I have to apologize for this newsletter being late. I had one ready
for July, but my hard drive crashed and I lost everything. Iíve
begun to back up everything I have. Too bad I didnít start that a
bit sooner. At any rate, here is the latest. Please watch for my new
textbook entitled, Geometric Dimensioning and Tolerancing in 2007.
It is the most comprehensive book Iíve ever written on the topic. It
should be ready for sale in November.
Subject: Greeting and some words from China
Dear Mr. Meadows,
This is Jietong Lin, a Ph.D. of Nanyang Technological University (NTU).
I am a citizen of P. R. China, and now I have been working for
Delphi China, an automobile components and systems supplier, for two
years. My PhD major is about tolerancing, and I have read your
books, Applications and Techniques for Use in Design, Manufacturing,
and Inspection as well as MEASUREMENT OF GEOMETRIC TOLERANCES IN
MANUFACTURING, three times when I was pursuing my Ph.D. degree in
Singapore. I have learned a lot from them, and really respect your
knowledge in the GD&T area.
In addition, I am continuing to concern your E-newsletters on your
webpage. Today, I surprisingly found a letter between you and
Mr. Not Eating
I guess that you have not yet visited China, have you? There are
some misunderstandings on the conditions in China, I think. It is
rare that in China, in the recent past years, a manager will be shot
just as there are some quality issues in his/her products as far as
I am not sure if you are interested to know more about China. If
yes, I believe the best way is to have a look at it by your own
eyes. Anyway, welcome to China when you are convenient, and I am
willing to guide you, if possible.
Of course, you are right. I was given the story of the shooting many
years ago by a military officer while working on a project for
Lockheed. The newsletters are all written from emails that I receive
or conversations that I have with people from companies all over the
world. The opinions are only those of the writer.
I apologize if China has been incorrectly characterized in the
newsletter. Many Americans find it difficult to comprehend cultures
that are different than their own. Foods from other nations are
often one of the most difficult things to get used to, and many find
the topic amusing and easy to relate to, since many Americans are
traveling to other countries in their work now.
I think what I am seeing these days is fear that the United States
is giving up their manufacturing base to other countries such as
China, and Americans are worried that we won't be able to sustain
our economy without it.
I agree with those who think that if we don't manufacture anything,
eventually we won't have any jobs or the money to purchase the
things we now take for granted.
We can't blame China for this though. It is our own fault.
Businesses simply want the most cost effective workforce, so they
take their manufacturing to countries where these workforces exist.
Thank you for writing and for reading my books. I have just
completed another textbook that covers a wide variety of tolerancing
topics. It is very flattering to me to know that someone who has
achieved the level of success that you have, has read my books. If I
am ever invited to work in China, I will seek your guidance as to
the most interesting sights to see there.
I wish you continued success and prosperity.
Subject: Question about Datum Feature Symbol Alignment
Hello Mr. Meadows.
I have a question regarding Fig. 6-28 in your textbook. I was told
that Datum A can be placed anywhere along the cylindrical edge of
the diameter .500 cylinder instead of being aligned to the
dimension. Is that true? Iím looking forward to your reply.
Yes, it is true. Since this feature is a diameter, it will generate
a datum axis. It doesn't matter where the datum feature symbol is
placed on the diameter.
One reason I usually try to associate the datum feature symbol with
the dimension (often as an extension of the dimension line, or
aligned with the dimension line) is to show it is the entire feature
of size that is the datum feature. It makes no difference with a
diameter, since it always generates an axis. But if the feature of
size was a width, instead of a diameter (see page 123 for an
example), it would make a big difference where the datum feature
symbol was shown.
On a width, if the datum feature symbol is aligned with the
dimension line, the datum plane is a centerplane (in the middle of
the width). The features being located from that centerplane datum
would be measured from the centerplane of the width.
But if the datum feature symbol was moved off of the dimension line,
the datum feature would just be the one side of the width and
generate a datum plane from the high points of just that one
surface. Basic dimensions would then generate from the plane which
exists at that surface and would lead you to the holes being
What we try to do when measuring anything from an axis or a
centerplane is make certain people reading the drawing don't get
confused and think that they are just measuring from the edge. That
is why we usually associate the datum feature symbol with the
dimension in these situations.
