Close Window


Written, with help from students and clients,  by James D. Meadows
The Tolerancing Newsletter February, 2008

Subject: Profiled surface used as a Datum feature

I have taught GD&T from your text and work book for several years now, and have been thoroughly pleased with the results we see. Before choosing your text, I used Lowell Foster's books, because I originally learned from him back in the 70's. I particularly like your new 2007 text and the way you have reorganized the material.

I've been called in to "referee" in the following discussion and would like your interpretation. Please refer to the attached power point slides and .pdf drawing.

We are in the midst of a discussion with a supplier regarding the effects of specifying a tertiary datum for a flight canard profile. The 4 canards are stored inside a control housing, and are deployed after launch, rotating on a pin and stopping with the leading edge at a predetermined angle relative to the rocket axis. Control surface contours are critical, and the supplier uses profile control extensively.

Datum G is the canard center plane, derived from a relatively small feature. Datum J is the axis of pin hole on which the canard rotates, and Datum plane H is the plane of the trailing edge of the canard. The subject of discussion is the effect of eliminating reference to datum H as a tertiary datum in sections L-L, N-N, and R-R.
Profile of a line is used in these section views because the cross section thickness is not constant.

Our supplier is asking permission to remove the tertiary datum H reference from the profile callout in these sections because the datum feature is a plane that is governed by bilateral profile of a surface control. Their GD&T leader believes that including datum H results in loss of one-half of the profile tolerance of that surface. He bases his discussion/interpretation on your September 2006 newsletter in which you discuss use of profile where the datum feature is part of the profile control that references it.

I believe that in our situation it is necessary to specify the tertiary datum feature to ensure that the profile measurements are made perpendicular to the trailing edge plane. Without the tertiary datum feature, rotation is not stopped, and design intent is not completely conveyed. Have I gone off the deep end?


Thanks in advance for your input.


Your supplier would have been correct had datum H been used as a location datum and surface H had been part of what was being toleranced by the profile control.

However, in this instance, it appears as though datum H is strictly being used as an "angular orientation" datum to control rotation of the profile tolerance zone. The profile control is located from datums J (an axis/2 planes) and G (a centerplane). Since J and G were used in the feature control frame prior to H, they form a three plane datum reference system. By the time H is referenced in that control, the plane it creates can only "clock" the three planes that already exist. Therefore, H can remain in the profile control without sacrificing half of the tolerance zone.

Hope this helps,

Subject: Virtual condition

Hi Jim,


I attended a GD&T class you taught at the Sunnyvale, Ca. Westinghouse Marine division about 20 years ago (now Northrop Grumman). I still use the study material you provided to "present my case" from time to time. Well, I am unsure of the correct interpretation as it relates to a functional gage per the attached print callout. My questions are as follows:
1. Should the lower .001 TP tolerance be a composite callout to control radial movement?
2. If a functional gage is used to inspect the .001 TP of the .3434 hole to the .4379 Datum -A- hole, it can move .008 radially where it enters the .3434 - .3439 hole. Is it acceptable to use a functional gage when the referenced feature is not adjacent (4.00 inches away in this case)?

Your help is very much appreciated.


1. It appears from the illustration that there is only one hole being controlled here. Composite tolerancing is used to control the holes within a pattern more tightly in their relationship to one another than in their locational relationship to the datums.

On the other hand, if you are referring to the 8 hole pattern using Composite tolerancing to tighten their relationship to one another (and any angular relationships to datums), while keeping a looser relationship to the datums for location, then that would be fine.

2. A functional gage can be used to inspect the position of features to datums no matter how far they are from one another.

If I've misunderstood your question, feel free to try again.

Subject: Locus???


I have had some inquiries about something called Locus, as it applies to GD&T. Such as Inner and Outer and Negative Locus.

This is a term I am unaware of and haven't been able to search/find anything about it. Do you know what this is and is there a book or literature somewhere explaining it? Is it related to ASME Y14.5 somehow?

Thanks for your support.



I've attached a page from one of my books on GD&T. It should clear up the meaning of locus for you. If you have the yellow textbook, there is more information around the same page as I've attached. This is a term that ASME adopted from JEDEC. I've not heard of the term "Negative" locus. It must be specifically a JEDEC or someone just coined the term and is using it for a common situation they've encountered.

