Subject: Inner/Outer Boundaries
I recently began working through your Workbook and Answerbook for
Geometric Dimensioning and Tolerancing to start learning the basics
of GD&T. The first problem in the workbook asks to convert
specifications to equal bilateral toleranced dimensions generated by
their inner and outer boundaries. The first specification is a 20
+/- 2 diameter hole with positional 2 at MMC referenced from datums
A, B, and C at RFS.
It seems to me that the inner boundary should be 16 and the outer
boundary should be 24 but the answer shows 16 and 28 respectively. I
do not understand where the (22+6) comes from and I have not been
able to find anyone who can explain this to me. Could you please
clear up this matter for me?
Thank you for your time.
When features of size are referenced at MMC, as they depart from MMC
a bonus tolerance of position is gained. This is to protect the
virtual condition boundary. The virtual condition (inner boundary)
is, as you’ve pointed out, 16. So, the MMC is 18 and 18 is allowed
to move out of position by 2 millimeters. 18 minus 2 is 16. So,
you’ve got to ask yourself, “What if the hole was produced at its
LMC of 22? How out of position would it be allowed to be before the
16 millimeter inner boundary would be violated?” Since the LMC is
22, and 22 is 4 millimeters larger than the 18 millimeter MMC, a 22
millimeter hole would be allowed to be out of position 4 millimeters
more than if it was produced at 18 (MMC). In other words, 18 minus 2
is 16 and 22 minus 6 is 16. So, a 22 millimeter hole is allowed to
be out of position 6, and when 22 and 6 are added (instead of
subtracted), you get 28.
If you think of the 16 millimeter dimension as the size of a gage
pin located at “true position” to A,B and C and an 18 or 22
millimeter hole was produced, all you’d have to do is ask yourself,
“How much could each hole move out of position before hitting the
gage pin?” The answer is 2 millimeters for the 18 millimeter hole
and 6 millimeters for the 22 millimeter hole.
I’m glad you are learning this. It sounds like no one around you
knows the basics of GD&T. Bonus tolerance is one of the first things
one learns. When you get a little more practice, everyone should be
coming to you for the answers.
Subject: Idea Thieves
My boss steals all my ideas and passes them off as his own. He
constantly calls me into his office to ask what I’ve come up with as
solutions to technical problems faced by our company. Once I’ve told
him, he calls a staff meeting, invites his boss and tells everyone
who will listen what a great idea he’s had to quell the storm and
calm the waters. He does this when I’m in the room.
The way he says it, without ever looking
at me, I think he even believes that these ideas are his, once he
steals them from me. Everyone thinks he’s a genius, but he has no
technical knowledge at all. He has a degree in business (probably
business ethics) and has no idea what should be done, other than to
cling to me like a giant sucking creature, draining my ideas like a
like a vampire sucks bags at a blood bank.
The good side to this is that, as long as he’s my boss, I’m in no
danger of being laid off. He gives me a decent raise each time I
come up for review, and he says I’m a reliable worker.
The bad side is that he tells everyone that I’m “task oriented” and
that although I can carry out specific orders once he’s decided what
should be done, I’ve never had an original idea in my life.
As the man warns me, “Times is hard. Jobs are scarce. I’m lucky to
have a job.” But it just grinds me the way a person in his position
can use this to lie, steal and cheat his way to success. I have to
admit that violent thoughts and dreams have begun to dominate my
days and nights. I used to work at the Post Office.
Although, sometimes in life, violence is the answer, in this case,
technology might work against you. It’s just like my old friend Dead
Man told me recently. He said he used to carry a gym bag with a
sawed off shotgun inside, because he just never knew when the urge
to rob a liquor store would strike. But he had to give it up because
there are video surveillance cameras everywhere these days. They’re
outside the store, inside the store and at every stop light. Dead
Man says, “You can’t get away with anything in this electronic age!”
Your boss could have a state-of-the-art
camera in his office recording everything you do. Remember, if you
think ‘Times is hard’ where you are, it’s probably harder in prison.
Subject: Datum Question
I recently purchased your GD&T training course on the 12 DVD's. It
took me the better part of a week to run through the DVD's and I've
now kind of run through the book. I must say that it is a wonderful
course!!! Thank you for all that you put into it. I know that I
would do better going through the actual class live. I've been at
this (GD&T) for a while, actually.
My question is regarding an actual relay that has locating pins,
dowel pins, as well as flat head screws. It's a product that's been
in existence for quite a while. Anyway, regarding the locating pins,
which are the 2 diagonal holes on the 2 mating parts, that is seen
on the left top side of section B-B. I'm wondering what the
difference is when one datum is applied to the 2 holes & when 2
datums is applied, one to each hole.
I was thinking of making the mating planes the primary datums and
then the center planes the secondary and tertiary datums to locate
the locating pin holes and then use the locating holes as a datum to
locate the other holes for the connectors, the guide pins (for the
reeds), and the dielectrics.
