Links to stuff on this blog

Use the Site Index of Projects page link above for an easier way to find stuff on my blog that you might be looking for!

Sunday, June 26, 2011

GD&T Basic(s) True Position and Tolerances

This post is a very simple explanation of Position as used in Geometric Dimensioning and Tolerancing. Why am I writing about Position? One of the most frequent questions people ask me regarding Geometric Dimensioning and Tolerancing is "what does that target bulls-eye symbol mean". That bulls-eye symbol is called Position and it seems to be the most confusing and mysterious symbols in GD&T for some people. Before I talk about Position you should go back and read - or read if you haven't read already - THIS post that I wrote about tolerances and size and maybe even THIS post I wrote awhile back. There is nothing really mysterious or even complicated about the concept of Position and how it's used with Basic Dimensions in GD&T. The application can get pretty scary and complicated sometimes but the concept is pretty straight forward. I'm going to try and explain it in a overly simple way and later tie all these Design Related posts together as I write more of them.
Square Tolerance Zones
The first thing that is important to point out is that Geometric Dimensioning and Tolerancing is all about the dimensions tolerances so I'm going to compare the 'traditional' method of tolerancing to Position as a starting point. So to start with have a look at a 'traditional' drawing below that uses linear coordinate dimensions. On a 'traditional' drawing that is using linear dimensions the tolerances are put on each of the dimensions either directly as in the picture below or in the title block (or notes) on the drawing. Have a look at the below drawings 2A and 2B that are dimensioned 'traditionally' with the tolerances on the dimensions themselves. I have left the dimensions of the block itself off the drawing for clarity.

Linear Dimensions with a Square Tolerance Zone
In the top view of the above picture (2A above) there is a rectangular block and a couple of dimensions to a point near the middle. Imagine that you want to drill a hole 1.5 inches from the left side and 1 inch from the top as the dimensions show. Note that each dimension has a tolerance of +/-.25 inches so to get the hole in the right spot you first measure down from the top of the block 1 inch +/- .25 inches, giving you a total tolerance of .50 inches. Same thing with the other dimension, measure from the left 1.50 inches +/-.25 inches - again giving you a total tolerance of .5 inches. To get the hole in the right spot according to the dimensions (and the tolerances) you would have to drill the hole so that the center of the hole was somewhere inside that .5 inch square tolerance zone. Does that make sense? It seems strange if you think about it that a round hole would be positioned in a square tolerance zone doesn't it? Read more and this will start to make sense...

So looking at the above drawing 2A again there is a square tolerance zone created by the +/- tolerance on each of the dimensions. The point in the center of the tolerance zone is the Nominal position or the exactly perfect place for the center of the hole. In other words the dimensions are to the nominally perfect point that the hole center can be and the tolerances are showing how far away from that nominally perfect point the center of the hole can be. 
Another way of thinking about this is: The dimensions on a drawing are locating tolerance zones and not the features themselves. Read that last sentence again and keep it in mind because it's a important concept and will be really important soon. So in the picture above the 1.50 and 1.0 dimensions are not dimensioning to the hole they are dimensioning to the tolerance zone that the center of the hole has to be in. It's easy to look at a drawing like the one above and think that the "dimensions are to the hole" but in reality they are not really dimensions to the hole, they are dimensions to the area that the center of the hole can be in. I'm going on and on about this concept because it's important to understand especially later (in future posts) when I'm going to write about more dimensioning concepts.
In 2B of the drawing above you can see the square tolerance zone with a dimension from the nominally perfect point in the center to the corner of the square tolerance zone. That diagonal dimension is .354 inches and that is the worst case position that the center of the hole can be in, or the farthest off nominal that the center of the hole can be and still be OK.
"Really, the hole can be off .354 inches" you ask?
At first glance you might think that the worst case position that the hole can be off from nominal is .25 inches, after all the dimensions are +/- .25 inches, but that isn't the case because the tolerance zone is square shaped. Now have a look at the drawing below of the square tolerance zone that has two possible positions for the center of the hole, both .354 inches from Nominal.

