REGISTER NOW FOR
A UNIQUE PUBLIC WORKSHOP PAIRING…
both courses presented by GD&T ‘expert’ James D. Meadows
Geometric Dimensioning and Tolerancing
[per the ASME Y14.5-2009 and 1994 Standards
...and the Differences between them] (2 ½ days)
December 9-11, 2013 – in Huntsville, AL
and/or (take one or both courses)...
Tolerance Stack-Up Analysis [for Plus/Minus
and Geometric Tolerancing]
(2 ½ days)
December 11-13, 2013 - in Huntsville, AL
See details or call
(586) 677-0555 to register and
inquire about discounts.
Subject: Questions regarding Simultaneous Requirements and
Position without Datum References
Hope this email finds you doing well. Things are good here. Our
company was recently bought by another. Big changes are coming, I’m
We are continuing to create standards here to minimize confusion and
we’ve bumped up against a question that we can’t agree on.
As you know, we have, in the past, relied on a consultant (not my
choice) that is intent on “Profiling the world” (to quote you). It
is one of the things he advocates that I just can’t agree with,
although I find it difficult to find a strong argument against.
We do rely on profile heavily. It makes sense for much of what we
do, but there are many times where position, perpendicularity etc.
are equally viable and clearer, in my opinion.
The question comes in two parts:
First, does the simultaneity principle (making multiple features and
patterns of features a simultaneous requirement-shifting only as a
pattern, measured in the same set-up or with one gage) apply to
profiled and positioned features if their datums and modifiers are
Second, is there a requirement for datum(s) on a positional callout
(ignoring the concentricity special case)?
The argument is that a position without a datum is simultaneous with
all the profiles without datums (assuming there are no modifiers)
and that the datum isn’t required for the profile.
Hope this makes sense.
Thanks for your time.
It’s good to hear you are doing well. I’m also sliding along in
1. Simultaneity does apply equally to position and profile controls
located from the same datums with the same modifiers.
To quote the current Y14.5-2009 standard section 4.19 page 76: “A
simultaneous requirement applies to position and profile tolerances
that are located by basic dimensions, related to common datum
features referenced in the same order of precedence at the same
boundary conditions.” In fact, in Figure 4-39 the title is
Simultaneous Position and Profile tolerances. No simultaneous
requirement exists if no datum references are used. In such a case,
to attain a simultaneous requirement between position or profile of
a surface controls, the local note SIM REQT may be used.
2. There is no requirement for datum references in a position
control. There never has been such a requirement. If two holes
within a pattern are located at a basic distance apart and their
position tolerance references no datums, the two holes are
positioned to each other. In fact, all position tolerances used on
patterns of features (such as holes) position the features to each
other before they position them to datums. The datum references are
additional requirements, after the holes are positioned to each
other within the pattern. What often happens is the two holes are
positioned to each other, then they become datum features, from
which all other features on the part are either positioned or
profiled. I thought when Figure 7-59 was added to the 2009 Y14.5
standard showing two shafts positioned to each other without datum
references, then showing the shafts becoming a pattern datum, which
is then referenced in a position control by other diameters on the
part, that people would stop saying position has to reference datums.
But, it seems that since Figure 7-59 shows two coaxial diameters,
someone at your place thinks this is only a special case for coaxial
diameters. It isn’t. The two diameters could just as easily be side
by side with a basic dimension other than the implied basic zero
dimension separating them.
I hope this helps.
Subject:GD&T for Pipes, Hoses or Tubing
Could you please help me in interpretation of below symbol used for
Position tolerances of Brake Pipes?
Thanks & Best Regards
Whatever they are doing, it isn’t supported by the ASME Y14.5
standard on dimensioning and tolerancing. It kind of looks like they
are calling out datum targets as datum features of size at Maximum
Material Boundary. But, without looking at the drawing, I can’t be
sure. We reference datum features in position controls, such as A, B
and so on, but we don’t reference A1 or A2 or B1 in position
controls. Someone has gone beyond what Y14.5 allows, but it may
still be interpretable. It just could have been done in a more
conventional manner. Also, I understand why we give X, Y and Z
dimensions for the axis location of tubes. We’ve always done that.