[Side note: it has been recommended that one hole on the thin mating
plate should probably be a slot or a larger hole, but this is what
it is now.]
What you’ve described to me sounds like a logical approach. I assume
you mean that the widths of the part in both directions will become
datum features and generate the secondary and tertiary datum center
planes from which you will locate the two cylindrical holes. As you
know, you can’t just put a datum feature symbol on a center plane.
It has to be put on the width which then generates a centerplane. If
you do that, you should consider a feature control frame for the
first width that states its perpendicularity to the primary datum.
Then you should consider a perpendicularity control to tie the
tertiary datum feature width to the primary and secondary datums.
Now, on to the cylindrical holes, which you will position to the
datums discussed above. If you say that the 2 holes are a datum
pattern and are referenced at their maximum material boundary, they
will generate an axis halfway between their virtual condition
boundaries. Think of two gage pins that are sized at the virtual
condition (MMC minus their geometric tolerance). The datum axis of
the two-hole datum feature pattern is halfway between those two gage
If, instead, you make one of the holes a secondary datum feature and
the other hole a tertiary datum feature and then reference the
remaining holes to them in that respect, then supposedly the
secondary datum feature is for location and the tertiary is for
angular orientation (to stop rotation), and the datum axis is at the
center of the secondary datum feature and the orientation (clocking)
of the measurement is generated by the axis of the tertiary datum
hole. But, according to the Y14.5-2009 standard, the gage would be
the same as it would for the 2-hole pattern datum, and that would be
the same as if you called each hole a separate datum feature, but
referenced them in compound (such as D circled M dash E circled M).
The discussion of the “elongated hole vs. the round hole” for the
tertiary datum feature is usually one that occurs when they aren’t
certain manufacturing can hold the appropriate distance between the
two holes and they want a larger positional tolerance for the
tertiary hole’s position tolerance in that direction. It is done
commonly on automobile panels, because they are so large and
flexible it is difficult to hold the position of the tertiary datum
hole. Generally, this isn’t needed for smaller, easier to
manufacture parts. But, if they do that, it makes your decision
easier on which hole locates and which one controls rotation. In
that approach, the secondary round datum hole would be positioned to
the planar datum and the two widths you were discussing. Then the
tertiary elongated hole would be positioned back to the planar datum
for perpendicularity, the round hole for location and maybe one of
the widths to stop rotation. Then, subsequent holes would be
positioned to the planar datum for perpendicularity, the round hole
for location and only the width of the elongated hole for rotation.
Try not to fall into the trap of making the entire elongated hole a
datum feature, since the only degree of spatial freedom you need it
to stop is rotation.
Hope this helps.
Subject: True position question - threaded hole
I’m not sure if you remember me, but you led a training session at
our facility last year.
I was wondering if you could answer a question for me regarding
using True Positioning on a threaded hole. I’ve attached a portion
of the drawing for you to review ( I hope it comes through
properly). This drawing is supposed to be interpreted in accordance
with the 1994 Y14.5 standard.
When we calculate the True Position of the threaded hole, should we
be using the pitch diameter or the minor diameter? Is Bonus
Tolerance applicable to both the pitch diameter and the minor
diameter? Just to clarify, I’m not asking if I can combine any
possible Bonus Tolerance from both the pitch diameter and the minor
diameter, I would just like to know if it could be applied to either
one of them.
These parts are machined from 7050
aluminum. We inspect every part before we send them out for
anodizing and they all pass at that point. The problem that I am
having is that about 20% of our parts are failing final inspection
after plating because one or both of these tapped holes is out of
tolerance by .0001”. I am uncertain of the correct way to check the
true position of a threaded hole. I was taught to use a best fin
gage pin in the minor diameter and our QC department is using a
threaded plug but I do not believe that they are making any
allowance for Bonus Tolerance – if it is applicable. Any insight you
could offer would be greatly appreciated.
Threaded holes derive a negligible, non-quantifiable amount of bonus
tolerance from their pitch diameter. When the threaded holes are
given a geometric tolerance like a positional tolerance that uses a
projected tolerance zone, bonus tolerance is best utilized by using
fixed-sized threaded gage pins that thread into the holes as part of
a functional gage designed to check the position tolerance (or
perpendicularity, angularity or parallelism tolerance) of the
threaded holes. When the threaded holes are measured using the minor
diameter, there is no way to utilize the bonus tolerance, since the
minor diameter of the hole isn’t the functional portion of the
thread that is engaged by the mating screw. In other words, any
bonus tolerance derived from the minor diameter is not functional,
therefore is a mistake functionally (and technically).
