You taught a class here at my company a year or so back and I found
it to be very informative.
have a question on how to specify shaft runout to the axis of
rotation of a motor and specifically how to label a datum.
Would you say that attached sketch is properly defined for checking
individual shaft runout without a functional gage that would combine
Perpendicularity, Concentricity and Runout?
Thanks for any insight you can provide on this.
Thanks. I look forward to coming back to your company.
There is a rule in Y14.5 that states that datum features are
identified on drawings by means of symbols. These symbols relate to
physical features and may not be applied to centerlines, center
planes or axes. This is avoid confusion about which diameter
generates the datum axis. An inspector must know what diameter to
chuck up on, grab or probe to generate datum axis A. So, putting
the datum feature symbol on what could be the axis of several
different diameters is not legal and it isn't specific enough. You
must pick a specific diameter, then attach the datum feature symbol
to that outside or inside diameter.
Circular runout does not control the perpendicularity of a planar
surface. It just equalizes material on each side of the datum axis,
so that it doesn't wobble when rotated. Total runout does control
flatness and perpendicularity of a planar surface to a datum axis.
So, if you want the planar surfaces to be perpendicular to datum
axis A, just replace the single arrow (circular runout) with the
double arrow (total runout).
Circular runout used on a diameter usually controls its roundness
and its coaxiality to the datum axis. But on your diameter, the
size tolerance is so tight that it takes over the job of controlling
the roundness, straightness and taper of the surface. Rule #1
states that the size tolerance controls the surface form, unless
overridden by a tighter control. All that leaves for the circular
runout to control is the centering (coaxiality) of that diameter to
the datum axis for balance. Total runout would be capable of
controlling cylindricity (roundness, straightness and taper), but
only if the total runout tolerance was tighter than the size
tolerance. Both total runout and circular runout control the
centering (coaxiality) of the diameter to the datum axis.
hope this helps, and that I get to see you again some time.
Subject: Re: Rule Number 1: Does it also controls form variation
such as flash.
enjoy reading your extensive info regarding G,D,&T. It's amazing
how some people are allowed to guess at the interpretation G,D,&T
and of "Rule Number 1". To help me end an argument and promote your
expertise, can you help me convey the following.
This company seems to think the rule number 1 doesn't have any
control over a form variation such as plastic flash. Without
additional notes, does rule number 1 in any way not apply to plastic
flash????? And, is there any quick reference you know of that
states this??? And, is there an appropriate flash allowance note
that you know of to supplement rule number 1 for the allowance of
hate to be the bearer of bad tidings, so I have attached the
appropriate page from the standard ASME Y14.8-2009-Castings,
Forgings, and Molded Parts. It says, "Gates, riser stubs, flash,
etc., may exceed perfect form boundary at maximum material condition
(MMC) unless otherwise specified."
Subject: How Best to Purchase your Books and DVDís
When purchasing your G,D,&T books and DVDís for use, who Should I
purchase it from to get the best price and speed of delivery?
Any of my books can be purchased from my website
www.geotolmeadows.com or by phone at (615)824-8644. This is
usually faster and the middle man gets cut out.
Hello Mr. Meadows,
I hope this finds you well...
First of all, your Dimensioning and Tolerancing book (yellow cover)
was my greatest resource - along with the Standard, of course - in
passing the Senior-Level GD&T exam - a very well-written book. I
keep it at work.
I am starting to read my newest purchase - your GD&T book based on
the new 2009 standards - obviously, yet another good book.
I have a few questions.
Before I continue any further with those questions, and it really is
only a few, knowing your time is very valuable, do have a few
moments to correspond with me, a fellow GDTP Senior Level "Club"
am well, thank you. I appreciate you purchasing and using my
books. It's always nice to get praise for my work. We all need
that from time to time.
congratulate you on your success at being a certified GD&T senior
professional. Itís gratifying that I played a small part in your
success in passing the test. Iíve been receiving a lot of
ďnotificationsĒ lately from professionals who have passed the
Geometric Dimensioning and Tolerancing Professional Senior Level
exam. They are from people who wanted to thank me for teaching them
what they needed to know to pass the exam and people like you who
have gotten what they need from my books or DVDís.
Itís interesting to me, in that I donít teach or write books
specifically to pass the exam. Itís just that what I teach and
write apparently allows people to easily pass the exam.
