As many of you know, for over twenty years now, I
have used this newsletter as a way of allowing former students,
future students and professionals with different levels of Geometric
Dimensioning and Tolerancing knowledge to write in and ask technical
questions. I believe that those in and interacting with technical
fields such as design, manufacturing, quality and inspection have
the ability to learn to apply and read the language of GD&T. Well,
most of them anyway. There was the time I was trying to teach one
inspector what MMC is. I said, “Look at the size specification on
this shaft. It is given as a limit dimension. There is a big
number and a small number. The MMC of the shaft is the big
number.” He looked at me, then back at the page and said, “The
numbers look the same size to me, Jim.” I thought about that for a
moment, then said, “No, not the type style, the value.”
Question on position:
I hope all is well with you---I am again trying to
get you in here or at least get the engineers to you for your
course. I will persist.
I have a round part with thru holes placed every 60
degrees. The drawing gives a start angle and then a note specifying
the size, with the position callout and the statement: "6 holes
equally spaced". The start angle and B.C. are basic. They want the
start angle to be a +/- tolerance and keep the "equally spaced" note
as basic. I am having trouble with this.
Is this in keeping with the standard?? I have looked
but can't seem to find any examples.
I would prefer to take the start angle off the
drawing and put 6X 60 degrees basic with the note for the holes
pointing to the horizontal axis of the part. The orientation is not
know what you're doing. What they want to do is illegal and beyond
that, it makes no sense. The positional tolerance on these holes is
what tolerances the basic angles of 60 degrees from hole to hole and
the basic distance from hole to hole (and any angles and distances
from the datum or datums). If they give the angle a plus and minus
tolerance and then give the holes a positional tolerance, you would
have competing tolerances trying to do the same job.
you say, keep the angles and the distances basic from hole to hole
and from the datums, then rely on the position tolerance to
tolerance all these basics. If the relationship to the datums is
less important than the relationship from hole to hole, use a
composite positional tolerance.
shown a similar part example from one of my books below.
Diameters as Datum Features:
My name is Joe and I work at a company in Iowa. You gave our
company some in-house training on geometric dimensioning and
tolerancing - level 1 in December of 2001.
I just finished a heated discussion with two of my co-workers
regarding diameters as datums. The issue is when using a diameter
as a datum feature, does the datum feature symbol have to be lined
up with the dimension line? One of my co-workers says yes, the
other vehemently says no, it does not have to be lined up, the
meaning is the same either way. I'm confused.
Please see the attached sketch. Do the two datum feature symbols
mean the same thing?
On page 128 through 130 of your book Geometric Dimensioning and
Tolerancing Applications and Techniques for use in Design,
Manufacturing, and Inspection, you give explanations and examples of
how the symbol is to be applied.
The two arguments go like this:
Argument #1 - since a diameter is a feature of size (and can only be
a feature of size) whether the symbol is lined up with the dimension
line or not is immaterial. The datum feature is the diameter
(surface) and the datum is the axis created by that feature. Also,
the first bullet point on page 129 states that, "...place the datum
feature symbol on...an extension line of the feature outline,
separated from the size dimension. This designates that the datum
is the axis of the cylindrical feature." (emphasis added by me to
“separated by”, not in the text)
Argument #2 - if the symbol is not lined up with the dimension line,
the datum is the surface of the diameter, not the axis. Similar to
the description given on pages 123 through 125 on centerplane datums
for non-features of size. Therefore to denote the axis as the
diameter, the symbol must be lined up with the dimension line.
Can you shed some light on this?
is no difference whatsoever. The surface of a diameter can't become
a datum. Datums are axes or planes (regular planes or centerplanes).
Argument #1 wins. Argument #2 has no merit. Diameters always
generate an axis.
making a diameter a datum feature to generate a datum axis, we do
try to line up the datum feature symbol with the dimension line as a
matter of drafting preference, but to not do so doesn't change the
argument made referencing page 123 and 125 does hold true for widths
and centerplane datums, but not for diameters and the datum axes
Position with a Square Symbol? Measuring Position on Square
- attached is a print that we have marked up with questions, but
is an interesting call-out that I wanted to get your feedback on.
The part has a true position control on a square hole that is a
portion of a star shaped hole and it has a square symbol after the
position symbol and before the positional tolerance of 0.08.