But, the person was correct that with diameters there is no
difference in the interpretation whether the datum feature symbol is
aligned with the dimension or not aligned with it.
Hope this helps,
Thank you for such a quick reply. I wanted to hear this from the
ultimate authority. Really appreciate your guidance.
Subject: RE: Profile vs. Vector
Can you help me understand the following? On a Drawing the Profile
tolerance is 0.5mm.and the CMM inspection report has X, Y, & Z
values all less than 0.5mm. but the V=.534 (Vector). Is the part
good, because Profile is under 0.5.mm. (Drawing Requirement Profile
is 0.5mm.) or is it considered out of print because Vector Value is
over 0.5mm? Can you help me understand why the V (Vector) is even
considered for Profile? I know X, Y, Z would be Spherical Dia .from
Jim, how do these relate. Or are they two separate requirements? How
do I explain the inspection report?
The Drawing is undimensioned Math Data. All I have is the Inspection
report at this time. The Engineer is asking from this report is a
V=0.534 for an undimensioned drawing (CAD Math Data was supplied
with a 0.5 Surface Profile requirement.) The X, Y, & Z values are
all under 0.5. The X, Y, & Z values were given in a Charted Table on
a separate sheet. I hope you may be able to give a partial answer or
guess to the Engineers question.
Well, there are two factors to consider. 1) Is the profile tolerance
an equal bilateral tolerance of plus and minus 0.25. If so, how has
the deviation from the basic dimensions been reported? Has it been
reported as a total of 0.534, compared to 0.5, or has it been
reported as a radius of .534 vs. a total of 0.5? Apples to apples or
half an apple vs. a whole apple. And, if the tolerance is
unilateral, that would be a whole different set of circumstances to
But, I think it is more likely that your problem lies with number 2)
the fact that they think the value of the vector somehow exceeds the
tolerance on the X,Y and Z basic dimensions shown. In short, the
hypotenuse of the deviation from the basic dimensions may exceed the
tolerance allowed. It is similar to when a dimensional deviation
from a true position on a hole is given as 0.5 in one direction and
0.5 in the other, but the hypotenuse of the triangle created
surpasses the allowed diameter positional tolerance of 0.5, because
of the Pythagorean Theorem.
Without seeing the drawing, I'm just shooting from the hip here.
But, it's the best I can do under the circumstances.
Thank you Jim,
Subject: Re: Profile using MMC
Here are two similar Dimensioned parts (see attached)-one with
Profile using MMC callouts and one without. My understanding is that
Profile of a Surface is always RFS and No Bonus Tol., but what about
MMC when used in the Datum Feature Control callout? There still is
No Bonus Tol., with Profile even when used with MMC in the DFC box.
Then what is the difference between the callouts? No SEP. REQT.?
What would be the difference in the Checking Fixture/ Gauge? Are
they the same? Pins will be virtual size in both? Please set me
straight on this issue-Company uses this callout on many of their
Formed parts. I think one reason they do this is because the vender
thinks there is Bonus allowed for Datum Features with MMC. Any
advantages one over the other? Shift? Your comments will be
appreciated. Back of plate is Datum A. Second Attachment is actual
Drawing to use Profile callout.
When the maximum material condition symbol is used after datum
features of size, like holes B and C in your drawing, it means that
the profile tolerance zone remains the same size (in this case
.010), but can shift by an amount equal to the location datum
feature's growth from its virtual condition (of .400 for B). The
profile zone can also receive an additional rotation from the
angular orientation datum feature's (in this case C) growth from its
virtual condition (.500).
Any out of perpendicularity of these datum features will negate a
portion of this profile tolerance zone shift (movement) or rotation.
The gage pins representing the datum features would be a diameter of
.400 for datum feature B and a diameter of .500 for datum feature C.
The example that doesn't use the MMC symbol after datum features B
and C is denied any potential shift/movement or rotation of the
profile tolerance zone (since RFS is implied). The .010 profile zone
would remain fixed in its location and rotational relationships to
datums B and C. The gage pins that represent B and C would ideally
be expanding gage pins that lock into the holes regardless of their
Sometimes on very thin parts, these are
represented with tapered gage pins. The result is similar and only
becomes a problem if the part being gaged is thick enough that out
of perpendicularity of the datum feature holes reaps a different
result than expanding gage pins would have.