The Pitfalls of Square Tolerance Zones
The drawing above shows the square tolerance zone and a couple dimensions to possible center points for the hole. Notice that the orange .354 dimension to a possible hole center is outside the tolerance zone but the black .354 dimension is just inside it.  The center of the hole can be off Nominal by .354 inches but only if the hole is off diagonally from the nominal point. If the center of the hole is off by .354 either horizontally or vertically then the hole is out of the tolerance zone and the part is considered to be bad. That is a very odd way to dimension hole because the hole is round and it usually doesn't matter which direction a round hole is off from nominal, because the hole is round! A round hole can usually be off a little bit in any direction and still work in the design. If you dimension the drawing with a square tolerance zone you would have to reject all the parts that had holes off by .354 inches unless they were off diagonally. This odd situation is the result caused by the square tolerance zone.
In the picture above I put a bunch of points where you might expect to see the centers of holes if you were to make a bunch of parts and measure the hole centers on all of them. When you mass produce parts you tend to get a Normal Distribution around the nominal position for all the dimensions, those points represent what you might see if you made a bunch of parts and measured to the hole centers on all of them. Using a square tolerance zone would mean that a lot of parts would be rejected and possibly scrapped because the hole centers were outside the square tolerance zone even though the parts would probably work OK.
Round Tolerance Zones
At this point I want to finally talk about Position and what it means in GD&T. In a huge oversimplification I'm going to say that in this example "Position is a round tolerance zone". I'll probably get a lot of emails ( and maybe even nasty comments on this Blog about that last sentence because Position is a lot more than a 'round tolerance zone' but for now in the context of this post, think of Position as a round tolerance zone (it's actually cylindrical in this case but for now just think of it as round). To start this off I've redrawn the above drawing of the block with the hole in it using Position. Have a look at the drawing below and notice all the rectangles with numbers in them. The drawing looks complicated but really it's almost the same drawing as I did above.

Block and Hole Redrawn with a Position Tolerance
(the square tolerance zone is shown for reference only)
In the drawing 2C above I redrew the block and the hole but this time a equivalent Position tolerance is used instead of the square tolerance zone. The first thing that is different between the drawings is the 1.50 inch and 1.00 inch dimensions have boxes around them. When you put a box around a dimension it's called a Basic Dimension and Basic dimensions don't have any tolerance associated with them, they are perfect. Most people freak out at this point and say "you can't have perfect dimensions without tolerances" because nothing can be made perfect. That is true, all dimensions must have tolerances but the tolerances don't necessarily have to be on the dimensions themselves. With basic dimensions the tolerance is someplace else and not on the dimensions.
The concept of having 'perfect' Basic dimensions is not really that different from the +/- toleranced dimensions in the first drawings 2A and 2B above. With the +/- toleranced dimensions the 1.50 and 1.00 dimensions are dimensioning to the Nominally perfect center of the square tolerance zone so they are really perfect right? In the case of Basic dimensions (with the box around them) the 1.00 and 1.50 are dimensioning to the Nominally perfect center of a round tolerance zone and they are perfect too. The same perfect dimensions with just different shaped tolerance zones. The Basic box around the dimensions is really just a reminder telling you that the tolerance isn't associated with the dimension as it was with the +/- dimensions, the tolerances are someplace else.
Have a look again at the 2C drawing above. The 1.50 and the 1.00 Basic dimensions are locating the center of a round tolerance zone that is .708 inches in diameter. The .708 inch diameter tolerance zone is being defined in the rectangular box under the hole diameter with the "target bulls-eye symbol" Position symbol. The rectangular box under the hole dimension is called the Feature Control Frame and just like it's name it is controlling the Position of the feature (in this case the hole). This is a handy way of specifying the location of the hole because the location tolerance for the hole is right next to the hole diameter.
In drawing 2C I drew in the old square tolerance zone for comparison to the new round Position tolerance zone. Notice that the square tolerance zone is circumscribed by the round Position tolerance zone. That is because the .708 inch diameter round tolerance zone is 2X the .354 worst case square tolerance zone hole center location shown in drawing 2B above. Remember in the case of the square tolerance zone the hole could be off nominal by .354 inches only in the diagonal directions and not horizontally or vertically. The .708 inch round tolerance zone allows the center of the hole to be located .354 inches off nominal in any direction! With the position tolerance not only is the round hole being located with a round tolerance zone but if you make a bunch of parts and the hole centers are normally distributed around the nominal 'perfect dimensions' all the parts will be OK and not rejected.