1. Is that correct as to how they drew it?
2. How do you measure it? For example, if you had a CMM what would
Just so you know - I took your gage design course at the UWM
Education which has been a very valuable tool as I do design lots of
attribute gages for our product. I look forward to your feedback.
there is no provision in the Y14.5 standard for using a square
symbol inside of the feature control frame. However, you can create
a square positional tolerance zone for a feature by giving it two
feature control frames. Each position tolerance would point in a
different direction (one in the X direction and one in the Y
direction) and both position controls would reference the same
datums. Still, it is pretty easy to figure out what they wanted to
do, and in tolerancing, clarity is No. 1. In other words, even if
they circumvent the rules, why not give them what they want? They
can always go back and correct the drawing to abide by the Y14.5
rules ASAP. As to how to measure it, technically with a position
control, one should not probe the hole, but instead probe a
substitute for the hole, such as a gage pin. But since that is so
difficult to do, most CMM operators would simply probe the hole and
treat the location tolerance zone as though is was plus or minus
0.04 in both the X and Y directions.
shown a similar example from one of my books below (not a square
zone, but the concept is close). It creates a rectangular tolerance
zone for a round hole. Notice the perpendicularity control prevents
the axis of the hole from leaning across the hypotenuse of the
rectangular positional tolerance zone.
greatly for the quick response. One other question. I have a
drawing that uses perpendicularity on a surface to a datum axis
constructed by two diameters (A-B). Does the call-out for
perpendicularity relating this surface (which later becomes datum
feature C) to this compound datum axis make sense? Let me clarify
what I am asking. If I needed to measure this perpendicularity
control, I would try to hold datum A by some means and then
basically check face runout. The problem I have is they say to
measure from A-B. I have an engineer who says that we need to hold
both A and B simultaneously, and I do not see how that would make
related issue is if you look at the right top detail the face has an
angle to it making it very difficult to check.
the opposite face from C has a callout to A-B, but would it make
more sense to have it be parallel to C instead?
a lot of questions. One at a time. Measuring perpendicularity to a
compound datum axis (A-B) is thought of as a little different than
checking total runout. But the result is that the same geometries
are accepted. Total runout is implied to be measured while chucked
up on the datum diameters and rotating about the datum axis they
generate. Perpendicularity is implied to be measured in a
stationary state while centered on the datum axis generated by both
diameters. Perpendicularity can be measured on a coordinate
measurement machine (CMM). Probing both diameters and asking the
computer to generate a single axis (hopefully from the highest
points probed), then probing the surface or surfaces being
controlled by the perpendicularity characteristic is actually quite
doable. Whether or not it makes sense should be considered from a
functional aspect. If both diameters are used in the assembly to
stabilize the part, then it would seem to make sense.
question about the surface with an angle callout that is difficult
to check seems to be a different issue. But as long as that angle
is needed to complete the part definition, it only makes sense to
dimension and tolerance it. Whether it is easy or difficult to
measure should not be the deciding factor. Our ability to measure
things is only limited by our creativity and our budget, but parts
must be completely defined.
the last question (Should one face have a parallelism control to the
other instead of a perpendicularity control to the same datums?),
one is almost as good as the other. If you go with the parallelism
control on the second face, you accumulate error to the original
compound datum axis (A-B), but have a more direct control to the
first face. If you go with the perpendicularity control, there is
no accumulation of error to the original compound datum axis (A-B),
but there is an accumulation of error to the first face in that the
two faces would be related to one another to within the sum of their
perpendicularity tolerances to the compound datum axis.
Composite Positional Tolerancing
question about composite tolerancing:
have 3 coaxial holes 8.3-8.5, positioned within a diameter of 3mm to
the main datums B & C).
Then I have them set up as a set (composite) with no
datum reference within a diameter of 0.3 (to hold the alignment of
the 3 holes’ axes to each other).
run my numbers to figure the inner & outer boundaries, do I take the
size and add the 0.3 only or do I add the 3 as well.
I know that the 0.3
must remain within the 3.
holes will have two inner and two outer boundaries. One set of
inner and outer boundaries will be based on the collective effects
of the size limits and the 3mm of position tolerance. Completely
separate from that the other set of inner and outer boundaries will
be based on the collective effects of the size limits and the 0.3mm
of position tolerance.
didn't tell me why you are calculating the inner and outer
boundaries, but whatever the reason (tolerance stack-up analysis,
determining worst mating conditions, calculating minimum wall
thickness, etc.), you must determine which set of boundaries is
applicable and then use the appropriate geometric tolerance to find
the unknown you are seeking. The first rule of tolerance stack-up
analysis is to know where you are going to be able to choose the
correct path to get you there.
shown a similar situation from one of my books below.
