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
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
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
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 Ø.3434
hole to the Ø.4379 Datum -A- hole, it can move .008 radially where
it enters the Ø.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.
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
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
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
Thanks for the quick response. If and when it gets included in the
standard, we'll implement it in our engine.
Datum Shift at LMC
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
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
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
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
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
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
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
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
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 126.96.36.199.
Readers: Y14.5 M-1994 paragraph 188.8.131.52 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
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
D8 DUAL DIMENSIONING
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.