Hope this helps.
Subject: Profile with Tangent Plane
I took your GD&T course several years ago. I have a question: I am
working with a component that has a feature that slides through it.
I am trying to control the width so that the feature that slides is
not binding inside the envelope. I had released it using the profile
callout. See attachment # 1.
The supplier had called me back after understanding the ultimate
goal of the component and suggested to use profile callout with a
"tangent" plane (The T with a circle around it). See attachment # 2.
I was not aware or familiar with this callout so I looked in your
book and noticed that it is only mentioned on one page (page 312).
It seems to me, and I could be reading it wrong, that it is only a
unilateral callout. Can you help clarify this callout for me a
little better? Thank you so much,
Page 312 from textbook: Tangent Plane Parallelism
First of all, it looks like the profile control on both
illustrations is hanging on the 39 millimeter basic dimension,
instead of the surface opposite datum B or C, depending on which
drawing I look at. I take it that it was meant to apply to just the
one surface in each case, so it needs to be up against an extension
line of that surface or have a leader line out of the profile
control that terminates in an arrowhead that points at that surface.
Unless you want the profile control to apply to both surfaces that
are opposite of one another. If that's the case, then you should
have two leader lines coming from the one profile control and
pointing to both surfaces (one to each side of the part). Either
way, you don't hang the profile control on the 39 millimeter basic
Your regular profile control says the entire surface must reside
within the profile tolerance zone, which controls its shape
(flatness, if it's meant to be flat). The tolerance zone would be
equal bilateral, unless you showed a phantom line that said it was
But if you used a tangent plane control, it would then say that the
tangent plane of this surface (or surfaces) must reside within the
tolerance zone. It would act as a location and orientation control
for the tangent plane of the surface. It would not control the form
of that surface. Regular profile controls always control the shape
of a surface. But, of course, tangent plane controls never do.
Tangent plane controls are usually used on orientation controls, but
there is no rule against using them on a profile control. It's just
unusual. Profile has the advantage for you of being capable of
location. You just have to ask yourself what you want to locate. The
tangent plane (a plane that touches the surface at its 3 highest
points) or the entire surface (which would control its shape).
Either way, its easy to deduce what the part would fit inside of.
Either way, if you apply the profile control to one surface, the
part would fit inside of an envelope that is the basic dimension of
39 millimeters plus half of the profile tolerance. Whether it's a
tangent plane control or a regular surface profile control, the
tolerance zone is split at the 39 millimeter dimension.
If you apply the control to both surfaces that create the 39
millimeter dimension, it eliminates the need to use one surface as a
datum feature that is referenced in the profile control (whether
it's a regular profile control or a tangent plane control). Once
that datum feature is taken out of the profile control, then, the
part would fit within an envelope of 39 millimeters plus half the
profile tolerance that applies to the left side of the part plus
half the profile tolerance that applies to the right side of the
part. In other words, 39 plus the entire profile tolerance.
If you applied the profile tolerance to both the left and right side
of the part, but kept the datum reference which is one of those
sides, the part would fit into an envelope that is 39 millimeters
plus half the profile tolerance only. This is because you would form
the datum plane for B (or C depending on which illustration) by its
highest points of contact. The datum feature would lose half of its
profile tolerance on that side of the part. It would lose all of its
growth tolerance on the datum feature side.
Hope this helps.
I do not mean to go back and forth with this but it sounds like what
I have, which is attachment # 2(newest release), is what I want. I
just need to point the profile tolerance onto the surface to be
controlled, not the dimension. And yes, you are correct that I want
Datum C to be there and only measure the other side.
This is my second question that I have asked you and you have really
helped out a lot. I really appreciate you still answering questions
after taking a class of yours. Taking your class has been one of the
best things I have done for my career.
Subject: Functional gage
I have a question about functional gages.