#1 and Inspection
Given; inspect a part with only size dimensions, no
geometric tolerance. So, checking to Rule #1, you make a two point
inspection to check that the part is within MMC and LMC.
Finally, you check the envelope at MMC. That check is my problem.
The geometric characteristics are indirectly checked by Rule #1, but
how do you check, for example, the outer envelope of a round shaft
without directly checking directly for roundness. Another example,
is cylindricity. Other indirect geometric controls, or all, may
fall into my problem. Help!
I have the impression that inspecting to Rule #1
should be less costly than inspecting to geometric controls. In
general, how do you do this without directly checking
geometrics? Inspecting the envelope at MMC for Rule #1: if high
volume, with hard tooling? Costly? Or, if at low volume, with open
setup? But then, how would you check the envelope at MMC of a
"straight" part without directly checking the geometric control for
purpose of Rule #1 is to have the size tolerance control the form
tolerance. The way size is inspected is to ensure that it controls
form. In fact, size tolerance controlling form tolerance is most
often more restrictive than using a geometric control on a
part. With a geometric control such as cylindricity, one can allow a
shaft or hole to grow or shrink a lot with a large size tolerance,
but be better in its 3-dimensional form by adding a tighter
cylindricity tolerance. Just calling out a tight size tolerance
would control both size and form to within
the tight tolerance.
Measuring a part would require cross-sectional checks for LMC (like
a micrometer check for shafts). Then, an envelope check for MMC
would require (per Rule #1) a GO gage to either be used or
simulated. So, the answer to your question is that geometric
controls don't make the part more expensive. Their goal is to make
the part less expensive, but to still function well.
And, you can't check the envelope of perfect form at
MMC (created by Rule #1) without also checking (on a cylinder) the
cylindricity which controls roundness, straightness and taper.
could always eliminate Rule #1 by a variety of methods including
just writing a note that states, "Perfect form at MMC is not
required." But then, unless you add a geometric control, you will
have no form control at all and the part could look like a banana or
even worse, it could curl completely around on itself.
can do pretty much anything you want to do, but remember that Rule
#1 is in place to allow you to control the size and form to within
the same tolerance. Geometric controls such as cylindricity are
available if you would like to have a smaller form tolerance than
size tolerance. Straightness of the derived median line (axis) is
available to apply to a shaft or hole to eliminate Rule #1 and allow
the feature to be out of straight even at MMC. And as I mentioned,
notes such as "PERFECT FORM AT MMC IS NOT REQUIRED." are available
to say that size and form are entirely independent of one another.
So, just decide what is best for the product, and then set about
creating that situation by what you put on the design drawing and/or
a guy with a bumper sticker that said, “Ask me about GD&T.”
Thinking he might be an expert or at least another interested
practitioner of (G)eometric (D)imensioning and (T)olerancing, I
followed him. Every time I figured he was about to stop, he would
take another dusty side road or go down a dark, garbage strewn
alleyway. Before I knew it, it was midnight and I was 50 miles
outside of civilization. He finally pulled into the parking lot of
a really sleazy-looking joint called “(G)irls, (D)rinks and (T)rouble.”
to think of it, I was right after all---we did have a lot in
common. Still, finding this out took us on a 3-day escapade, most
of which I don’t recall (although I’m fairly certain some firearms
and sirens were involved). Anyway, I am left with the faint
recollections and physical evidence of being (G)ross, (D)isorderly
and (T)attooed. Know any way to have the words “U.S. Amy” removed
from one’s chest? The tattoo artist apparently never won a spelling
problem is that I’ve never known anyone named Amy and, besides, even
if he had gotten that word right, what I seemed unable to remember
at the time was that I was in the Navy---not the Army.
Tattooed and Blue
(D)iscipline and (T)herapy a try. Then, (a) date only women named
Amy or (b) Consider a battleship as a cover-up tattoo.
Tolerance Stack-Up Analysis &
Accumulated Tolerance Error When Multiple Datum Reference Frames are
I recently purchased
your book 'Tolerance Stack-UP Analysis" and have a question related
to exercise 8-5, problem #1 "answer page.
In step 1 you
indicate the following:
+.050 = Geo. tol
.310 dia =
outer boundary of hole
+.130 = pos. tol.
of datum D
Then you add .130
for pattern shift of datum D. This is where I become confused. Can
you please explain to me why you add the .130 as pattern shift after
adding it as positional tolerance of D at LMC. Wouldn't the .130
shown above account for the pattern shift?
