum accessibility, check for conflicting or redundant callouts, confirm MMC/LMC/RFS appropriateness, and ensure inspectability. This catches GD&T issues before machining, saving rework and scrap costs.
Continue Reading
- DFM Analysis: Why Automated Software Can’t Replace a Machinist’s Eye
- The Engineer’s Guide to 5-Axis CNC Machining: When to Use It & When to Avoid It
- Designing Undercuts for CNC Machining: A Practical Guide for Mechanical Engineers
- How to Achieve a Mirror Finish on 6061 Aluminum Without Secondary Polishing
