What is True Position?

True position is a GD&T symbol that defines the permissible variation of a feature’s location from its “ideal” position.

True Position Calculator

The calculator will check if you pass the True Position test. It features these options:

  • Calculator with MMC (Maximum material conditions).
  • Calculator with LMC (Least material conditions).
  • Consideration of the bonus tolerance.
  • Color indication: Green – the actual position is within the allowed tolerance. Red – the actual position is outside the permitted range.

True Position Formula

Parameters:

True Position formulas parameters
  • TP – True Position. Maximum allowed positional deviation.
  • C – Material condition: None, MMC or LMC.
  • A0, B0 Theoretical required feature’s position.
  • D0 Nominal diameter of the feature.
  • T – Features tolerance.
  • A1,B1 Measured position.
  • D1 – Measured diameter.
  • P – Position. The actual’s feature position.

True position formula (without MMC/LMC)

\( \large P = 2*\sqrt{\left ( A_0-A_1 \right )^{2}\,+\,\left ( B_0-B_1 \right )^{2}} \)
\( \small P = 2*\sqrt{\left ( A_0-A_1 \right )^{2}\,+\,\left ( B_0-B_1 \right )^{2}} \)

If P<=TP Then the feature is within the permissible position envelope. If P>TP Then the position is nonconforming.

True position formula for with MMC/LMC

The formulas are straightforward. However, it is a tricky calculation since it is easy to get confused with the signs (Plus/Minus)

Step 1 – Obtain the position deviation P from the above formula (True position without MMC/LMC)

Step 2 – Obtain the Material Condition (MC) from the below table depending on your feature and condition types.

Feature MMC LMC
SHAFT MC = D0 - T MC = D0 + T
BORE MC = D0 + T MC = D0 - T

Step 3 – Obtain the Bonus Tolerance (BT) from the below table depending on your feature and condition types.

Feature MMC LMC
SHAFT BT = MC - D1 BT = D1 - MC
BORE BT = D1 - MC BT = MC - D1

Step 4 – Get the new TP with the Bonus tolerance TP = TP + BT

If P<=TP Then the feature is within the permissible position envelope. If P>TP Then the position is nonconforming.

True Position Definition

True position is a GD&T symbol that defines the permissible variation of a feature’s location from its “ideal” position.

Feature:  Typically a hole, shaft, slot, or keyway. Holes are the most popular feature where True position is used with.

Position: Distance in X and Y from a datum.

True position GD&T symbol and notation 

True Poistion
  1. True Position GD&T symbol: It means that all the proceeding symbols and numbers correspond to a true position tolerance.
  2. Diameter Symbol: If present, it Indicates that the feature and tolerance are diametrical. True position is most often used on holes and, therefore, will include the diameter symbol. In such a case, the position deviation is multiplied by two. (see formula). If the feature is a slot, then this symbol will be omitted.
  3. True Position Toleance: The maximum allowed deviation from the theoretical position.
  4. Material condition: If a material condition is indicated, you can add a Bonus tolerance to the allowed deviation (3). (True position is typically paired with MMC)
    1. M – MMC – Maximum Material Condition.
    2. L – LMC – Least Material Condition.
    3. Omitted – No material condition.
  5. Datum: The datum plane (or axis) from which the position is measured.

True Position with MMC (Maximum Material Condition).

What is Maximum Material Condition?

Maximum Material Condition (MMC) is a GD&T symbol indicating the maximum or minimum allowed tolerance of a feature where it has the maximum amount of material (volume/size).

  • In a hole/bore, MMC = Minimum allowed diameter according to the tolerance.
  • In a Shaft/pin, MMC = Maximum allowed diameter according to the tolerance.

Combining true position with MMC is very powerful. It means that the maximum allowed position deviation (3) is considered where the feature’s size is at its maximum material condition. As the difference between the feature’s measured size and its MMC grows, you use a bigger tolerance on the position. This additional tolerance range is called Bonus Tolerance. (see example below).

What is Bonus Tolerance?

Bonus tolerance increases the allowed position deviation (3) due to the feature’s size relative to its maximum material condition. The minimum bonus tolerance is zero, and the maximum is the tolerance field of the feature’s size. 

Bonus Tolerance Example:

  • Let’s look at a bore of 1/4″ +/- 0.004″ with the below true position callout of 0.002″
  • The MMC is 0.25-0.004=0.246″
  • If the actual bore measures 0.252, the bonus tolerance is 0.252-0.246=0.006″
  • The original position deviation of 0.002 can be increased to 0.008″.

True Position Example

Without MMC (Dimensions in Inches)

True Poistion example without MMC

Actual measurements on the part:

  • Hole diamrter: 0.252″
  • A position: 2.001″
  • B position: 0.998″

The Position deviation is:

\( \large 2*\sqrt{\left ( 2-2.001 \right )^{2}\,+\,\left ( 1-0.998 \right )^{2}} = \textbf{0.0045} \)

Since 0.0045 > 0.002, the part is nonconforming.

With MMC (Dimensions in Inches)

True Poistion example with MMC

Actual measurements on the part:

  • Hole diamrter: 0.252″
  • A position: 2.001″
  • B position: 0.998″

The Position deviation is:

\( \large 2*\sqrt{\left ( 2-2.001 \right )^{2}\,+\,\left ( 1-0.998 \right )^{2}} = \textbf{0.0045} \)

Because of the maximum material condition callout, we can add a bonus tolerance:

\( \large MMC= 0.25 – 0.004 = 0.246\)
\( \large BT = 0.252 – 0.246 = 0.006\)
\( \text {Hence, the new permisable True Position is:}\)
\( \large TP = 0.002 + 0.006 = \textbf{0.008}\)

Since 0.0045 < 0.008, the part is OK.

Scroll to Top