But, giving X, Y and Z separate tolerances that are all the
samenumber is odd.
Why not just give it a position control with a diameter of 4
millimeters that confines the axis of the tube. If the tube is
curved, this is done under the “BOUNDARY” method shown in Y14.5.Here
is an illustration from one of my textbooks:
FIGURE 19-4 [Positional Boundary Concept Used on Hoses, Pipes and
I hope this helps.
Subject: Bonus Tolerance vs. Datum Feature Shift
Hello Mr. Meadows,
I am looking at a tool drawing someone designed with the second hole
referenced to the first hole with a datum modifier MMB and a 3rdhole
referenced to the 2nd hole at MMB. My overall question is more over
the concept of, “Is there a point to making a single hole have a
Datum Shift Modifier instead of just providing the appropriate MMC
alone to give bonus tolerance?” I can clearly see the necessity to
use a Datum Modifier for a hole pattern in order to separate from
what the individual hole tolerance is, but why for a single hole? I
have attached a scan of a page from your book (1st and 2nd scanned
pages). I understand the simplicity you used for the sake of
explaining the concept, but otherwise, is there any practical reason
to not set up the second hole to just have true position tolerance
with extra bonus instead of a shift modifier?
Also, I have a question on the 3rd and 4th pages I scanned. So when
there is a datum modifier, should I always consider the datum
feature to shift with the type of tolerance in the original
reference frame, like perpendicularity in the 3rdpage. I have seen
some explanations from others that made it seem as if you took your
example, it would be looked at like a positional shift (no matter if
it originally referenced something like perpendicularity).
The pages Joey scanned from one of my books:
A Difference between Bonus Tolerance (Growth) and Datum
Feature Shift (Movement) of Tolerance Zones
One of the most often asked questions in measurement and also in
tolerancing is, “Can we take tolerance from the datum feature
referenced at MMB and give it as tolerance zone growth to the
features being measured from that datum?” The simple answer to that
question is, “No!”
Granted, there are some isolated cases where this strategy might
work out, but many more cases where it will not. Certainly, for a
pattern of holes referenced to a datum regular feature of size (such
as one hole), as the datum regular feature of size departs from its
virtual condition (Maximum Material Boundary concept), that pattern
of holes may shift as a group an additional amount. This apparent
shift of the pattern of holes is actually a movement of the datum
feature axis away from its imaginary datum axis. But it will appear
as though the entire pattern of holes has shifted/moved. This
concept is thoroughly explained in other sections of this book.
In this section, let’s explore a situation that is very simple: one
hole positioned to two datums. The planar primary datum will serve
the purpose of perpendicularity control, while the secondary datum
feature will be a hole which generates an axis that will be used to
hold a 500 millimeter distance. So, datum A will be for
perpendicularity and B will be for location in the following
FIGURE 5-29 [Part Drawing]
In the simple example depicted below, the following illustrations
show correct distributions of the tolerances that would allow parts
to pass the gage.
FIGURE 5-33 [Tolerance Zones]
Shifting vs. Growing Tolerance zones
FIGURE 7-20 [Shifting vs. Growing Tolerance Zones]
Many people feel the above two callouts (FIGURE 7-20, Examples 1 and
2) result in essentially the same geometric control. In reality,
they are quite different. In Example 1, the shaft axis is controlled
for perpendicularity within a diameter of 0.1 at MMC to datum A. As
the shaft departs from MMC (is made smaller, but still within size
limits), the tolerance zone will grow to permit a maximum
out-of-perpendicularity of the axis to datum plane A of a diameter
of 0.3 at LMC. Datum feature A has not, in this case, been
controlled for flatness. Datum plane A is taken from the high points
of the datum feature.