It is possible to measure the threaded holes position tolerance with
a projected tolerance zone that uses a fixed size threaded gage pin
when using other measurement techniques, like coordinate measurement
machines, but it is difficult in that the inspector would be
expected to use the clearance between the threaded hole’s pitch
diameter and the threaded gage pin to “wiggle” the threaded gage
pin’s axis into the projected position tolerance zone. That
description is the best one to describe the amount of bonus
tolerance the threaded hole is entitled to.
Hope this helps.
Subject: Symmetrical Parts
Here's what I'm wrestling with that I tried to describe to you
yesterday afternoon. The rectangular bosses need to be in line. I'm
thinking of perhaps Profile for the outline in the detail view. Do I
then use basic dims from cut out to cutout? And what about the 3 to
1 rule you sometimes use when assigning tolerance relationships
between the datum features?
Many very grateful thanks!,
The approach you used seems sound, so far. You worked your way in
from the outside using centerplane datums. Measuring in from the
edges would have worked, if you didn’t have symmetry concerns. Then
you made a two hole pattern a datum feature pattern. That works.
Another approach would have been to just make each hole a different
datum feature and reference them as secondary and tertiary in
The cutouts that are elongated can be positioned, but then there is
the rest of the cutout to deal with. As you point out, you can
control the entire cutout with profile but that means you can’t use
plus and minus dimensions for the size. Basic dimensions would have
to be used for the size and would make it harder to gage and be a
more restrictive control, in that you would then have to use profile
of a surface as the geometric characteristic symbol to tolerance the
basic sizes as well as the orientation and location basic dimensions
between the holes and the datums. If you position them instead of
using profile, plus and minus dimensions can be used to show the
size, and then basic dimensions would be used to locate the center
of the elongated features. So, plus and minus tolerances would apply
to the sizes and the position tolerance(s) would apply to the
orientation and location.
The 3 to 1 rule is just for measurement repeatability. It is often
overridden by fixed and floating fastener formulas and cost
considerations. The rule is one I made up and use to remind me that
the thing you measure from should have the tightest tolerance. It’s
not a rule, just a rule of thumb. If the primary datum feature has a
larger tolerance than your secondary datum feature (which is
measured/related from the primary) then getting repeatable
measurement data is difficult, in that you might be rocking on the
primary datum feature more that the tolerance you are trying to hold
Subject: Maximum Material Boundary (MMB)
How have you been?
I have a question about MMB. It is on the attachment. The first
three examples are OK, but figure 4 looks like an exception to the
rule. I’ve stated the rule I believe is applicable below the title
MMB Modifier Explained.
The applicable MMB is usually the virtual condition to the datum
features that precede the datum feature with the MMB symbol. But, in
fact, that statement, although simple, is incomplete. There are
exceptions that one occasionally runs into. Yours is one of those.
When the datum feature is a pattern, one must first account for the
position of the holes within the pattern to each other. As you
noticed, perpendicularity can't do that. So, you had to revert to
the positional control (which can).
I ran into another strange one when I wrote my gray textbook on page
374 and had to spend page 375 explaining it. One would expect the
applicable MMB to be the one that has the tightest tolerance to the
datum that precedes the one with the MMB symbol. But on that one it
That's why I hate the word "always".
See my exception below.
Since this gage is used to measure the position of the four-hole
pattern, the location of datum feature D is not a factor in the size
of the datum feature simulator’s radii. Therefore, the datum feature
simulator that represents D has radii that are altered by only half
the profile tolerance to A (1 divided by 2 equals 0.5).
If this gage was, instead, used to measure the position of datum
feature D, then the radii on the gage for the datum feature
simulator for D would be altered by half the sum of the profile and
position tolerances (1.4 divided by 2=0.7).
Subject: Noting abbreviations on prints
There is a debate here about abbreviations used on prints. I have
always used lb for pound and in-oz for inch/ounces. We have an
engineer who now wants to use LB for pound and IN-OZ for
inch/ounces. He states the Y14.5M states it should be upper case for
everything except for millimeters (mm). I cannot find it. Is he
correct? Thanks for your assistance.
Y14.38 is the standard on Abbreviations and Acronyms for Use on
Drawings and Related Documents. You can buy a copy at www.asme.org.
Y14.5 says almost nothing on the topic. However, in Y14.5 section
1.5.4 (Combination SI Metric and U.S. Customary Linear Units) it
states: 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
Y14.38 has 130 pages on how to show abbreviations and acronyms on
drawings and in text.
Subject: GD&T Certification Test
I am preparing to take the ASME Senior GD&T certification test
again, having scored in the low seventies earlier.
I have a question regarding purchasing one of your books, in lieu of
attending your course which I would prefer, should I purchase your
Geometric Dimensioning and Tolerancing-Applications, Analysis &
Measurement per the ASME Y14.5 2009 standard or your previous book
that is per the ASME 1994 standard. I understand the test is based
on the 1994 standard which should be used in parallel.
