Here is a sample lesson from our GD&T Basics Fundamentals Course. We explain why it is much better to use a Position tolerance and Basic Dimensions over locating your feature with a coordinate dimension system.
Position is one of the most useful and most complex of all the symbols in GD&T. The two methods of using Position discussed on this page will be RFS or Regardless of Feature Size and under a material condition (Maximum Material Condition or Least Material Condition). However, since this is such a useful symbol, we will continue to add content and examples for other uses of this nifty little symbol in the coming months.
True Position is actually just referred to as Position in the ASME Standard. Many people refer to the symbol as "True" Position, although this would be slightly incorrect. The Position tolerance is the GD&T symbol and tolerance of location. The True Position is the exact coordinate, or location defined by basic dimensions or other means that represents the nominal value. In other words, the GD&T "Position" Tolerance is how far your features location can vary from its "True Position".
Although incorrect, we title this page and may sometimes refer to the symbol as True Position since this is typically the term people are referencing when they are looking for the specified tolerance. However, if you want to be correct to the ASME standard, just use the term "Position".
Position is defined as the total permissible variation that a feature can have from its "true" position. Depending on how it is called out, true position can mean several different things. It can be used with Max Material Condition(MMC), Least Material Condition (LMC), projected tolerances, and tangent planes. It may apply to any feature of size (Feature with physical dimensions like a hole, slot, boss or tab) and control the central elements of these size features. In these examples, we will use holes, since these are the most common types of features controlled by true position. Position can be used on any feature of size (but not on surfaces where we would use Profile).
Position is probably the most widely used symbol in GD&T. If you are looking for more information about Position or any of the other symbols, you should check out our GD&T Fundamentals Course. If you like the simplified approach to GD&T on this website and in the video above, be sure to contact us to learn more about the course!
Position used with Maximum Material Condition becomes a very useful control. True position with a features of size can control the location, orientation and the size of the feature all at once. MMC true position is helpful for creating functional gauges that can be used to quickly insert into the part see if everything is within spec. While true position on its own controls where the reference point locations need to lie, true position in MMC for a hole sets a minimum size and positional location of the hole to maintain functional control. It does this by allowing a bonus tolerance to be added to the part. As a part gets closer to the MMC, the constraints become tighter and the hole must be closer to its position. But, if the hole is a bit larger (but still in spec), it can stray from its true position further and still allow proper function (like a bolt passing though).
A 2 dimensional cylindrical zone or, more commonly a 3-Dimensional cylinder, centered at the true position location referenced by the datums.
The cylindrical tolerance zone would extend though the thickness of the part if this is a hole. For the 3-dimensional tolerance zone existing in a hole, the entire hole's axis would need to be located within this cylinder.
True position of a feature is made by first determining the current referenced point and then comparing that to any datum surfaces to determine how far off this true center the feature is. It is simplified like a dimensional tolerance but can be applied to a diameter tolerance zone instead of simple X-Y coordinates. This is done on a CMM or other measurement devices.
Locations of the gauge pins or holes are given on the drawing as basic dimensions. All gauge features should be located in the datum true positions, but sized according to the formulas above.
When a functional gauge is used for True Position, any difference the actual feature size is from the maximum material condition would be a bonus tolerance. The bonus tolerance for position then increases as the part gets closer to LMC. The goal of a maximum material condition callout is to ensure that when the part is in its worst tolerances, the True Position and size of the hole/pin will always assemble together. For instance, if you had a large hole size but was still in tolerance (closer to LMC), you make more bonus tolerance for yourself making the true position tolerance larger. You can now have the hole center more out of position due to the bonus tolerance.
Bonus Tolerance = Difference between MMC & Actual condition.
Confused? No worries! For more detail on how bonus tolerances play into these callouts, see our sections on Maximum Material Condition. Or check out our GD&T Course, where we go into deep detail on the position symbol!
True position is closely related to symmetry and concentricity as they both require the location of features to be controlled. However, True position is more versatile since it can be called on a feature of size or combined with other geometric tolerances to specify an entire part envelope.
True position with used of MMC or LMC is related to axis perpendicularity when used on a hole or pin. The tolerance of both perpendicularity and true position now refers to the uniformity and cylindrical envelope of a central axis. However with true position you can make the tolerance referenced to several datum's as opposed to just one with axis perpendicularity. When you callout true position using datums on the face, and sides of the part – perpendicularity is controlled as well. See example 2 for more details.
In example 1 you can see how a hole can be called out using true position. However this can also be applied to anything in need of a location tolerance, such as a pin, a boss or even an edge of a part. When you have a hole in a part such as a bolted surface, true position is usually called out. It can be used almost anywhere to represent any feature of size.
True position of a feature of size under MMC is used when a functional gauge is ideal for checking the part. True position is also useful for describing and controlling a bolt pattern for a pipe fitting or a bolted fixture. If you specify the control using MMC, it allows you to have a pin gauge that you can insert into the part to see if the bolt pattern is functionally accurate. You will see true position called with MMC very commonly in bolt patterns where relative location of all the bolts and necessary clearance is critical. LMC with true position is a little less common, but often used when minimum wall thickness is desired.
Four holes are to be located on a block to ensure contact is always maintained and located within a specific position. The holes need to line up with the threaded connections in the mating part.
With true position called out the holes do not need to be in exact positions as shown below, but their centers can vary by the amount specified by the tolerance. The basic dimensions (dimensions in the squares) are un-toleranced and describe the true location the hole would be in if it was perfect. In a 2D check of the upper right hole, the true location would be 40 mm from datum A and 40 mm from datum B. The holes center is calculated, usually by a CMM and compared to the true location. As long as the holes center is in the blue tolerance zone of 0.2 mm specified by the feature control frame, the part is in tolerance.
