Position with Only One Datum?

This time around, I’d like to present another “pet peeve” of mine, at least in the world of GD&T.  It involves using the position symbol when the only quality being controlled is perpendicularity.

This is very common — it stems from some subconscious notion that if GD&T is going to be used on a hole, it’s got to be the “true position” symbol.  NO!

Consider the following example. There is a position tolerance applied to the large hole on the left, and the datum being referenced is A.

      

But let’s go to the standard and examine how the geometric control called “position” should be used: ASME Y14.5-2009 (and prior editions)  state that position’s main job is to control location — meaning that it involves a distance — and perpendicularity often comes along as part of that position control.

Since the large hole given above is already distanced from the edges by plus/minus dimensions, the geometric tolerancing has nothing to do with location. The only relationship that the large hole has with datum A is one of orientation. Therefore, an orientation symbol must be used:

Notice the perpendicularity symbol. This is the correct way to identify this hole, since the hole itself now becomes the datum feature for other features to locate back to.

That said, there are no GD&T police that will haul you to jail if you insist on using the position symbol. But recall that the purpose of geometric tolerancing is to use a standardized language to express the design requirements. So it’s best to stick with the proper terms and symbols if you want to minimize confusion when expressing your requirements!

One final footnote — there are times when a position tolerance may reference only one datum: If a pattern of features (two or more) are being positioned with one feature control frame, then a single datum plane is allowed (because there is the location between the two features that position controls).  And another example is that of coaxial features; we may have one diameter positioned to another diameter, and this “coaxiality” is indeed a location control.

45 Comments

  1. Finally!!!!! someone who knows what he’s talking about when it comes to GD & T. I am so sick & tired of engineers using it incorrectly and then using their findings as the basis of rejecting parts.

    • Sorry but GD&T is a langue and it has rules. We spell peace and piece different because they mean something different. If you really knew GD&T you would know the hole needs a basic tolerance and there for has to have a positional. Basics are used when dimensioning to and from theoretical axis, planes, and points. You are probably one of those who thinks you can true position a point too.
      If you chose to use the langue then use it the way it says to. Perpendicularity does not control position. Yes they look to be the same but they are not. We are told true position cover location and perpendicularity does not. Sorry like peace and piece when we talk it does not matter but you cannot say the person knows how to spell. I fell perpendicularity is a modifier. I want a hole located within .010 but it needs to be perpendicular within .005. Stop being ignorant of the langue and learn it.

      • Hello P — I’d have to gently say that you’re barking up a tree that’s not even there.
        You are adamant that “perpendicularity does not control position.” I certainly agree with you! But nowhere did the article claim that perpendicularity controls position.

        There was absolutely no attempt on the second drawing to use GD&T to control the location of the hole. Here’s the key: that left-hand hole creates a datum. So wherever that hole is, its position simply is. (You seem to think that every hole has to have a position tolerance. That’s not true.)
        Now, for a complete definition of the part, a profile tolerance might be added to the outside edges, related back to datums A and B by basic dims. Then we’d still have no location tolerance for the large hole, but everything else would be toleranced relative to the hole.
        So I’ll simply reiterate that the only point of the article was that position is not to be used unless it involves an element of location.
        Thanks for reading the blog!

    • I’m with you bro, tired of seeing this issue with different customers.

  2. I am relativly ‘new’ the the world of GD&T. I use a cnc controlled CMM and two different manual CMMs, with with cnc and manual CMMs having different software. I run into these type of things on print all the time and the people I report to can’t understand why my software will not report the things being specified on the prints. By the way, how do you do true position of a hole with no datum specified?

  3. The only way to use position tolerancing with no datum references is if there are two or more holes involved in the same callout. Then I suppose it’s possible: each hole simply becomes a datum for the other. The only example of this shown in the official GD&T standard is for coaxial (in-line) holes. In that case, they don’t even need to be perpendicular to anything; the only thing desired is to keep them in line with each other. On your CMM, it wouldn’t matter which hole you zero out on first.

  4. A pet peeve of mine is when the (I think) uninformed refer to the position symbol as “true position.” Am I correct in asserting that there is a concept of “true position” as mentioned in 14.5 and a “position symbol?”

  5. Hi Dave … yes, you’ve nailed it. The standard calls the symbol itself “position.” (I believe the symbol was at one time called “true position,” but that’s been several decades!)