Cylindrical Tolerance Zone with Position

Earlier in this post I said that Position tolerance zones are round but that wasn't exactly correct. Position tolerance zones are actually cylindrical in this case because in the real world parts are 3 dimensional objects. Position tolerance zones can be other shapes too and I'll write about those cases in another post, for simplicity in this case think of Position tolerances as cylindrical.
In the Feature Control Frame below the hole diameter I've added the letter A in it's own box. The letter A in this case is referencing a Datum that is being defined in the lower view of the part. What this means is that the .708 diameter Position tolerance zone is located in relation to Datum A, in this case the flat face of the rectangular block. Have a look at drawing 2D above to see what I mean and note that the round tolerance zone shown in the top view is extending through the entire part perpendicular to the flat surface datum A.
Remember that for the part to be OK the center of the hole has to be inside the tolerance zone. The center of a hole is really the center axis of the hole because the hole is a 3 dimensional feature. Because the Position tolerance is referencing Datum A the cylindrical tolerance zone is Perpendicular to the flat face of the part. What this all means is that the center axis of the hole must be completely inside the cylindrical Position tolerance zone as shown in drawing 2D above. The Position tolerance is controlling not only the location of the center of the hole but also how perpendicular the hole must be to the Datum face A. Isn't Position cool? 
In the drawing 2D above the hole isn't exactly Perpendicular to the face of the part but the center axis is entirely within the tolerance zone so the part is OK. If you wanted the hole to be even more perpendicular to the face of the part (but not change the tolerance zone) you have several options and I'll write about those in another post. For now the important concepts to remember are:
Dimensions on drawing are to tolerance zones and not to the features themselves.
Position tolerance zones are 3 dimensional and the center of whatever they are dimensioning must be entirely within the position tolerance.
Basic dimensions have a box around them and they are perfect, the tolerance for Basic dimensions is someplace else on the drawing.
Square tolerance zones allow things to be farther out from Nominal than the tolerance on the dimensions state because the tolerance zones are square!
This post is a simple explanation of the Geometric Dimensioning and Tolerancing concepts of Basic Dimensions, (True) Position and Datum's. There is a lot more to all these concepts that I didn't cover in this post in the interests of keeping it simple. I intend to elaborate on not only the concepts in this post but the other posts where I wrote about GD&T HERE and HERE and tie them all together. I will also cover other Position concepts as well as  lots of other fun and exciting GD&T stuff!! If you have any questions or see something I might have missed please leave a comment or send me an email at and I'll be happy to get back to you!


  1. Hello sir,
    I have some doubts, 1.what is the major difference between position tolerance and linear tolerance. 2. why people preferred position tolerance instead of linear tolerance? 3.where we use linear tolerance and where we use position tolerance? 4. which symbol we can you position tolerance?

    please sent me the answer to my mail id

  2. To answer your first question... The major difference between linear tolerancing and position tolerancing is you get more tolerance with position than with linear. The square tolerance zone with liner tolerancing is smaller than the circular tolerance zone with position. Position also allows for use of Maximum and Least material conditions which control the position of the feature based on it's size. This can be used to ensure that the parts will fit together.
    The second question about why it is preferred: One reason is it's easier to do tolerance stack ups and calculations.
    The third question about where to use them: There really isn't any hard rules on when to use one or the other. You can even use both on the same drawing. Generally if you want to ensure interchangeability of parts position is the way to go. Also if you want to make functional gauges to check parts position works better.
    The position symbol is the circle with the cross over it.

    For a good overview of GD&T check out the wikipedia link below.

    I'm planning on writing more about GD&T as I get time so check back on my blog. If you have any more questions please let me know and I'll be happy to help if I can.


  3. Still I couldn't understand why this diameter or square tolrance is being used instead of linear tolerance.As par mine both are having same meaning.More specific if suppose my true position is out of diameter tolerance then I will make changes in particular axis whichever is out & after carrection automatically it will correct the true position.Same is with linear tolerances.Then what is difference.
    Pl. clarify my point sir,

  4. Amol Mankar,

    Thanks for the question. In the example above with a round hole it makes more sense to use a round tolerance zone rather than a square one. Using a linear dimension and tolerance as in the first picture above the hole can be 'off nominal' by 0.354" in the diagonal directions only (the corners of the square). If the hole is out 0.354" horizontally or vertically then the part is out of spec.
    Because of this, when designing this part it would be important to make sure that the part still fits if the hole is out worst care position of 0.354" - so one would have to make the hole big enough for proper function at 0.354"
    As the second picture shows that when the part is made in large quantities the locations of the holes measured on many parts would be all around the nominal position in a normal distribution. In this case many of the parts made would have to be rejected because some of the holes are outside the square tolerance zone, BUT those parts are still usable!!
    Using Position and a round tolerance zone of diameter 0.354" all the parts manufactured can be inspected and used.
    That is one of the advantages of using Position, higher yield of parts in mass production.

    I hope that makes sense, if not let me know!

    - Otto Belden

  5. Thanks for ur reply,
    But my point is,can we say linear tolerance & diameter tolerance are same in nature.If it so then why we used diameter position tolerance in many drawings.Is diameter tolerance means True position.

    -Amol Mankar

  6. Amol Mankar,

    A True Position diametrical tolerance is not the same as a linear dimension(s)with tolerance. Linear dimensions with a tolerance result in a tolerance zone that is square. True Position diameter tolerance result in a tolerance zone that is round. It makes so much more sense to use a round tolerance zone on a round hole, and not a square tolerance zone on a round hole doesn't it?