FIGURE 7-21 [Tolerance Zone for Example 1 in Figure 7-20]
In Example 2, the controlled feature is the bottom surface of the
part. That surface must be within two parallel planes 0.1 apart.
These imaginary planes are perfectly perpendicular to datum axis A
when datum feature A is produced at its MMC of Ø15.2 (which is also
its Maximum Material Boundary). All elements of the controlled
feature (bottom surface of the part) must lie between these two
parallel planes. This controlled feature is not only controlled for
perpendicularity but also for flatness to within 0.1. Since the
surface being controlled by perpendicularity is not a feature of
size, it is not allowed to be modified with the MMC symbol.
Consequently, the 0.1 tolerance zone cannot grow under any
circumstances. The flatness of the surface is controlled to within
However, the datum feature is modified with the Maximum Material
Boundary (MMB) concept using the . This means that as the datum
feature departs from its MMB (is made smaller than 15.2, but still
within size limits), a shift of the tolerance zone controlling the
bottom of the part may appear to occur. The two parallel planes 0.1
apart, within which all elements of the actual surface must reside,
may appear to shift (tilt) as a unit an amount equal to the datum
feature's departure from MMB. In actual fact, the datum feature axis
may tilt away from the imaginary datum axis by the diameter’s
departure from 15.2. This has the effect of increasing the allowed
out-of-perpendicularity; but at the same time, the flatness of the
controlled feature is held to within 0.1 (unlike Example 1). For a
visual depiction of this phenomenon, see FIGURE 7-22.
FIGURE 7-22 [Tolerance Zone for Example 2 in Figure 7-20]
When you have one hole positioned to another, it is like saying that
they work together, for example, they mate with the same part. If
they mate with the same mating part, the MMB modifier used with the
MMC modifier in the same control, is a way of saying that if either
hole deviates from its virtual condition, the holes may deviate more
from being perfectly positioned to each other. The larger the hole
(without being more out of perpendicularity to a planar primary
datum), the more each hole may move away from the basic dimension
that connects them. Picture a gage with two virtual condition sized
gage pins on a plate, one for the datum feature referenced at MMB
and the other for the hole being positioned. As each hole grows
(without being made more out of perpendicularity to the primary
planar datum), that hole may move more before it hits the gage pin.
Or, as each hole grows, it may be more out of perpendicularity to
the primary planar datum. Or, a little bit of both, but no more than
the gage pins would allow.
The gage described above would be different if the datum feature of
size (hole) wasn’t referenced at MMB, but rather implied at RMB. In
that instance, the gage pin simulating the datum feature would have
to expand into the hole, locking it up, and allowing no shift.
As far as your other question, that the perpendicularity control
shown on the third and fourth pages you scanned would somehow create
a shift that would equate to a position shift, no, that’s wrong.
There is quite a bit of difference between angle and location.
Position controls both angle and location, but perpendicularity
controls only angle. So, the shift on a perpendicularity control
that references a datum feature at MMB would only allow an angular
shift zone, since the relationship being controlled is only one of
angle (not distance).
I hope this helps.
That does help. I am still a little confused on the second concept I
brought up and you explained, but this figure I attached actually
illustrates my problem better than what I tried to use. For the hole
on the right, does the datum modifier of -B- at MMB represent added
positional shift (being in the original Datum Reference Frame) of
the feature datum or perpendicularity shift (since that is what -B-
has as a tolerance type) of the feature datum?