Note: in this case, the surface of the part is called out (Datum C). This means the entire hole must have its axis align with the datum. The tolerance zone would actually ensure that the location and the perpendicularity is within the specified tolerance. Since all the central points at any cross section are controlled by true position, the parts axis (line between all central points) would be controlled for orientation.
The biggest thing to note about this design is that no matter what size hole you have, your true position would always have to be the same. This is ideal for when proper exact alignment is required for function of the part. It does, however, remove the possibility of using a functional gauge.
Taking the same example, the true position can also be specified with a maximum material condition callout. This means you are now controlling the envelope of the entire hole feature, including the size of the hole throughout its entire depth.
Adding the little "M" makes a big difference.
With an MMC callout you now can use a functional gauge to measure this part, to determine that the size and geometric tolerancing are within spec at the same time.
This would be the go gauge that would measure for hole size, orientation and position. The part would be pressed down onto the gauge and if it fits the part is in specification. Notice that datum A, B and C are all included in the gauge to check the location of the hole. The desired function of the part is met by ensuring that the part touches all the datums, and that the gauge pins are able to fully go through the holes.
As long as the gauge can go into the part, it is in spec. This makes it very easy to accurately gauge the part right on a production line. The function of the part is confirmed because as long as the surface that the part is bolted to has the same tolerances, it will always fit.
Remember the further you are from MMC when it is referenced in the feature control frame, the more bonus tolerance you are allowed. For a hole, the larger the diameter, (closer to the LMC) the more bonus tolerance you have for your true position.
Note: Keep in mind the opposite is true for a positive feature like a pin, where the smaller the pin means you have more bonus tolerance.
There are two ways true position can be called out – either as a distance, in X and Y or most commonly as a diameter. When true position is called out as a distance, you are permitted to move from the tolerance in X or Y direction by the allowed tolerance. However when done this way, the tolerance zone actually forms a square. This is usually undesirable since in the corners of the square are further from the center than the sides. This also removed over 57% of your tolerance zone! Most commonly, true position with reference to location is called with the diameter (Ø) symbol to be called as a cylindrical or circular tolerance zone.
Another common way true position can be called out is with slotted features. If you have a slot in your part that must always be located correctly, you can use true position to ensure that each of the planes that make up the slot are always located in the correct position. Symmetry can also be used in this case – but only if the slots have a referenced datum plane that they are symmetrical about (and measuring symmetry is very difficult!).
True position on the drawing doesn't have any datums. What does it mean?
Typically, in the vast majority of instances a position control always requires the use of at least one datum. The only exception to this rule is if the drawing is trying to control the co-axial relationship between two separated diameters. Think of a wooden rolling pin, like you might find in the kitchen. If you wanted to ensure that the two handles of the pin were maintained, within a certain degree, were aligned on the same axis you could specify a positional tolerance with no datums. This is somewhat of a more rare circumstance, but it does come up. The only place it's mentioned is in the ASME Y14.5 – 2009 spec in Figure 7-59.
If your situation is anything different than what I've described then your drawing is in error and needs further refinement. Come back and contribute further to the community knowledge base.
We cover this topic and many others in our GD&T Advanced Course. Visit our website course listings for additional information.
This is a quick an easy one. If the diameter symbol is present then it indicates that the tolerance zone is a diameter and the control is applied to a cylindrical feature of size (like a hole). If the symbol is absent then the tolerance zone is the space between two parallel planes and the control is applied to a non-circular feature of size (like a tab or slot).
Hope this helps. We have excellent content that goes over topics like this and many more in our GD&T Basics – Fundamentals Course. It's an in depth self paced course that many of our customers have found to be immensely helpful.
Does true position of a cylinder refer to the location of a single point on the axis or the entire axis. If it is the entire axis how would you calculate it. I've always seen TP as a two dimensional control but we have a blueprint with TP called out on a diagonal hole and I don't think our CMM is computing it correctly.
I can't help you with the CMM, but I can help clarify your understanding of position. The tolerance zone applies to the entire axis along the entire thickness of the feature. For a cylindrical feature you are defining a tolerance zone of x diameter relative to datums A, B, C etc. The entire axis of the cylinder must lie entirely within this tolerance zone for the part to be considered acceptable. This includes the combined effects of translation (x, y translation) and orientation (feature tilt). Additionally, ever two point measurement of the feature must be within size for the part to be correct.
I hope this clarifies things. If now, feel free to come back and ask additional questions.
Shall we provide the positional tolerance with diameter symbol?
It depends, is what you're trying to control a cylindrical feature of size (internal or external)? If it is, then yes. Otherwise no. Consider taking our GD&T Basics course. Plenty to learn.
Doe the pin Gage is machined with same position tolerance or at worst case of position tolerances?
The rule of thumb from ASME Y14.43 is 10% or less of the feature tolerance should be used for the gage tolerance. I strongly encourage you to reference the spec I mentioned. We also address functional gage design in one of our lessons in our GD&T Basics – Advanced Course.
I hope this helps, cheers.
We are grateful to have so many people using our website each day to learn more about GD&T. We would love to hear your anecdotes or experience using GD&T as well as address any suggestions or feedback about the content on this page.
We do not answer questions about GD&T interpretation or application in the comment section. However, if you are getting stuck with how to apply or interpret GD&T, be sure to check out our GD&T Training Program. Our courses come with our GD&T Forum where our ASME Senior-Certified Experts can directly help you work through all of your interpretation or application issues. Thanks again for using the #1 GD&T online resource!