Let's say I have a boss(shaft) and it is .200+/-.020, positioned
within a diameter of .030 at LMC to datums A B & C, located
I want to design a functional gage. The gage is going to pick up on
A(3 highest points) B(2 highest points) and C(1 point) and gage the
boss. I will make the hole in the gage at .290 minus, say, .0002 so
the hole is .290/.2898 dia and I will position that to it's datum's
within a dia of .003, basically. So, now I have toleranced the gage
properly according to what was said in the feature control frame. I
have chosen to use a small tolerance on the hole size on the gage
because I deem it important to me.
I set the part on the gage and the boss is at it's least material
condition, being .180 dia. It scraps against the side of the hole in
the gage(.2900/.2898 dia) and slides all the way down engaged the
total length of the part. Because it went into the gage ok--this
tells me I have a good part. I have checked for size and found out
it measures .180 dia on the button for its entire length. This would
be sheer luck and I am using this just as an example.
The centerline of the .180 dia boss is now at .055 from the nominal
basic centerline according to the part print. I only get .030 dia at
the boss' least material condition. I would seem to be off by .040,
which is equal to the total size tolerance.
If I keep my wits about me, I would think I have a "bad" part, but
the gage accepted it. I am confused on whether I have a good or bad
Can you help me in my confusion?
Functional gages can only be designed to inspect geometric
tolerances that are referenced at maximum material condition, not
least material condition.
Should I use a CMM to measure it?
Yes, a CMM would do nicely. LMC controls are very hard to measure,
in general. They change the MMC envelope to an LMC envelope which
resides within the material and makes it impossible to use a GO gage
to measure LMC and incorrect to use it to measure MMC. Then, it
makes it impossible to create a Functional gage to measure the
virtual condition boundary, because that "constant" boundary is the
outer boundary of the hole, which can't be measured with a receiver
gage. So, if you are determined to use the LMC symbol, be prepared
for a measurement nightmare.
I reckon that was a good question I asked. I have learned something
Subject: Books on G D&T for the Automotive industry
Dear Mr. Meadows,
I am a senior manager in an IT consulting company and am responsible
for CAD/CAM/CAE services that we provide. I happened to browse your
website and understand that you are an authority in GD&T. I would
like to know whether any of your works addresses the stringent GD&T
requirements for the automotive industry. Could you refer any book
or CD that I could purchase that would address this specific area?
I thank you in advance for your guidance here.
Although no books only address GD&T for a single industry, I have
been the GD&T trainer for Daimler/Chrysler Quality Institute for the
last 15 years and my books have many examples from that industry. We
use my two books on Geometric Dimensioning and Tolerancing for the
courses we conduct there. On my website you will see illustrations
of all my books. The two books we use for GD&T at Daimler/Chrysler
Quality Institute are the yellow textbook and its accompanying
yellow workbook. The workbook especially has many examples of
automobile parts. These two books are coordinated. Chapters in each
book are numbered the same, so that (for example) Chapter 6 in the
textbook explains concepts of how to tolerance sheet metal
automobile panels and Chapter 6 in the workbook shows many examples
of automobile panels as they are correctly toleranced.
We also have a DVD series of a live workshop that was conducted over
a period of 4 days using exactly the same set of books. It is the 12
DVD set that is explained on my website. Together these training
aids/reference materials should be enough to take anyone from a
novice level of knowledge to an advanced level of GD&T knowledge on
any product, but especially on automobile parts and assemblies.
Since I began as a journeyman die maker at Chrysler Corporation,
many of the examples in my books are from the automobile industry.
You will find examples from not only Daimler/Chrysler, but also many
examples from General Motors and Ford and other automobile
I hope this helps.
If you wish to discuss this further, please contact my office and
speak to Jeannie Winchell (my associate), since I will be traveling
for the next 5 weeks.
James D. Meadows
Many thanks for your detailed response. Let me go through the
examples that you referred to Ė I think by your description, your
books and DVDís seem to be what I am looking for.
Is there a number that I can call if I want to talk to Jeannie?
Thanks once again and best regards. Have a nice journey!
Subject: Composite Profile GD&T question - thin parts
Under Y14.5 the composite profile tolerance can be used to control
size, form, and position.