    However, the term “true position” still has meaning. It is the theoretically perfect location that is desired. The “position” symbol then tells us how far from true position we may stray.
    It’s not a huge deal, but yes, this is the idea that you were thinking of.

  6. THANKS!

    But I have to add that I dont care if you refrence 15 datums, or a pattern. Say what you mean and mean what you say. Design engineers should use the orientation callout that makes proper sense for manufacturablility. In this and many cases : . PLEASE USE IT! or LEAVE IT OFF THE PRINT!

    Great article.

    • I am also new to this type of work. and I cant seem to understand how an Engineer with all there years of study have not managed to stumble upon and learn some GDnT seeing as they use it on there prints.

      the intention behind GDnT was so that everyone could have a similar language no matter if you spoke mandarin or English we could all read a print using GDnT and understand what the creators intention was.

      So why the fff don’t engineers know this??

  7. for diameter 5.6 you have given position tolerance 0.8 relative to datum A and B.What’s the role for datum A? From where you take reference for datum A to control the position tolerance.Because the hole and datum are in same plane.

    Please help me to clarify

  8. Vinoth — Datum A has two roles. First, it tells everyone that before we lock onto the axis of the large hole (datum B), we must first stabilize the part on that back face. Recall that datums tell us how to “grab onto” the part for fixturing, etc. So even if datum A were to play no quantitative role, it’s still telling us to keep the part primarily flat against that surface before locking onto B. Think of a part where datum feature B is slightly angled; we want to stay flat on A.

    But there is another role for datum B: it controls the perpendicularity of the 5.6 hole, although only in the left-right direction. If that hole tilts, that is another way to use up the position tolerance.

    • vinoth is making a good point. Datum A controls the orientation of the part and the holes must be perpendicular to A. The entrance to the hole could be spot on. The position error at the top is zero. However, because of the orientation of the hole’s axis, the end result of the position would have to be OOT because of the squareness or orientation to A. So, like so many, I don’t like the original position call-out, but it is proper in my opinion.

      • Vinoth asked why datum A was referenced in the callout that used two datums; I think he was OK with datum B(location) but struggling with the purpose of keeping A in there.
        I agree with your premise that orientation is being controlled in both drawings. But here’s the difference: In the first drawing, orientation is the only thing being controlled by GD&T for the left-hand hole. Yet by definition position is a location control (which happens to bring orientation along with it).
        So the thinking is that if position is not even doing its most basic job, then it can’t be used.

        • Hi, I just started learning about GD&T. My biggest issue right now is understanding why some features, such as a hole, in one example will have 3 reference datums, and then in another example a hole will only use 2 or 1 reference datums. For instance, in the 5.6 diameter hole in the above example there is only two reference datums. Why is there not a third C datum? Is it because, in the function of that part, the two holes do not have to be aligned vertically as long as it falls within the +/- tolerence?
          I’d really appreciate some tips on selecting the adequate number of reference datums for features.

          • You are pretty much correct. We only reference the number of datums needed to control what is desired for that feature. In the example above, the 5.6 hole only needs to be controlled for position in the straight-across distance (horizontal) from the larger hole.

            In general, think of it this way: There are six degrees of freedom. Some GD&T callouts need to have all six DOF constrained for proper function. But it’s fine to leave some DOF unconstrained if it doesn’t hamper the function of the part.

  9. ASME Y14.5.1M-1994 Supports not using position on a secondary datum that is a feature of size. We should always remember the mathmatical definitions when dealing with features as datums. Use of position in the example is wrong and not allowed based on the standards.

  10. What happens in the same case…when a hole is held positionally back to a single datum feature that happens to be…YES!….A CYLINDER!!!

    • Yes, Rikk. There are times when a single datum suffices.
      But the post is dealing with cases where the only quality that ends up being controlled is perpendicularity, as mentioned in the first paragraph. So even if that datum feature is a cylinder, if there’s no distance involved then perpendicularity is the symbol to use.

  11. Sorry…I’ve been searching for an answer to my question and every which way I put in my question it keeps directing me here. My situation is a bit different than the post…yes…as it involves a hole being held positionally (reference control frame references only one datum)…back to a cylinder (as datum) that is neither coaxial to the hole nor parallel…cylinder axis runs in X…hole axis is in Z…again sorry…thanks for your time.