I greatly appreciate
your time in explaining this.
the following illustration:
What you have to ask
yourself is, “Would there be a difference if the 4-hole pattern’s
position control did not use the MMC symbol after D?”. When you
switch datum reference frames in mid-part definition, you accumulate
additional tolerances. This analysis recognizes that the datum
feature generating the axis from which other things may be measured
may first experience a movement of its own (from the first datum
reference frame). Then, wherever that axis lands, it then becomes a
new datum axis (D) from which the pattern of holes is measured and
from which that pattern may shift away due to the MMC symbol next to
the datum feature D in the hole pattern's position control.
Think of it as two
gages. One gage measures the location of the first hole (and gets
the .130), then the second gage measures the location of the hole
pattern (and it gets the .130 also). Each gage must represent the
hole from which the .130 comes with a gage pin that is .130 smaller
than the hole may be produced (LMC of .600 minus Virtual Condition
of .470=.130). For a more complete answer with pictures, see the
last newsletter for July/August 2004.
I hope this helps,
for Symmetrical Parts
Mr. James D. Meadows,
recently purchased your book GEOMETRIC DIMENSIONING AND TOLERANCING
Applications and Techniques for Use in Design, Manufacturing, and
(per ASME Y14.5M-1994). Thank you very much for such a good book.
you please answer the question (please see the attachment):
you establish datums on symmetrical part (for instance such as Fig.
15-44 and 15-58 in your book (please see the attachment also), is it
clear for a part inspector which datum surfaces should be
simulated? Since the part is symmetrical, the inspector may choose
any of the four surfaces as a secondary (B) or tertiary (C) datum
feature. Also, the inspector may choose a surface opposite to A
shown on the drawing as a primary datum A. It looks ambiguous to
me. How does the inspector determine the correct datums when all of
them look identical? Is my concern valid?
Thank you very much for your time and consideration. I look forward
to hearing from you.
concern is a valid one. The Y14.5 standard addresses this by
recommending that when this is a concern, the datum feature may be
made distinguishable by physical identification. One way to do this
is to design in a feature such as a notch to make it possible to
tell one surface or width from another. Other ways are for the
manufacturers and inspectors to physically identify the surfaces by
stamping or etching letters into the surface. When I was a die
maker (many, many years ago) I used to carry a crayon or piece of
chalk with which to mark surfaces, so that I would be consistent in
setting up parts to machine or measure.
MMC on Datum
Hi Jim, attached is
a linear guideway drawing that is dimensioned to
communicate to the supplier which holes we will be using to attach
their product. We assemble this part to a machined extrusion with
tapped holes (with the same dimensioning scheme). The clearance
holes are referenced to a datum feature hole at MMC). My question
is regarding the MMC modifier on the Datum A hole. A question came
up in our Quality department regarding how to apply the bonus
tolerance as the Datum A hole departs from MMC.
Do we check the datum A feature size and the holes to be inspected
and add the amount both features depart to get our total position
tolerance zone? OR Does it only allow the hole pattern as a group
to depart from the datum feature axis? I believe that if the holes
were dimensioned to each other as opposed to individually
dimensioned from Datum A, then the bonus tolerance gained from Datum
A hole departure from MMC would only apply to the hole pattern?
(Note: I think I need to change Datum A to be the mounting surface
opposite the counterbore side, Datum B as is - centerline of the
rail width and Datum C to be the hole now noted as Datum A. We will
be making gages for these parts soon.)
Thanks for your help.
The short answer to
your question is that the additional tolerance gained from datum
feature A (by virtue of referencing the pattern of holes to A at MMC)
only allows the hole pattern as a group to depart from the
datum feature axis.
The way the basic
dimensions are depicted on the drawing, whether they are from A
or from one hole to another, has no bearing on this drawing
interpretation. It is the same either way.
The only way the
drawing could be interpreted differently is if each hole was a datum
feature and the next hole was positioned only from the previous hole
(in other words, referenced to the previous hole as its datum).
This would mean each hole would reference a different hole as a
datum feature and the accumulated error would be huge. But if all
holes are referenced from the same datums, located with basic
dimensions, there is no accumulation of error. That is the big
difference between basic dimensions and plus and minus dimensions
for location. When plus and minus tolerance was used (hopefully in
the distant past) for the location of holes dimensioned from each
other, it made for the possibility of horrific accumulated error.
Basic dimensions can be used as vehicles to add or subtract from one
another without accumulated error (as long as the datums aren’t
I like your idea of
making the mounting surface opposite the counterbore a primary datum
feature, then B as secondary and the hole as tertiary.