We create parts from thin materials (<.020) that are laminated and
molded to a final shape. Often these thin sheets have oddly shaped
holes or profiles. (See attached simplified example.)
Since the edge of the material can not really be measured, is it
really appropriate to use a profile of surface as opposed to profile
of line? These parts are cut by CNC laser or waterjet, so we also
include notes like "UNLESS OTHER SPECIFIED, ALL CAD DATA ARE
Your thoughts are appreciated.
I don't think it matters whether you use composite profile of a line
or composite profile of a surface. Because the part is so thin,
either will give you the same results. It's kind of like expanding
the part in your mind until you can see it has thickness. But, since
it is so thin, you can only check one line element, pretty much no
matter what measurement tool you use..
However, having said that, your use of composite profile of a line
is incorrect. In composite profile or composite position
tolerancing, any datum features referenced in the lower level
control must have already been used in the upper level control and
must be used in the same order. You have left datum feature A out of
the upper level control, but referenced it in the lower level
control. That is illegal.
If it was me, I would use the profile of a surface control you sent,
just as it appears. It is correct and recognizes that even though
the part is thin, it still is a surface.
Hope this helps,
Thanks for the input. Profile of a surface it is...
Subject: Drawing Interpretation
Iíve sent you this drawing to review its GD&T content for
The approach you have used is one that works. It has a couple of
problems. If datum features are referenced at MMC in position or
profile controls, the datum features need to be geometrically
toleranced. Without B being completely toleranced with a size and a
tolerance on that size and a geometric tolerance relating B to A, we
can't reference B as a secondary datum feature at MMC, because we
won't know the virtual condition of B to A. To do tolerance stack-up
analysis and to be able to properly represent B in gages or
fixtures, it must (if referenced at MMC) have a virtual condition
that is evident on the drawing. Without B being completely
toleranced, we won't know at what size it is to be represented in
gages, fixtures or tolerance analysis.
The same is true for datum feature C. In order to reference it as a
tertiary datum feature at MMC, it must be dimensioned and toleranced
for size and also have a geometric tolerance that relates it to A
and B. That way we can calculate the virtual condition of C to A and
B. Then we can properly do a tolerance analysis or create gages or
fixtures and know what size C is to be represented at.
You have chosen to profile the pipe. That is OK, as I said. At some
companies that remains the preferred practice. At other companies,
it is preferred to use the positional boundary concept on all pipes,
hoses and tubes. The attachment is just such an illustration from
the textbook that I am currently finishing.
Hope this helps,
Copyright 2006 by James D. Meadows
Thanks for your response and comments.
I have sent your books to our Costa Rica office for review and
possible training courses there for our engineering and production
Subject: Re: Floating or fixed fastener?
With a Dowel pin going into a hole in an assembly that will be taken
apart to build products, do I treat the Pin and hole as a floating
or fixed faster application. I assume using projected tolerance zone
It is treated as a fixed fastener assembly. Just as the threaded
hole grabs the screw and fixes it into place, one of the parts has a
tight fitting hole that grabs the dowel pin and fixes it into place.
That is the part that has the hole or holes that you apply the
projected tolerance zone to. The key then is that the hole and the
dowel pin it is pressed into, become one. Treat them like a "mounted
shaft". Calculate their virtual condition by adding the MMC of the
dowel pin to the position tolerance applied to its hole (whose
position tolerance is projected through the dowel). Make certain the
hole on the other part has a virtual condition that is compatible
with the "mounted shaft".
So, the (MMC of the hole on the other part minus the position
tolerance on that hole) must not be smaller than the (MMC of the
hole that grabs the screw plus its position tolerance). Or, the
virtual condition of the holes must not be smaller than the virtual
condition of the "mounted shaft" with the projected tolerance zone.
Make sure that projected tolerance zone is only used if the hole is
to have the dowel pressed into it later. If the dowel is actually
shown on the drawing already pressed into the hole on that part,
there is no need to project the tolerance zone, because then you are
applying the position tolerance to the dowel pin. And the dowel
pin's position tolerance already projects through it.
Hope this helps.
Thank you, Jim. That is exactly what I was looking for.
Subject: Re: your book
Hello Mr. Meadows,
I purchased your book Measurement of GD&T in Manufacturing and it is
now a great and informative resource in our arsenal.
