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 ˝ 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 ˝ days)
December 11-13, 2013 - in Huntsville, AL
See details or call
(586) 677-0555 to register and
inquire about discounts.
Subject: Basic dimension conflict?
Hello Mr. Meadows:
A colleague and I are having a discussion about whether there’s a
problem with what is shown on the attached snippet of my drawing:
I’m using the slot to define a datum plane “E”. My datum is then
used for the true position control of some other features not shown
on the snippet. What I’m wondering is whether or not there’s any
conflict between the theoretically exact size of the slot (6mm)
.2362”, and what is shown as the fabricated size of the slot
This situation arises in my CAD system (SolidWorks) because the hole
gets drawn to its nominal size of 6mm, yet applying an F8 fit to the
hole, (and then converting to a limit dimensions) changes the actual
hole dimension to read on the +/+ side.
I know that the ANSI standard says that tolerances are not inferred
from a dimension which is basic; but it admittedly looks a bit
strange on the drawing. Can you help me clear up the confusion?
Dimensioning the width of the slot at both basic and then as a limit
dimensioned size is wrong. Choose one. I’d choose the limit
dimension. That has a size tolerance and a position tolerance. The
one that has a basic width would need to be profile toleranced,
since profile is the only geometric tolerance capable of tolerancing
a basic size.
Subject: Threaded Features as Datum Features
Long time no speak.
What is your opinion regarding threads as datums? Is that a loaded
question? In my particular case I’m trying to protect the Virtual
Condition boundaries between two very long parts that mate together.
One part is a shaft with external threads and the other part is a
hole with internal threads. The debate is which features would make
better datums? The shaft/hole or the thread/thread on each part? My
thoughts are since I can calculate the Virtual Condition on a
shaft/hole much easier than the Virtual Condition on threads; I’ll
make the threads my datum and geometrically control the shaft/hole
to the threads at MMC. In my mind, a GO thread gauge could hold the
threads and the run-out could be measured on the shaft. The concern
is the “slop” between a thread GO gauge and the actual thread size.
But I’m allowing for the “slop” as pattern shift because the datum
is at MMC. Am I crazy? Not certifiable, but just in regards to this
topic. Thanks for the help and happy holidays.
Even though people normally try to avoid threaded features as datum
features, it sounds as though you’ve thought it through and have it
all worked out.
Subject: SURFACE PROFILE REQUIREMENTS
I took a training course that you presented at our facility several
years ago for GD&T. I have a question that I was hoping you could
shed some light on. I have a part with complex curvature that
contains no good datum features (see attached). I want to use a
surface profile callout as shown applying the control to only the
top curved surface, but it’s not clear to me whether or not I need a
datum A (which would be the bottom curved surface) listed in the
feature control reference frame. Would you please explain the best
approach for this example along with your rationale? What is the
difference between using datum A or not using datum A with respect
to surface definition and inspection?
Thanks for your help,
If the profile control is meant to apply “ALL AROUND” or “ALL OVER
(to all surfaces in all views) there is no need to reference a
datum. Without a datum they can scan the surfaces and allow the
computer program to determine if all points reside within the
tolerance zone. This would control the size, shape angle and
location of the surfaces.
The way you describe the control, it would only apply to that one
curved surface (the top), and would only control the shape of that
single surface, and the tolerance zone would terminate at the sharp
corners. In that case, you might want to reference datums to give
orientation and/or location of the surface being profiled from the
So according to the approach described in your 2nd paragraph, you
are saying it is acceptable, but not required, to use the other
complex curved mating surface as datum A? What are the pro/cons to
using or not using datum A? I have a QC guy here that is adamant
that datum A be included, so I am trying to get resolution for this
Thanks for responding.
Referencing datums in a profile of a surface control is optional. If
you wish to relate that surface to a datum plane or axis to hold an
angle or location, then reference one or more. If all you want to
control is the shape of that surface, then don’t.
I’m just surprised you aren’t defining more of this oddly configured
part with basic dimensions and profile tolerancing than just that
one surface. It seems like you’d want to define the entire periphery
with a profile tolerance to control its size and shape, as well as
the angles and location of all elements of all of the surfaces on
this part. But, I don’t know what the intent of the rest of the part
definition looks like, since you only described to me a partially
You could define this entire part with basic dimensions and basic
radii, then give it an all-over profile control that applies in all
views. The entire part would then be completely toleranced and it
could be done with no datum references.
Subject: GD&T Questions for a long cylindrical part
I hope you’re doing well.
I write to you with GD&T questions (as usual). Would you mind
reviewing the attached prints (deliberately incomplete on certain
features) and letting me know if you’d be interested in helping me?
Q1. What would be your recommendation on holding OD to ID of a long
cylindrical part like this?