    • The cylinder’s axis would control the spatial orientation and zero point for Y and Z, though Y and Z would still be able to freely rotate about axis X. Therefore, you would use perpendicularity to control the orientation of the hole’s axis with respect to Datum Axis X. The hole’s axis could still freely rotate about X, but could not lean toward/away from the axis in a manner which skews the basic 90° angle. So it would be perpendicularity, but only in one axis (X).

  12. Why is the hole true position to the face (datum) A?

    • Hi Jerry — if you’re asking about the difference between the two pictures shown above, the symbol controlling the hole is different. (In an earlier version of this post we had the symbols reversed, but now the graphics have been fixed. Maybe that’s what you are referring to.)

      But in general, when a datum is identified on a print, it’s good design practice to use GD&T to relate it back to the previous datums. So the designer is correct in relating the hole back to datum A (the face), but the only relationship that the hole has to the face is the quality of perpendicularity.
      So you are right — the hole should not be called out for true position to A. The second picture is showing the correct symbol to use.

  13. If datum B is simply a perpendicularity, which I agree with. How does that stop any rotation in the part and allow those basic dimensions to drive a true position in the smaller hole? It looks to me like if you are using B as a secondary datum, you are still leaving a clocking feature out and not fully constraining for that second smaller hole.

    • That’s true for the GD&T part of this drawing, but if we look at the big picture it’s not entirely true. The only relationship being established between the two holes by GD&T is a straight-shot distance. The outside edges of the rectangular part are not part of the datum system, which is what you’ve noticed! In other words, the left-hand hole could be a little up and the right-hand hole could be a little down. But… the position callout could be met perfectly. This might not be wise, but it is legal.

      The only thing that controls that rotation aspect is that both holes have to be within 10 ± 0.5 from the bottom edge. Again, perhaps it’s not wise to mix this type of tolerancing with GD&T, but the main idea about the datum and position is still preserved.

      • Well… you have to give the machinist the general vicinity of the left hole. How else would you convey that other than, the dimension scheme you gave in this example?

  14. Datum C is not required in above case? Datum B is a hole, part may still rotate with respect to Datum B hole axis.

    • Right — a tertiary datum is not needed. The given tolerancing only locates the small hole from the large hole in the horizontal direction. The dimension on the left side (10 mm) controls the vertical direction. (This may not be the best way to control the location of the small hole, but it’s enough to illustrate the point of the article.) Thanks for reading!

  15. hi,

    is it possible to use the positioning tolerance for surfaces?

    (Like: “These surfaces in line within 0.001)

    thanks,
    Richard

    • According to the ASME standard for GD&T, the answer would be no. (Position is only to be used on a feature of size; profile of a surface would be used to accomplish your need.)

      But according to the ISO rules for GD&T (GPS), yes, position can be used on surfaces. So the answer depends on which system is being imposed on the drawing!

  16. I still have a problem with this drawing. Must not the dimensions to the center of the hole axis be basic dimensions and the surfaces from which it is being located be datums?

    • Hi Nicholaus… the distance to the datum(s) must indeed be basic, and in this case that rule is being followed. For the position tolerance on the small hole, notice that there are just two datums referenced. The basic dimension relating that hole to datum A is an implied basic of 90º — per paragraph 1.4(j) of the Y14.5 standard. And the basic dimension relating that hole to datum B is given as 42.
      Your question then seems to be why an edge of the part are not a datum. Well, in this case it may only be desired to control the distance between the holes, not the distance from an edge. That is perfectly legal; it’s not always required to nail down the hole in every possible direction. (The drawing may be incomplete, but the GD&T as given is certainly legal.)
      Also see my reply to Ash above… that was a similar question.
      Thanks for reading the blog!

  17. Hi John,
    Thanks for this post, question for you… what if i add another small hole (with the same diameter) 42 units to the right & 10 units below (the existing small hole), can i add basic 84 & basic 10 units dimensions (from the big hole) and then add “2x” before the 5.6 – 6.0 diameter dim. Is that legal way to control the location of the new hole? and lastly what if i want to control the pattern of the holes can i add another location tolerance frame below the existing one and add tolerance say dia. 0.4 ref datum to “A”?