I'm like a lot of those people, just a technical geek who found a
fit between things that interest me (math, logic, a blend of
manufacturing, inspection and design skills I've both studied and
picked up along the way) and a subject that I can make a living at.
I enjoy being able to work on a wide variety of products as a
consultant and learning from those professionals I work with and
I'm always here for you if you have a technical question or just
want to verify something you think is true, but aren't certain of.
Best of luck.
Subject: Conical surface as datum
Dear Mr. Meadows,
One question left unanswered in my training is the use of a revolved
surface, other than a cylinder, to establish a datum axis. For
example, I would like to assume that a Datum on a leader attached to
the surface of a cone would establish the axis of the cone as the
datum. I might also place an "all around" symbol on the leader to
insure the horizon line of the cone is not mistaken for the datum
instead of the axis. I would greatly appreciate your feedback on
Ps. Is the price structure for your on site training listed on your
I've attached a couple of illustrations from one of my new books to
explain conical features that are used as datum features. Don't
worry about attaching an "all around" symbol to the leader. When
you specify a cone as a datum feature, you always generate a
datum axis at its center and also a plane at the apex of the cone
from which to measure. I've also shown an illustration of how the
ASME Y14.5-2009 dimensioning and tolerancing standard allows us to
override the plane at the apex of the cone, if you want to establish
another datum from which to measure distance in that direction.
The ASME Y14.5-1994 version of the dimensioning and tolerancing
standard didn't mention cones used as datum features (although it
wasn't specifically forbidden). The ASME Y14.5-2009 standard shows
that conical features can be used as datum features (as I've shown
in the attachments).
On-site workshop quotes are handled by Jeannie Winchell from my
office. She would be happy to send you a quote, but would need to
know how long a course you would like, how many people would be
attending and specifically what course you would want (basic,
intermediate or advanced), what year of the Y14.5 standard you'd
like covered (1994 or 2009) and when the workshop would be held.
She would be happy to call you or it could be handled entirely by
email if you'd prefer.
Hope this helps. The illustrations follow.
Illustrations of a Conical Datum Feature
Means this: Datum feature A generates an axis (which consists of
two planes intersecting at a 90 degree angle) and (from a point) a
datum plane. This means that conical datum feature A generates
three datum planes. The 12.5 holeís axis must intersect datum axis
A and be 38mm from the tertiary datum plane also constructed by
datum feature A to within the holeís position tolerance of a
diameter of 0.1 at MMC.
Specifying or Overriding the Degrees of Spatial Freedom-A Truncated
One of the most practical uses for overriding spatial degrees of
freedom created by datum features is for the conical primary datum
feature shown above. Cones are designed into many product lines
throughout the world and sometimes are the most functional feature
on the part from which to locate.
Since the conical primary datum feature, as shown above, not only
generates an axis for positioning the 10 millimeter hole, but also a
datum plane at the apex of the cone, it creates a situation where
one may wish to choose another datum feature for location of the
hole along the axis of the cone. The problem is that since the cone
is the primary datum feature, that longitudinal (z) degree of
spatial freedom has already been stemmed by the plane at the apex of
Overriding that degree of freedom is now possible per ASME
Y14.5-2009 by listing the degrees of freedom controlled by the
conical datum feature A [x,y,u and v], but not listing the spatial
degree of feature down that axis [z]. A subsequent datum feature is
referenced, in this case B, and the z degree of freedom is listed as
being controlled by it. In this way, we can have the 10 millimeter
hole be perpendicular to datum axis A and intersect datum axis A,
but hold its 24 millimeter basic location from datum plane B (all to
within the positional tolerance of a diameter of 0.2 regardless of
the feature size).
Subject: Question about Tolerancing a Slot Pattern
would like to ask you a question on slot location if you have the
Please see the attached powerpoint - a picture is worth a thousand
am trying to geometrically tolerance slots from a datum and also
control the two ends of the slot to each other. You must have seen
this a thousand times.
Thanks in advance for your help. I am looking into taking your
Geometric Dimensioning and Tolerancing class for the Y14.5-2009
The size tolerance on each slot controls their relationship for size
Composite Tolerancing (PLTZF)-First Level of Control-Pattern
Locating Tolerance Zone Framework:
The position tolerance controls the relationship of the centerplane
of each slot to the datums referenced in the pattern locating
tolerance zone framework (upper lever position control). The basic
dimensions should be shown from datum F to the center of each slot.