Can you help me with a problem Iím having on page 137, figure 5-60?
Is this method not measuring eccentricity, so that you would need to
double the numbers in the four columns (.000, -.004, -.002, -.007)
to obtain the diameter in which they fall? If this were the case,
not only would the .007 result be bad as you state, but also the
.004 radial reading (really, anything over .002 difference in the
Is this correct? Of course, please feel free to call or email me. My
number is below.
Concentricity and How to Measure it (page 137)
The book is correct. You are not recording eccentricity. You are
recording the full indicator movement at 180 degree points on the
surface. You are rotating around a datum axis which is the center.
An example I give is that suppose the part was perfectly round and
perfectly centered. The full indicator movement would be zero. If
the part was moved off center (up) by .001, the indicator would read
plus .001 on the top, but minus .001 on the bottom. The full
indicator movement would be 002, but you would only be off center by
a radius of .001. Therefore, a full indicator movement of .007 would
tell you that you are off center a radius of only .0035.
Thanks for the insight and taking the time to respond. I really
Subject: Primary Datum Question
Here we are, already a question and you've only been gone for a
week. I have excellent feedback from everyone that participated in
the course. They were very impressed and walked away feeling much
more confident. I would recommend you to anyone. I also hope we will
be able to have you back in the future for either gaging and
fixturing or tolerance stack-ups.
To my question, I wish we could have had this print when you were
here. I have attached it so you can see what we are looking at. I
have examples highlighted with text and lines. The first question
that came about was; can we use all 4 bosses as Datum A, I didn't
think it would be feasible. (All 4 bosses contact the engine and are
critical). I would think the bosses in example B would make the best
primary datum, The bosses in example A are stepped which would make
for finding 3 good high points of contact. The question then, in
your opinion, and if you were applying GD&T to this print, based on
the info I gave you revolving around the 4 bosses, which would make
the best Datum A? I appreciate in advance any advice you could give.
First, it would be legal to use any of the options. Functional is
usually the best, unless we can accomplish the same thing and make
the part easier to manufacture and inspect. I understand why you
like option B the best. It would be the easiest to understand and
establish as a datum for measurement. (Option B consists of two
datum target areas that are in the same plane). Stabilization could
be a problem though.
The way you describe it, option C would seem the most functional and
the most stabilizing. It would be a nightmare to figure out where
the datum plane is and in fact would actually eliminate more than
three spatial degrees of freedom and therefore would create more
than one datum plane (it would create the primary and secondary
datum planes). (Option C consists of 4 datum target areas, two at
the same height and angle and the other two at different angles from
the first two and at different heights than one another).
Option A is the least attractive of the three, in that it isn't any
more functional than option B, is harder to measure to, and is less
functional than option C. (Option A consists of two datum target
areas on different heights).
As a designer, I like option C the best. But practicality weighs in
favor of option B. I think if you use option B, then profile the
other two surfaces to datum A (created by option B), that might be
OK. But it really is a judgment call.
To best accomplish option C, you would need a fixture. If you plan
to build a fixture that could properly represent all 4 surfaces as a
datum (A1 through A4), then wrote a clarifying note that says
subsequent datums will act as the origin of measurement for location
and datum A will act only to stabilize and orient the part, that
would work. Without the fixture, it would be difficult for the CMM
to deal with 4 surfaces that are at different angles and are on
different heights to create datum planes from.
It's an interesting problem that I don't have a definitive answer
to. I would worry about option B not being able to stabilize the
part sufficiently and in a functional way. It is certainly the
simplest approach geometrically speaking, but not the most
functional. And, as I said, functional is usually the best. Maybe I
am a designer at heart, because I am leaning toward option C. Even
though it introduces a variety of measurement problems and would
require a note to cancel some of the jobs this particular datum A
would normally get (because of the planes it creates), it creates
the most stability and is the most functional.
Sorry I couldn't be of more help, Scott. It looks like you have a
tough decision to make.
As always your thoughts and logic are most welcomed and it has given
me something to go back to the group with. I do appreciate the time
you took out to review my question and print. Have an enjoyable