    • For the first part of your question… yes, you can add those additional basic dims to lay out a new hole to the right (and downward), and then place “2X” before the holes’ diameter. (An aside: based on the looks of this part, that new hole would be off the part! But I get the general idea of your question.)
      However, I would probably then add a diameter symbol before the 0.8 in the feature control frame. This is because you’re no longer just doing a straight shot from big hole to small hole; you’re now controlling several holes. (Think about the datums: you set the part down on A and then plug into datum feature B. The part can still rotate freely, but you are establishing a relationship among the three holes and that’s a bit more that a straight-across distance.)
      And yes to your last question also. An additional position tolerance that references datum A only would have the effect of tightening down the hole-to-hole distance of those two (and their perpendicularity to A, of course).

      • Thanks a lot John, i agree, there should be a diameter symbol before the 0.8 positional tolerance and as well as on the 0.4 for the pattern…

  18. Stop all the confusion by creating a stable datum reference frame. Visualise it like this:- Datum A (the flat surface) Datum B ( a pin perpendicular to A, probably at virtual condition) and Datum C (a pin perpendicular to A and pitched basically to B, again probably at virtual condition). Then control the size, location and orientation of the outside vertical surfaces by using an all-round profile of a surface call out.

    • Gary — I agree. But notice that you used the key word when describing datum feature B: it is perpendicular, and nothing else. That is why the main point of the article was to get people to stop using the position symbol when the only thing you can say about B (in this case) is that it’s perpendicular. Then for a fully detailed print profile could be used for the perimeter, etc.

  19. So if this were a mounting block attached to another part, we could then label the smaller hole datum C and then reference datums A, B, and C for features in the assembly, right? I have a similar situation but with both holes the same diameter. I was going to label datums A, B, and C just like you see here, but the engineer say he wants to call the left hole B, and then create a basic dimension that is tangent to the outside of both holes and call that datum C. Claims he needs an equalizing datum for this to work. I have never, ever seen anything like this! You always reference an axis for hole location, not tangency to the hole. Every GD&T guy at works says this is crazy, but he claims his is the only way to do it. Thoughts?

    • Hmmm…. I too have never seen anything like that. What you wanted to do is much more common. In some industries they would use the terminology “4-way datum” for that datum B hole, and then “2-way datum” for the datum C hole, because its only job is to stop up/down rotation.
      What your colleague wants to do might be possible. But to do that he’d have to use what we call datum targets: use a couple of targets on the top wall of each hole (such as B1 and B2) to create an imaginary line at those two tangent targets. He’d still need a datum C to control left/right movement of the block.

      • It is just a mounting bracket for a component that bolts into a frame. I said it would be even easier now to just group both holes together as datum B and just reference datums A and B for other features. I have no idea why you would reference the outside tangencies of a hole and call that datum C. First time in 30 years of GD&T I ever saw someone do that……

      • It sounds a bit like using the flats on a horizontal slot to control the rotation of the part and become datum c. In my 30+ years of experience, I’ve never seen hole tangencies utilized as a means of defining a datum. You can always ask him to show you what he’s trying to convey and more importantly how he’s going to fixture it for quality inspection.

  20. Thank you for this article!

  21. One item of interest – If the hole defined as datum B is close fit and I want to control perpendicularity but allow this limit to float based on the size of the 9.0-9.8 diameter I would use Position tolerance with a MMC modifier. So in this case if I wanted to allow a larger perpendicularity error than 0.8 with a larger hole I would have to use position tolerance as Perpendicularity does not allow for a MMC modifier. I have done this with very close clearance fits for part position control to allow shop to choose how they want to split up tolerance between hole diameter and perpendicularity. I think I am doing this correctly. In some cases I do this at zero true position with MMC modifier applied.

    • Hi John,
      Even in your case you should still use perpendicularity rather than position. You wrote that “perpendicularity does not allow for a MMC modifier.” But it does allow for it. If you have access to the Y14.5 standard, check out Figs. 6-13 and 6-14, which use the MMC modifier for perp. (But I do like your idea of using zero at MMC!)

      The general rule is that the position symbol should only be used when there is an element of location involved. Otherwise that symbol is missing one of its constitutive elements and we should use a lower-order symbol (perpendicularity).

  22. Dear john,

    Whether the perpendicularity has a basic dimension or ordinate dimension …. If both are there which is sufficient ?

Submit a Comment

Your email address will not be published. Required fields are marked *

*