It controls the movement (location) and orientation (angle) of the
centerplane of the slot from the datums to within 0.04.
Composite Tolerancing (FRTZF)-Second Level of Control-Feature
Relating Tolerance Zone Framework
The location of the slots to each other is controlled to within 0.02
(this lower level of control is called the feature relating
tolerance zone framework). This is also a centerplane control.
Everything would be correct if the basic dimensions were to the
centerplane of each slot, instead of to the edge.
Subject: Gage Dimensioning and Tolerancing
Compliments, I am enjoying your "Workbook and Answerbook" for
Did you design the gage purposely this way?
may not understand something? ISBN: 0-9714401-7-4 problem 50
(page-93) has a solution (page-248). Possible interference fit in a
worse-case scenario of a hole size smaller than the corresponding
largest worse-case shaft size.
Some feedback would be appreciated.
Functional gages are designed at the virtual condition boundary of
the features they inspect. The recommended gage tolerancing policy
of the ASME Y14.43-2003 standard (a committee I chair) is to accept
no out-of-tolerance parts. Therefore gage pins are all plus
tolerance and gage holes are all minus tolerance. Since no
out-of-tolerance parts are to be rejected, a small percentage of
borderline, technically in-tolerance parts will be rejected by such
a gage. There are two gage tolerancing policies that fit this
requirement. One policy is called Absolute gage tolerancing (which
allows no bad parts to pass, even in theory). The second policy is
called Practical Absolute gage tolerancing. The gage you are
referring to in your email uses the gage tolerance policy called
Practical Absolute gage tolerancing, which means that although a
mathematical possibility of the gage buying an out-of-tolerance part
exists, the gage will, in practicality, not accept a bad part. And,
as you have noted in your email, this policy will reject some (very
few), borderline technically in-tolerance parts.
Functional gages check geometric tolerances (referenced at MMC and
MMB) and the virtual condition boundaries they create (which is what
the gage pins represent).
gages check maximum material condition and use the recommended gage
tolerancing policy called Absolute that also says all gage pins have
only a plus tolerance (no minus tolerance).
There are other gaging policies described in Y14.43, but not
recommended. One of those policies is called Optimistic gage
tolerancing. Optimistic gage tolerancing allows some borderline
out-of-tolerance parts to pass inspection. Optimistic gage
tolerancing says that all gage pins have only a minus tolerance, no
Tolerant gage tolerancing allows both a plus and minus tolerance on
gage pins and gage holes. This is the worst policy, in that the
inspector doesn't know whether the gage is going to be made in the
range of sizes that accepts borderline bad parts or rejects
borderline good parts.
you are really interested in gages and how they are designed,
dimensioned and toleranced, please get a copy of ASME
Y14.43-2003-Dimensioning and Tolerancing Principles for Gages and
Fixtures, or a copy of the textbook that goes with the workbook of
mine that you have.
Hope this helps,
Subject: Dimensioning Question about Runout
Hope things are going well for you. We are busting our butts in the
engineering dept here. Production is kind of slow so we are busting
it with design work.
have a couple of dimensioning questions that need your help with.
1) See picture below. We need to know how this would be
dimensioned on a drawing. The shaft Runout is interpreted by us as
rotating while the motor is fixed. The shaft would be turning
between the bearings fixed in the assembly. The face runout would
be that the shaft is fixed and then the motor is turned. Same would
be true for the Eccentricity.
2) I have a tolerance analysis to do on the attached drawing to
determine the stackup of the Circular Runout . The customers spec
is attached. They wanted True Position, but our production line
wanted something that would allow them to check it on the floor by
using Runout. The main concerns are shaft straightness and position
of the Boss to the axis of the shaft. Based on this would we get
the same results and if so do I use Ĺ of the runout tolerance or
not? If not, can you help me understand how I do this analysis?
Thanks for your help. We are still planning on trying to schedule
you for a update training soon. I have budgeted the money.
hope you are doing well up there in that beautiful country. I'll
never forget my visit. It was something to see.