But let me offer
another suggestion. What if you did not make the hole a datum
feature at all. You could position all 17 holes as a pattern to the
mounting surface as primary, the width (now called B) as secondary
and the left edge as tertiary (making the .295 from that edge a
basic dimension) within a diameter of .100 at MMC. Then you could
refine that with another segment of position (below) that referenced
all 17 holes (to each other-which is always toleranced by the
tightest position tolerance anyway) to within a diameter of .0065 at
MMC and reference the mounting surface as primary and the width B as
secondary. This would allow all 17 holes to move left or right (in
the view you sent me) plus or minus .050 (a diameter of .100), but
keep their position tolerance to each other and the mounting surface
and the width B all to within a diameter of .0065 at MMC. Both
levels of position would use their own position symbol. This is
called a Two-Single-Segment Position control. Just a suggestion.
Also, you should
think about changing the entire drawing to either inches or
millimeters. Having both on the same drawing is kind of confusing.
Hope this helps,
boundary for RFS material condition modifier
afternoon Mr. Meadows,
Thank you for your time. I have been working at this company for 6
˝ years and have come to a basic understanding of GDT. One of my
goals at work is to better my skills in this field. Recently the
company library obtained a copy of your workbook "Tolerance Stack-Up
Analysis". Over the past two weeks I have been reading and trying
some of the exercises in the book. However I have come to a concept
that I do not understand and was hoping you would be able to help
me. I am having difficulty understanding how an RFS call out works
in a tolerance stack up. On pages 1-10 and 1-16 there are two
diagrams showing the worst case outer boundary and the worst case
inner boundary, respectively, in an RFS call out. For example in
the diagram on page 1-10, I perceive the center points of the 51 mm
diameter LMC dimension of the hole to be outside the 1 mm diameter
positional tolerance zone. Does not the median line composed of all
the actual local size centers need to lie within the 1 mm diameter
positional tolerance zone? I would appreciate it very much if you
could help me understand how the worst case is 49+2+2+1=54 for
axially out-of-straight holes.
Thank you very much,
Your question is a
good one. Most people misunderstand the concept of position
tolerancing. It falls under a principle that states that the axis
of the maximum inscribed cylinder for a hole and the axis of the
minimum circumscribed cylinder for a shaft must reside within the
positional tolerance zone. So, the answer to your question is,
“No, the median line composed of all the actual local size
centers does not need to lie within the 1 mm diameter positional
tolerance zone.” This concept not only applies to position
tolerancing but also to perpendicularity, parallelism and angularity
when used on holes, shafts, slot widths and tab widths.
You will find that
in the rest of the textbook I have not used these additional (size
tolerance times two) tolerances to calculate the boundaries for
holes and shafts, but instead, in RFS conditions, I have just used
the size tolerance one time. As I explain in the book, this is
because that although pages 1-10 and 1-16 are correct, I consider
them a special case (just for banana shaped holes and shafts) and
don't feel it represents the most common occurrences for parts.
Still, you have to be the judge of when this may or may not be a
consideration. I just try to show everything that could go wrong.
I gave a brief
presentation on this oddity recently at a ASME Y14.5 meeting (the
ANSI committee that writes the Dimensioning and Tolerancing
standard) and many of those present were shocked. One member even
came up afterward and tore off the flip chart pad sheets where I had
drawn illustrations similar to what I have on pages 1-10 and 1-16 in
your book. He said he wanted to take them with him because it was
such an eye opening experience. No one disagreed with the
Just remember, if
you work on very thin parts, such as holes in sheet metal, you
probably don't have to worry about this phenomena (banana-shaped
Hope this helps,
Good morning Jim,
I wanted to thank
you for your help. Your insight on the subject matter is truly
appreciated. As of this morning I have completed all the exercises
in Chapter 1 of the workbook. It is encouraging in that I am
understanding the concepts so far.
Thank you again,
you will all feel free to write in and share any insights you have
and ask whatever technical questions have been plaguing you and your
colleagues. In doing so, you make it possible for all readers to
learn about real problems you face daily in the workplace. And
hopefully, together we can find some answers to many of them.
that most of you will use good judgment in how you utilize this
forum. Not like the gentleman who faxed me 63 pages of questions in
one day or the one who called from a foreign country asking for bail
money. He said, “I attended one of your public seminars and you
said if I ever needed any help, I should call you. Believe me, if I
ever needed help, I need it now!” As much as I’d like to help, my
commitment to do so only goes so far.