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.
July 27th, 2010 at 4:21 pm
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.
January 3rd, 2012 at 8:42 am
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?
January 4th, 2012 at 12:10 am
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.
February 16th, 2012 at 7:35 am
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?”
March 13th, 2012 at 1:20 pm
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.
March 27th, 2012 at 12:11 pm
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.
July 14th, 2012 at 5:10 am
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
July 15th, 2012 at 7:05 pm
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.
August 13th, 2012 at 3:50 pm
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.
March 14th, 2013 at 4:46 am
Rite. If i may be allowed to post my interpretation and enquiry for some feedback and advice.
Datum A sets the back of the part as the first reference surface. The larger hole (9.0-9.8) is then defined and positioned via dimensioning distanced from 2 edges. We then come to the definition of its axis (i.e orientation (tip/tilt) by having the Perpendicular Callout with reference to Datum A. We then set the axis (orientation) of this larger hole as Datum B.
That done, we then have the smaller hole (5.6-6.0) defined. Its vertical position is defined and tolerated at 10 +/- 0.5. That leave us with the horizontal position tolerance, which is defined at the main linear dimension of 42, with the horizontal positional tolerance of 0.8 to Datum B. That leave us with the control of its orientation.
This is the part that i need to seek clarification on. How is a positional control of 0.8 to datum A able to serve to control the orientation for this hole? Isn’t it repeating the same mistake that the article explained?
Thanks,
Ian
April 3rd, 2013 at 12:54 pm
Hi Ian — the small hole does have an orientation relationship back to the two datums. It is supposed to be perpendicular to datum A and parallel to datum B.
However, because there is no diameter symbol in that position feature control frame, the orientation is not fully controlled by the GD&T; it’s only controlled in the direction toward and away from datum B. In other words, the tilt of that small hole’s axis in the left/right direction is controlled by the position tolerance (it’s a 3-dimensional zone of two parallel planes), but in the up/down direction the GD&T would never catch that tilt.
April 24th, 2013 at 8:30 pm
Wow, I had wondered about that from the first time I was immersed in the world of ANSI Y14.5 over 20 years ago. It always seemed to me that Datum B (in this example) need only have the perpendicularity constraint applied. This article indicates that is, in fact, true.
A few questions though: If I didn’t care too much about the distance between the two holes but wanted to control the parallelism of their axes, does it make sense to use the perpendicularity/position approach shown in the example (which I’m inclined to do) or is it “more correct” just call out parallelism to Datum B? Also, would the distance remain basic?
April 26th, 2013 at 1:59 pm
First, if parallelism is all that is desired between the holes, then the position symbol must be avoided. This is for the same reason given in the article: anytime the position symbol is invoked, there must be a “distance” that the GD&T speaks to. (In your case, there is no distance to control, but only an angle.)
So the left-hand hole should have the perpendicularity symbol, and the right-hand hole would actually use the angularity symbol, because that would control parallelism to B (per your request) but don’t forget that datum A is still in the picture. That isn’t parallel, but rather perpendicular. So angularity would serve as the miscellaneous angle control to both datums.
For your last question … if parallelism is all that is desired, then the distance between them must not be basic.
May 13th, 2013 at 10:33 pm
Hi John,
Thanks for your reply.
I do understand that by having the small hole position controlled to datum B, it infers its left-right orientation control from datum B as well. That leaves us with the up-down orientation unrestained, like you mentioned.
what i would like to find out is the intent for the positional control of 0.8 to datum A for the smaller hole. If it was to control its perpendicularity to datum A, shouldnt it be a separate callout of perpendicularity?
My thanks for your time once again.
Thanks,
Ian
May 14th, 2013 at 3:13 pm
Well yes, if the intent is really to keep the small hole perpendicular to datum A, then a separate callout for perpendicularity to A, with a diameter symbol, would be correct.
But keep in mind that datums are referenced not necessarily for direct control, but in order to establish a datum reference frame — with an order of precedence to be maintained. So for the small hole shown above, the main objective is to control the straight-across distance from the datum B. Yet we want that to be measured while the entire piece is flattened against datum A. (If we scrapped datum A from the small hole’s callout, then datum B would be primary, and force us to simulate that datum differently.)
So think about datums as telling us how to grab onto the part, even if the main objective is only to measure one aspect of that hole.
I hope that doesn’t muddy the waters further… feel free to ask again if clarification is needed.