Hope this helps.

Subject: Simultaneous requirements and orientation tolerances


We have a company evaluating our tolerance analysis engine and they say that simultaneous requirements can be used in conjunction with orientation tolerances (they implied that another expert who shall not be named) holds this opinion as well). They also state that not only is it supported, it is required per the Y14.5 standard.

This is something we've never considered. Our interpretation when reading the verbiage is that it only applies to tolerances of location. Can you shed some light on this issue? You're input, as always, would be most appreciated.

Hope things are going well,



Yes, you are correct. We discussed this in the Y14.5.1 committee years before their unnamed expert ever showed up on the scene. The words in Y14.5 only include features that are located to the same datums (to form a simultaneous requirement). Orientation isn't even mentioned in the passage.

Many think it should be. I agree. It should include multiple features oriented to the same datums. But, at this point in our history, it doesn't.

For those readers not familiar with the Simultaneous Requirement rule from ASME Y14.5, it says, When two or more features or patterns of features are located by basic dimensions related to common datum features referenced in the same order of precedence and at the same material condition, as applicable, they are considered a composite pattern with the geometric tolerances applied simultaneously.


Thanks for the quick response. If and when it gets included in the standard, we'll implement it in our engine.



Subject: Datum Shift at LMC

Hello Jim;

I was wondering if you could help me out with a problem.

At work we were trying to calculate a tolerance stack up issue, when we bumped into this Feature Control Frame, that places displacement allowed by datum features (datum shift, **I wasn't sure which words to use**), with Least material condition.

If we understand the meaning of this datum shift, then it means that your gauge will be at LMC and while your cylinder goes away from this condition it won't fit in your Gauge. Or so you subtract tolerance, which we didn't think you could.

Now we checked the ASME standard but it only makes reference to datum shift at MMC, and no indication of not being allowed at LMC.
So our question is: Is it considered obvious that you can't use datum shift at LMC, or how would you apply it at LMC?

If your question is, "What would the gage look like?" No physical gage can be constructed to measure geometric tolerances that are referenced at LMC. Any gage would have to be constructed within a software program, the part scanned and compared to the gage. This would be to see if the surface of the part violated the boundaries constructed by the LMC of F (whatever that is) and the outer boundary of the hole which is a diameter of 1.209.

These could also be measured with a CMM to determine violation of the tolerance zone (a diameter of .005 at LMC to a diameter of .015 at MMC) Datum shift would be allowed as datum feature F departs from its LMC (but since F is given as a reference dimension, this amount of shift is not calculable from the information shown).


Thanks for answering so quickly.

Our question was: Is Displacement allowed by datum features at LMC?
Since we could only find datum shift references at MMC (even in the Y14.5 standard), and no examples at LMC. We had considered it was not allowed.
Also, as you said no physical gage can be constructed, so thinking from a gage perspective we thought it was not possible to add datum shift.
And we had figured that the more you move away from LMC, you would be restricting the position and not adding datum shift, subtracting tolerance (which didn't make any sense).

So if Datum shift is allowed do we add tolerance just like if it were applied at MMC, but from LMC to MMC?
Thanks for your time.


Yes, you would add the datum shift just as you would if it was applied at MMC, but it is gained as datum feature F departs from its LMC.

Subject: GD&T question on relating threaded features


I have a question about how to control the internal and external threads on the attached part so as to control the two pitch diameters to be concentric to each other within a 0.02 MM zone over the length of the part. I am designing a differential adjustment mechanism and if the internal thread axis has much run out in relation to the external thread axis, the mechanism will bind or give a non-uniform adjustment.

I discussed this with the other engineers/designers here and no one has offered a solution. I attempted to apply some datum structure and controls to the part before the threads are cut, assuming that the tap will follow the pilot hole, but don't see how it will be inspected, nor do I want to constrain the machinist more than necessary in his approach. I imagine this part will have the external thread single point machined on the lathe, then have the internal pilot bore produced, then have the internal thread cut with a cutting tap. Thread start orientation is not important, only the pitch diameters having their axis close to coincident.