Q2. I’d like to get your thoughts on positioning Datum D (threads)
to Datum C (predrill for datum D threads), which in turn is held to
datum B (smaller through hole on center to predrill).
Q3. I'd like to get your thoughts on tying a feature such as Datum E
and Datum C to datums A and B(M). I think datum A is a no brainer.
Would it be better to position Datum D (threads) also to datums A
and B(M), like datum C’s feature control frame?
Q4. I'd like to get your thoughts on GD&T around a slot feature
Q5. A first mating part is attached to the datum A end of the part,
keyed by datum E and bolted on via the datum D threads. This first
mating part has an arm with a through hole in it, designed to target
hole on the cylindrical part (the .281 hole is shown on sheet 2). A
second part, that is designed to mate with the cylindrical part, is
inserted through this first mating part (into the .281 hole).
There is a strength concern at the thin wall section around the .281
hole - the GD&T on the .750 OD and .281 hole is meant to reflect
this. I understand LMC would be the ideal condition but considering
gauging, I thought MMC may be the way to go. Would you agree with
the way it is dimensioned?
I took non-important dimensions off – please let me know if you feel
you need more info.
Please let me know if we could discuss these questions by email or
over the phone, or better yet if you will be in Memphis in the near
Illustration of Long Cylindrical Part:
I’m doing well.
Addressing the matter of the order of how the datum features are
defined, datum feature B is perpendicular to A. Position isn’t
correct there. But, there is some question in my mind whether datum
feature A should be the primary datum reference, since it has so
little surface area. If something must seat well (3 points of high
point contact) on A, then it would make sense. If not, or it is just
a stop, well…in most of these coaxiality controls, it could be
Positioning The OD to datum feature B works. The only thing total
runout would add is a cylindricity (3D form) control to the location
control that position gives you, but since the size tolerance is
tighter than the geometric tolerance, it wouldn’t even do that.
Positioning C to B works. I won’t mention the same question I have
over and over about datum A as primary.
Positioning the threaded feature to C for coaxiality works, but a
question needs to be asked at this stage, “Why are you switching
datums so frequently?” A good answer would be that the mating
feature only interacts with the threads and C, and doesn’t reach
into B. Also, we try not to make datum features of threaded features
(D). This is especially a good thing to consider, since the slot (E)
isn’t positioned to D. It’s positioned to B. Could everything be
positioned to B?
The order of the datum references used for the position control for
the .750 diameter is especially odd. If the OD is centered to the
thread (D) in one direction, shouldn’t it be positioned to the
thread in the other? If D was primary, that would happen, then the
slot (E) could be eliminated in this control. But, if you want to
center the OD to the slot in one direction (let’s call that the X
direction), then center it to the thread in the other direction (the
Y), then this order (E then D) is correct. I’d hate to have to
design a gage to check it though.
Treating an elongated hole as though it is two round holes that
somehow got connected by a width is not something we often do. Why
not just get rid of the diameter signs and position the entire
elongated hole to H and E (in that order-so that E is just
controlling clocking/angular orientation).
If I didn’t cover everything, write back.
I hope this helps,
Thank you for your reply. It definitely helps, and I hope you
wouldn’t mind if I dive into this deeper:
I have the same concerns with the small surface area of datum A. The
reason it was chosen as primary is because unfortunately, it is
quite possibly the feature with the largest contact area with the
mating part, which I named the “first mating part” in my original
email. It has 3 mating features: datum A, datum E and datum D.
Datum E isn’t “mating” per se – it provides rotational clocking so
that it can used to accurately insert the 2nd mating part into the
.281 hole. As such, it is possible that datum E actually doesn’t
make contact with the “first mating part”.
When using this particular family of devices we recommended
tightening the bolt that holds the “first mating part” to this “as
much as possible by hand”. As such, it is possible that the
cumulative contact area between the threads (datum B) and the bolt
is larger than the contact surface datum A sees. However, it was not
chosen as the primary datum since this cumulative contact area is
not quantifiable, and since I am uncomfortable using threads as
primary datums in general. Having said this, I still thought it was
important to keep it in the Feature Control Frame since it appears
to be an important feature to the function of the assembly and hence
I would like to hear your comments on this.
I’m glad to hear positioning the .500 OD and .272 predrill to datum
B works. My quality engineer asks how you would inspect this, seeing
that datum B is over the majority of the 20” length.
Absolutely, everything can be positioned to B. This again becomes an
The reasoning for the threads (datum D) being held to the predrill
(datum C), which in turn is held to the ID (datum B) is that this is
the order of manufacturing process.
The reason datum E is held to B and not to D is also that datum E is
manufactured onto the part separately from the predrill and threads.