Any suggestions in preparing for the test would be greatly
On my website www.geotolmeadows.com I sell a test and an answer book
that is about three times the size of the one given by ASME. It
would probably be the best supplement to just studying the
Y14.5M-1994 standard. If you want to get one of my books to help you
pass the test, that would be helpful too. Even the books per the
Y14.5-2009 standard state which rules are per Y14.5-1994 and which
rules are per Y14.5-2009 and which rules are per both.
Subject: Question about new profile tolerance
I have purchased Your “NEW Rules” for ASME Y14.5-2009 training
manuals and your book “Geometric Dimensioning and Tolerancing” for
I have found both of them to be very helpful.
I have a question regarding the new Unequal profile tolerance
I understand how it works going around the O.D. of a block.
My question is what happens when the profile is on a pocket in a
Do you treat it like max. material as shown in the attached drawing
Please review the attached drawing and please let me know if figure
#1 or figure #2 is correct.
Your books give an example of a block O.D., but does not show a
I want to be sure I understand it correctly. Thank You for your
The tolerance number that appears after the circled U is the portion
of the profile tolerance that adds material to the part. That means
that cavities/holes/female features are allowed to get smaller by
that amount and shafts/male features are allowed to get bigger by
that amount. This statement now appears in my GD&T books written per
Hope this helps.
Subject: Questions on Runout
I have taken a few of your classes and at this point I’m studying
for the senior level exam. A few people here have already passed the
exam and have consequently made flash cards for the rest of us that
have yet to take it. One of the questions they came back with that
is said to be on the exam is as follows:
“Does runout control straightness?” … this doesn’t specify Circular
or total. After researching I found that circular does not! While
Total does. How is it that they can ask a question on the exam of
Both circular and total runout control straightness of the axis. As
you point out, only total runout controls surface straightness.
Subject: Question on runout
I took your class many years ago when I worked for Bulova back in
the 80's. I have moved on and now am at an aerospace company. I was
wondering if I could ask you a question on interpretation. How is
runout checked when the datum is a perpendicular face, and they want
the bore runout to within .001 to datum A the face.
I hope you can help.
If the primary datum feature is the face and the secondary datum
feature a cylinder, then orient the part perpendicular to the face
and then set-up on the diameter to generate an axis to runout to,
that is created by the minimum circumscribed cylinder about the
secondary cylinder that is also perpendicular to the primary face
plane (created by a minimum of three points of high point contact on
If there is only one datum feature referenced in the runout control
and it is the face, then the control is simply wrong. Runout is to a
Subject: Profile Tolerance inspection using CMM
I'm really enjoying reading all about GD&T in your books. I'm
hoping, one day I can meet you and attend your GD&T class in the
Anyway, I need your help for a better understanding as follows: Our
CMM measured the surface profile and the results are shown below:
X actual = 10.1
Y actual = 20.1
Z actual = 29.8
X deviation = 0.1
Y deviation = 0.1
Z deviation = 0.2
Profile tolerance call out is 0.5
Actual profile tolerance deviation from basic (software generation)
After checking, the software is using the formulae as below:
Profile tolerance deviation from basic= 2 times the square root of
deviations in X˛ + Y˛ + Z˛
Just to confirm, is the above formula generated by our software
correct or wrong? If wrong, what is the correct formula? Thanks
again for your help.
To calculate a point’s deviation from its basic location in space in
terms of a total width or diameter (for an equal bilateral tolerance
zone), the formula is correct. However, there are other ways to
express a profile’s deviation from basic. For example, it could be
expressed as a radial deviation from basic, using the worst case for
the largest plus deviation and the worst case for the largest minus
deviation. The formula would then be the same, but to express each
as a radial deviation, the “2 times” portion of the formula would be
eliminated. This would tell you the direction of the deviation and
the amount of maximum deviation in both the plus and the minus
directions reported separately. Also, if the profile tolerance isn’t
equal-bilateral, but rather unilateral or unequal bilateral, the
formula would not show the deviation from the mean profile, since
the mean profile isn’t shown.
The formula you are using is normally used to calculate the
deviation from true position of the axis (center point) of a sphere.
The software writers for your CMM have apparently used it to find a
profile of a surface deviation of each point on the surface
individually. Again, this would only work if the tolerance of
profile was equal bilateral, and you wanted to express the deviation
as being out an amount that could be directly compared to what is in
the profile feature control frame. This formula is adequate in some
cases, but wouldn’t tell you much about the deviation. For example,
it wouldn’t tell you which way the point has deviated from basic.
Also, to even tell how much it has deviated radially, you’d have to
divide the answer by 2.
By the way, there is an ASME standard numbered Y14.45 currently
being written to show how variables collected data should be
reported. Until it is published, there is no standard rule on the
reporting of measurement data.
Hope this helps,