If you are able to shed some reason on my dilemma, I would be grateful.



It seems to me that you have one good choice with small tolerances and one good choice that will be larger tolerances, but harder to measure.

1. Make the 5.08 diameter datum feature A and position both threaded features to A to within 0.01. That means that the threaded features will be related to one another to within the sum of their tolerances to datum A (0.02). The tolerances are smaller with this approach than with approach 2 below, but give a stable datum feature to measure from (but only if the 5.08 diameter is long enough to stabilize the part). This could be measured with a variety of measurement techniques. Using MMC symbols after both position tolerances and after the datum feature referenced would invoke the SIMULTANEOUS REQUIREMENT rule and allow you to build a gage that would inspect the part's three diameters at the same time.

2. Make one of the threaded features datum feature A and position the other one to it to within 0.02. For threaded features the position control and the datum feature automatically relate to the pitch diameter. Using this approach, the tolerances will be larger (0.02 instead of 0.01), but harder to measure without a gage (or at least a fixture). This method would actually be quite easy to measure if one of the threaded features was positioned to the other with the position tolerance referenced at MMC and the datum feature referenced at MMC. Then a functional gage could be built to screw onto the O.D. with an attachment that screwed into the I.D. It wouldn't give you variables data, but would give you attribute data and be a great way to determine if the part functions.

Hope this helps.


Thanks for your help. We chose the second scheme and look forward to seeing how high the quotes are on the parts.


Subject: Dimension requirement question

Mr. Meadows,

I have a question regarding symmetry on drawings.

If a drawing has symmetry indicated by the datum (as shown in the attached drawing), should features be dimensioned from the outside edge (datum surfaces), or can they be dimensioned from a center feature (if one exists)? Additionally, if there were an even number of holes in the below example say two), could they be dimensioned only from each other and be sufficiently defined? If so, is the below drawing fully dimensioned?

Your input in this would be appreciated.



The drawing is complete as it is. If features are to be held "symmetrical", they are not dimensioned for distance to outside edges.

If they are toleranced with position from the center plane of the datum feature (in this case, the widths), they are dimensioned from the center of the width.

If the distance is zero, no dimension is required from that center plane, since it is implied.

If a symmetry symbol was used, the feature would be assumed to be in the center of the datum or datums established, therefore no dimension is required, just a symmetry tolerance.

If there was an even number of holes centered about a center plane and given a position tolerance, no dimension from center is required. A center to center distance for the holes would be sufficient. However, a distance from the center plane datum would also be allowed either instead of the hole to hole distance or (if you don't mind a little redundancy) it can be included in addition to the hole to hole distance.

If the holes are asymmetrical about a datum center plane, then (in addition to a position tolerance) a distance from the datum center plane for each hole would be required.

Hope this helps,

Subject: Dual dimensions

Hi Jim,

I'm trying to help someone out who has a question about displaying dual basic dimensions. Is there a way this is supposed to be done? I don't even see dual dimensions being referenced in the standard. The only thing I see that comes close is paragraph


Readers: Y14.5 M-1994 paragraph states: Combination SI (Metric) and U.S. Customary Linear Units. Where some inch dimensions are shown on a millimeter-dimensioned drawing, the abbreviation IN. shall follow the inch values. Where some millimeter dimensions are shown on an inch-dimensioned drawing, the symbol mm shall follow the millimeter values.


In previous Y14.5 standards, dual dimensions and dual geometric tolerances were allowed. For example in ANSI Y14.5M-1982 Appendix D-Former Practices it is discussed. So, that would mean that prior to 1982, this was an acceptable practice. What it said in Y14.5M-1982 was:

Dual dimensioning is a procedure where both U.S. customary (inch) units and SI (metric) units of measurement are shown on the same engineering drawing. Two methods were recommended to distinguish the U.S. customary unit from the SI unit-either the position method or the bracket method. See Figs. D6 and D7. Each method allowed an option for the interchange in placement of these units from that displayed in these figures, provided the drawing note explained how inch and millimeter dimensions were so identified. Dual dimensioning is no longer featured in this Standard.

Hope this helps.

Close Window