Both Circular Runout and Total Runout are defined as a "surface to
datum axis control". If used on a diameter, circular Runout
controls roundness and concentricity to the datum axis. Total
runout controls roundness, straightness, taper, and
concentricity, if used on a cylindrical diameter.
Circular Runout controls balance of material on each side of the
datum axis, if used on a planar (flat) surface. Total Runout
controls flatness and perpendicularity to the datum axis, if used on
a planar (flat) surface.
Figure 2 Verifying Motor Specifications, in what is called "shaft
runout" if the motor isn't being centered on, and the motor's axis
isn't being rotated about, the only thing it looks like you are
measuring with that setup is roundness and (if you run the indicator
down the diameter longitudinally) perpendicularity. If you aren't
rotating about a datum axis, you aren't measuring any type of runout.
You would have to be centered on another axis, to measure the runout
of the shaft to that other axis.
what is called "face runout", if you are centered on and rotating
about the motor shaft, you can measure either Circular Runout of the
face (which protects a balance of material on each side of the datum
axis), or Total Runout (which protects flatness and perpendicularity
of the face to the datum axis).
what is called "motor shaft to pilot diameter eccentricity", that is
actually measuring Circular Runout. If the diameter on which the
dial indicator takes its readings was longer and the indicator was
moved down its length, then it would be measuring Total Runout.
Position, Concentricity, Circular Runout and Total Runout all allow
you to be off center of the datum axis one-half of the amount that
appears in the feature control frame. So, if the geometric
tolerance specification is .010, then any of the controls I listed
would allow you to be off center a radius of .005. Since indicators
read how much you are off center in one direction as "plus" and 180
degrees from that it would read "minus", then if you were off center
a radius of .005, your full indicator movement (FIM/TIR) would be
plus .005 on one side and minus .005 on the other. Your FIM would
be .010, which is all it is allowed to be out for Runout controls.
And even though Position and Concentricity are measured differently
than the Runout controls, they would not accept a part that was off
center any more than a radius of .005 either.
you need more information from me, I'll get back to you as soon as I
Hope this helps.
Subject: Re: GD&T questions about Combining Plus and Minus and
I took your advanced GD&T course last fall and I just had a couple
of quick questions I was hoping you could clarify for me. I
attached a rough sketch to help convey the meaning of my questions:
1. (see attached Fig. 1) According to the 1982 standard is it
allowed to have a regular dimension(.5+/-.1 in Fig 1) locating the
edge of the part when a positional tolerance is used to locate the
holes? Can the dimension be non-basic as long as the hole to
hole relationship is maintained or does the .5 dimension need to be
2. (see attached Fig. 2) According to the 1982 standard is it
allowed to use a compound axis as a reference in a profile
tolerance? Is it allowed to use the datum features being
defined as a compound datum reference in the profile tolerance?
(Only the dimensions locating the bottom surface of the channels are
I hope the sketches are clear enough,
Y14.5-1973, there was an example of what was called Combination
Positional Tolerancing. It allowed a combination of plus and minus
tolerancing to locate the hole pattern and then position tolerancing
was used to position the holes within the pattern to each other. It
was believed, at the time, to create rectangular tolerance zones for
the hole axes from the "implied datum features" which were the edges
of the part, and cylindrical tolerance zones from hole to hole (and
for perpendicularity, since the primary datum feature was shown in
the example and was for perpendicularity).
Y14.5-1982, this example was moved to Appendix D Former Practices.
In other words, it was taken out of the standard in 1982 and
replaced by Composite Positional Tolerancing as the acceptable
method of accomplishing a larger position tolerance from the
specified datum features and the planes or axes they generate and a
tighter position tolerance from hole to hole. Composite Positional
tolerancing had been in the Y14.5-1973 version of Y14.5, but in the
1982 version, with the removal of Combination Tolerancing, it took
on a more important role.
far as Profile controls referencing a compound datum axis, it is
most certainly legal and sometimes needed. The example you show,
profiling one side of the widths that create datum features C and D
to datum axis A-B is okay. I would think it is more common to
reference A-B to locate the entire width of C and D. The "or"
example is even more unusual, wherein one side of the feature
widths generating the centerplane of C-D are being Profiled to C-D.
Still, although not that common, it is perfectly legal. You might
also ask yourself if it is the best option though.
Hope this helps.