That one is positional shift. The relationship between the second
hole being positioned and the first hole (which is what the second
hole is being positioned to) is one of location. So, as the first
hole (datum feature B) grows from 49 toward 50, the second hole may
shift away from the datum axis of B by the growth of B. Any out of
perpendicularity of datum feature B negates the shift it allows as
The theory, as explained in Y14.5, is a little different than I
explained it here, and a lot more like I explained it the first time
with gages. The theory is that as datum feature B grows, its axis
may shift away from the imaginary datum axis B. This is pretty easy
to visualize, if you picture the gage I described with two pins on a
plate. The first pin axis simulates datum axis B. If the hole B is
larger than the gage pin (virtual condition), the hole B axis may
shift away from its own gage pin axis. So, to someone holding the
part in their hands, it will appear as if the second hole has
shifted away from its perfect location from the first hole. But, the
theory is that it is the first hole that has shifted. And because of
this shift, the first hole’s axis (datum feature axis B) will not be
coaxial with its gage pin axis (which simulates the imaginary datum
axis B). The axis of hole B (datum feature B) has shifted away from
the imaginary datum axis B (simulated by the axis of the gage pin).
Subject: Runout and Free State
I hope you are doing well. I have taken a couple or your classes in
Huntsville, AL, and I would like to get your input on a of couple
These questions are relative to ASME Y14.5M-1994.
As I understand it (188.8.131.52.1, p 189), Runout requires establishing
an axis by chucking/touching the stated datum reference feature(s)
and actually rotating the part to measure the FIM of an indicator
(dial, ldvt,…). Figure 6-17 (p 169) seems straight forward with
respect to free state, however, Figure 6-49 leaves me with some
1) Is the Runout of Figure 6-49 (p 191) considered to be a free
2) Assuming a lathe is used and is chucked on the datum reference
surfaces of Figure 6-49, can Runout be measured while still in the
lathe and be a valid Quality inspection, and would there be a note
required (or is it already understood) on the drawing to “allow” the
Runout to be measured while still in the lathe?
3) Considering the text implies the part is to be rotated about the
simulated axis and the indicator to be in constant contact with the
surface, for Figure 6-49, are the discrete points of a coordinate
measurement machine a valid means of checking Runout if the part is
Thank you for your time,
1. Yes, the runout controls in Figure 6-49 are free state
measurements. All measurements are free state unless a note is
written to specify they are to be restrained while measured. Free
state measurements are considered those wherein the measurement
equipment (chucks, probes, etc.) do not distort the part to obtain
compliance. In the gaging and fixturing standard (Y14.43, a
committee I chair) we say, you will use zero measurement force.
Still, we all understand zero measurement force is unattainable. But
the goal is understood to be: not distorting the part or the
equipment to an amount that significantly changes what the part
would measure in an absolutely free state.
2. Yes, you can measure it on the same machine on which you
manufacture the part. It isn’t considered a great measurement
approach, since we try to measure parts on machines that are more
accurate than those we manufacture them with. But, there is no rule
against it. All measurement is flawed in some way. It is up to the
company in charge of the project to decide how much measurement
error is acceptable. A measurement plan may be written that states
the part is to be measured on the lathe, but that isn’t necessary.
It just might save some arguments from occurring later on.
3. Y14.5 isn’t a measurement standard. Y14 standards are
documentation standards. B89 standards are measurement standards.
For example: B89.3 standards deal with Measurement of Geometry. What
you are trying to verify with circular runout on features such as
are shown in Figure 6-49 is that the surface is round and coaxial.
Circular runout generates a tolerance zone in these instances that
is (an infinite number of) two concentric circles that are the
geometric tolerance apart radially and centered on the datum axis.
Any way you can estimate that the surface is in compliance with
this, including using the CMM to do it, is valid, provided all
possible effort is taken to properly establish the datum axis and
enough surface points are collected (and enough circular
cross-sections are measured) to reach a confidence level sufficient
to satisfy the customer.
I hope this helps.
Subject: GD&T Dilemma
I would like your opinion on an issue I can finally share. One of
our design groups is trying to designate a pattern of rectangular
contacts a pattern datum. They are finding one pin center, finding
the relationship of that pin to all the others, taking some kind of
average location giving them the “centroid”. They want the
“centroid” of this pattern to be a datum from which other types of
contacts will be located…INCLUDING THESE! If these contacts were
cylindrical in design I would not have an issue with it in a
different configuration (4 select locations), and I understand why
they want to do it, but... They are working with a highly advanced
vision system which, in effect, builds a new gage for every part
checked by positioning a cylindrical zone on a basic dimension grid
originating from this “centroid” (the features are positioned at RFS).