Regarding the .750 diameter, I don’t understand your comment “If the
OD is centered to the thread (D) in one direction, shouldn’t it be
positioned to the thread in the other? If D was primary, that would
happen, then the slot (E) could be eliminated in this control. But,
if you want to center the OD to the slot in one direction (let’s
call that the X direction), then center it to the thread in the
other direction (the Y), then this order (E then D) is correct.”
This may not matter, but here’s the background. I focused on the GD&T
around the .281 hole first. Then, I used the same GD&T on the .750
OD because there is a strength concern in the relationship between
the .281 hole and .750 OD.
Thank you again.
To address the last thing first, when the OD references A/E/D, A
serves as a perpendicularity datum, E centers the OD to the slot
centerplane and D centers to the axis of D in the direction that E
hasn’t controlled. This is unusual. Normally, you would want to
center the OD to the axis of D. This would eliminate the need to
reference E, since, at that stage, it could only serve the purpose
of anti-rotation of the OD and that isn’t needed.
The order of the manufacturing processes for the assignment of datum
references is really a minor factor. This isn’t a process
engineering drawing. It’s a finished product requirement based on
functional needs. Every time you change datums, you accumulate
tolerance error, and if one of your concerns is wall thickness, it
could adversely affect that. If one datum feature is used, such as
B, to center everything, then one gage could be made to inspect all
features referenced to the same datums (as a simultaneous
requirement). That’s if they want to gage it. If not, one set-up
would be required to measure everything that is referenced to the
One thing that is gnawing at me about the comments you are making,
is that it seems you are allowing the manufacturing and inspection
people to dictate how you are specifying your functional
requirements. That only works if the changes you make to appease
manufacturing and inspection results in a product that is just as
functional. If not, if it was me, I’d insist that the functional
requirements not be abandoned.
My comments on using datum A as a primary datum remain the same. If
A is needed to dictate the angle at which the parts assemble, then
use it, and use it as primary (or else it’s useless). If A is just a
stop, then don’t use it, if all you are trying to control is
coaxiality of one diameter to another. If the parts are to be gaged,
a threaded feature as a primary datum feature isn’t difficult to
It sounds from you description of how the part works that, for the
hole that becomes H, since E is only being used as a datum to stop
rotation, it must be used after the datum that is to be used to
locate/center the other diameter(s). In this case that would mean
that instead of E/C, it should read C/E.
There’s probably a bit more I should comment on, but I'll let you
think about this for now.
Subject: Virtual Condition question on I.D.'s
Dear Mr. Meadows,
My name is Eric and you taught a class at our company in Chicago,
Illinois last year. I have a question because I am not sure of
We have a part that has two concentric bores. One bore is labeled
Datum –B- and is 3.379-3.378 in size. The other bore is 4.251-4.250.
Based on the attached PDF what would the VC of the 4.251-4.250 be
4.249 at MMC with the 3.379-3.378 bore at 3.379 due to the bonus
4.250 (Bore at MMC)
-.000 (bonus tol on bore size)
-.001 (bonus tol due to 3.379 size on the 3.379-3.378 bore)
Dear Mr. Meadows,
Thanks for the clarity. The Datum feature B would have a
perpendicularity control of .0005 relative to A. My intent is to
setup the part so that a functional gage could be designed and used
for resting on Datum A and would check Datum B and 4.251-4.250 bore
positions. FYI, the Datum surface A, B, and the 4.251-4.250 features
are machined in the same setup.
4.251 = LMC of counterbore
+.001 = Geo. Tol. @ LMC
4.252 = Outer Boundary of counterbore
+.001 = Pattern Shift Datum B M
4.253 = Outer Boundary counterbore w/ shift
+.0005 = Position of Datum B
4.2535 = Outer Boundry of the counterbore
4.250 = MMC of counterbore
-.000 = Geo. Tol. @ MMC
4.250 = Inner Boundary of counterbore
-.001 = Pattern Shift Datum B M
4.249 = Inner Boundary counterbore w/ shift
-.0005 = Position of Datum B
4.2485 = Inner Boundary of the counterbore
4.250 is the virtual condition as defined in the ASME Y14.5
standard. Virtual condition for a hole is; the MMC minus the
geometric tolerance that applies at MMC (4.250-.000=4.250). The
datum feature shift derived from using a circled M after datum
feature B is often a factor in calculating tolerance stacks where
this hole is one of the pertinent features in the stack, but the
virtual condition definition does not include that shift. This is
just semantics. If the datum feature/pattern shift is a factor in
your calculation, use it. Just don’t call the result a “virtual
As an aside, unrelated to this discussion, the datum feature B needs
a perpendicularity control relating it back to datum plane A.
Without it, datum feature shift and the virtual condition of datum
feature B wouldn’t be possible to calculate.