    A diameter symbol on a dimension that is not used with True Position isn't the same as a True Position diameter tolerance. A diameter symbol on a dimension is used for a dimension on a feature that is round. So the dimensions if for the feature, not the tolerance. A diametrical tolerance with True Position can be used with a feature of any shape because the diameter is referring to the features location, and not the features shape.

    - Otto

  7. Otto,

    Thanks for the great write up! I now understand how to use/read True Position tolerance that references a single datum.

    I'm not sure how to interpret True Position tolerances that reference multiple perpendicular datum though. Could you help me?



  8. Nick,

    Thanks for checking out my blog, I'm glad you found some if it useful.
    I'd be happy to explain multiple datum references, email me at:
    and I'll explain the concepts. I'm also in the process of writing a post about that very subject so I'll have info here on my blog at some point as well. In the meantime check out the other GD&T posts I have:

    - Otto

  9. Hi Otto,
    Trying to make a gage for true positional callout of two in-line bores.
    And this is the first time we have come across this... the call out on the part print is "true position diameter 0.000 mmc to datum E at mmc"

    Does this mean the bores have to be perfect with each other?
    And if so, would my "go" plug gage just be made to the minimum bore tolerance of each hole? (1.000/1.004(E)& .5000/.5008)
    Thanks for any advise you could give!

  10. Hello Chad,

    Thanks for the question! If I understand your question (I can't see the drawing)the two bores would have to be perfectly in line when they are both at their MMC conditions. As either bore, or both departs from MMC they could be misaligned by the sum of each bores departure. So if one bore is off MMC by 0.002 and the other by 0.001 they could be out by 0.003
    Having said that a GO gage would have to be at the minimum bore sizes.

    - Otto

  11. Great article! Thanks a lot for the thorough explanation. I had learned about this in a drawing class but needed to refresh my memory.
    One question: are there any standard positional tolerances for bolted or screwed assemblies? What I mean is if I have 2 parts being assembled with 4 1/4inch bolts in a certain pattern, what positional tolerance should I use on each part to ensure they can be assembled properly?
    I assume such a standard would be a function of the bolt size.

    Thanks in advance.

  12. Great article!
    One question: are there standard positional tolerances for bolted assemblies and for screwed assemblies?
    For example, if I have two parts that are to be assembled using 4 1/4" bolts in a certain pattern, what positional tolerance should be used on the position of the hole on each part in order to ensure they can be assembled properly?
    I assume such standards would be a function of bolt size.


    1. yacpro13,

      Yes there are charts and guide lines for fastener patterns that show the True Position tolerances and hole dimensions. I'd be happy to send you a chart if you email me. I'm in the process of making a chart for this blog but it's not done yet. It is a little bit complicated and depends on the application so its just a guideline. Send me an email and I'll send you the chart.

      - otto

  13. Good information with Illustration.
    While converting a linear tolerance band into a Diametric one, why do we not care to use a inscribed circle, since if we are using a tolerance of +/- 0.25mm on both the axis we can as well mention dia 0.5 in the GTol. Now since we are considering the Circumscribed circle, the dia will always be equall to the diagonal length(dia 7.07mm) of the square or rectangular tolerance area. Which by the way is bigger than can be ideally manufactured at the same cost. This point can be good for a supplier with 57% lesser rejection rated (as some training materials state it) but may not be a ideal for design and assembly. Is inscribed circle advised.

    1. Girish,

      It depends on the application. If the feature (like a round hole) that you are dimensioning to will work at the larger tolerance of a circumscribed circle then use that.


  14. Hello Sir,
    What is true position?How to measure it?

  15. Thanks a lot for this great article... This clears a lot to me. And thanks to u, from now I will implement this in my drawings.. Good impression in office too.. ;) Thanks a lott..

    1. Varun,

      I'm glad you found the information here useful. Thanks for checking out my blog!


  16. in the future may we have drawings beside the text so we can readly see what we are reading. Great job on the explanations!!

    1. Anonymous,

      Thanks I'm glad that you like my Blog and find the information useful. I am in the process of moving my Blog to a better host, Blogger (now that Google has taken it over) isn't easy to use or even functional.
      As soon as I find a better place to post I'll provide a link (and more pictures!)

      Thanks again,


  17. Can we create a non draft rib in our part and represent it as our datum?

  18. I have a Question Sir
    I have two options in case of T.P
    1. The value of T.P is preceded with dia symbol
    2. T.P without Dia symbol in the frame
    what is the difference between both of them?