The only pattern datums I have ever dealt with are a pattern of
Is there a legitimate way to do this on the print? I have attached a
basic drawing of the connector.
A bit more background…
• The customer does NOT trust gaging and has invested in this vision
• We have an internal spec which allows us to create a cylindrical
tolerance zone for a rectangular contact feature based on the
printed circuit board opening, but this does not necessarily allow
us to consider the rectangular feature to be a cylindrical datum…
• It would appear that between ASME, ISO combinations and the
customer demanding what they do not understand, it is very hard to
maintain the specifications set forth. The customer wins…until there
is an issue and we cannot prove we know what we made was acceptable
based on an inability to interpret.
Any input you may have would be greatly appreciated.
First off, rectangular feature can’t have cylindrical tolerance
zones. Y14.5 states:
7.4.5 Noncircular Features of Size
The fundamental principles of true position dimensioning and
positional tolerancing for circular features of size, such as holes
and bosses, apply also to noncircular features of size, such as
open-end slots, tabs, and elongated holes. For such features of
size, a positional tolerance is used to locate the center plane
established by parallel surfaces of the feature of size. The
tolerance value represents a distance between two parallel planes.
The diameter symbol is omitted from the feature control frame. See
Figs. 7-30 and 7-31.
The only mention of a square feature as a datum feature is in figure
4-46 shown below:
Normally, when a rectangular feature is used as a datum feature, we
use two sides as the secondary (width) and two sides as the tertiary
(width). Each generates one plane, the secondary and tertiary center
As it affects your situation, although the use of the diameter sign
in the feature control frame for the 20 rectangular features is
incorrect (wrong), they can use the 20 rectangular pins as a datum
feature pattern. It could also be said that the 20 widths in both
directions could create a centroid center plane for X and Y
measurements to use an the origin of measurement for the 16 pins.
For example, if a circled M had been used after the 0.2 for the 20
rectangular pins and subsequently, a circled M used after the datum
feature pattern reference B (in the position control for the 16
pins), a functional gage could be constructed consisting of 36 holes
(20 made to the virtual condition of B and 16 made to the virtual
condition of the 16 round pins).
The problem comes into play when they have to construct a centroid
for the 20 rectangular pins as produced regardless of material
boundary (RMB as it is called in Y14.5-2009). Y14.43 (the gaging and
fixturing standard) states that in situations like that, the gage
holes would have to contract at the same rate until the part is
immobilized by the gage holes contacting the pins. The question is,
how is the vision machine constructing the center planes of datum
feature pattern B?
This not only seems extremely difficult to measure and hard to
understand as a tolerancing scheme, but unnecessary, as there are
other datum schemes that would give the same results, but be
infinitely easier to measure and comprehend. In fact, in the Y14.5
and Y14.5.1 (Math) committees, they are currently trying to find
consensus as to what it even means when a group of cylindrical holes
or shafts are referenced as datum patterns RMB. There are at least
four competing theories of how to construct the centroid, and those
are round features. Yours are even more difficult, in that they are
If they insist on this path, good luck getting anyone to agree on
what is the proper method for constructing the center planes from
datum pattern B.
Subject: Profile with a Refinement of Flatness
Can flatness be used as a refinement of profile?
Yes, provided it is used to refine the flatness to within a smaller
tolerance, where the profile control is doing more than just
flatness within a larger tolerance. For example; if profile of a
surface is used to make multiple planar surfaces coplanar (existing
in the same plane), then each surface may use a refinement of
flatness. This will have the effect of making the surfaces
individually more flat than they are coplanar to each other.