|
Subject: GD&T Question about Cylindrical Tolerance Zones
James,
I have a question I would like to ask you (I took your class
about 7 years ago). Can you take a look at the attached print? The
circled area or DATUM C is the area in question. Our manufacturing
facility is stating that the positional callout on Datum C should be
not called out diametrically. I am more along the lines of that it
should be a diametrical callout. Can you please let me know your
expert opinion?
Thanks in advance for your help.
Regards,
Jason
Jason,
Both
datum features B and C need a diameter sign in their feature control
frames. Perpendicularity to datum plane A of both holes is a
critical issue for any part that mates with these holes and seats on
A. The holes’ axes may not violate a cylindrical tolerance zone
(which the diameter sign signifies) and still generate compatible
mating boundaries. If the diameter sign is left out of either
control, it would most commonly be viewed as a typographical error.
Jim
Subject: Quick Question Regarding Angles
Jim,
I
attended a GD&T seminar of yours a few years ago at UW Milwaukee.
Today, I am asking for a quick print interpretation (my first and
only one as a prior seminar attendee).
The 16
+/-0.5 degree angle, as drawn, would one measure the angle to the
"leg" directly under the angled tube (left most leg as seen in the
view with the angle call-out) or to datum A? Can one assume the
left leg is in the same plane as datum A?
Thanks
for the help,
Scott
Scott,
The
fact that there is a datum plane A on the drawing has nothing to do
with checking the 16 degree angle. Datum features and the
subsequent planes and axes they generate are only used for what we
tell people to use them for in feature control frames with geometric
tolerances.
The
fact that datum feature A seems to be in the same plane as what the
16 degree angle is measured from or to (who knows which), is not
pertinent to the measurement.
It does
raise another question, and that is, "Did the designer mean datum
plane A to be constructed from one surface, or two, or three?".
If
datum plane A was referenced in a feature control frame for
something like Angularity within a tolerance measured in
millimeters, then the 16 degree angle would have to become a basic
dimension (a boxed dimension without a plus and minus tolerance next
to it). Then we would know what was measured from what and the only
thing we would need clarified would be how many surfaces constitute
datum feature A and should it or they be controlled for form (and
possibly coplanarity) tighter than what is given in the size
tolerance from the opposite side of the part?
Jim
Subject: Query on a Datum Feature That References Itself
Hi Jim,
Please
clarify my doubts about the attached illustration.
The
issue is a Feature of Size having a Positional tolerance that
references datum B and the same Feature of Size establishes Datum B.
Does
this make sense and is it legal?
Regards,
Janardhan G.
Janardhan G,
The
control is just clumsy. The two holes called datum pattern B could
be positioned and only datum A referenced in the control. That
would mean the two holes are positioned to each other and
perpendicular to datum A to within zero at MMC. What has been done
on the drawing you sent me was probably trying to do that, but got
clumsy and it ended up as two controls with datum B mistakenly
referenced in the position control.
Jim
Subject: Tolerance Stack-Up Question
James,
I took
your tolerance stack-up analysis course several years ago. I
remember that you encouraged us to contact you if we have
questions. I like the approach you taught us, but I find that when
I'm checking work of other engineers, I find mistakes aren't made on
what's there but on what's not there.
For
example:
If a
print doesn't have a position callout on a hole, the engineer
conveniently forgets to consider it. This tends to happen when
using prints from days past when we weren't as diligent with our
prints. It makes the analysis easier but it's wrong. Engineers
tend to use the print as a checklist of things to consider when
performing the analysis. This assumes that the print is correct.
(Bad assumption.) Besides making sure prints are complete and
correct, do you have any advice to avoid this mistake?
Steven
Steven,
I agree
with everything you wrote. I find the most vexing problem in doing
stacks is incomplete or incorrect requirements. I take the easy
route and call the person responsible and try to fill in what is
missing, so that I can continue the analysis. I'm no better at
analyzing incomplete or incorrect product requirements than anyone
else.
I'm
like you, in that, I always assume that something in the
requirements will be missing or wrong. I usually look for those
before I do anything else, so that once I begin the analysis I'm not
slowed down or stopped when I reach that point.
Jim
Subject: Question
about Coplanarity
Hello Jim.
My old company laid
me off. They are in the process of closing the plant. I am now
employed at a new company and have a quick question that I am unable
to answer (without trepidation). So I am deferring to you and your
expertise.
I have a sheet
metal bracket. The end view has an omega shape; 2 tabs on the bottom
and a raised middle portion. The tabs form the primary base datum
-A- and are used to locate features on the bracket.
I have 2 options:
Option 1:
apply a 0.5 profile to the face of the tabs-both surfaces- and call
it -A-.
Option 2:
apply a 0.5 flatness callout on the 2 surfaces and call it
interrupted surface -A-.
I know the power of
profile. Is flatness legal for an interrupted surface primary datum?
I look forward to
your answer.
Thank you in
advance,
Ted
Ted,
Flatness won't put multiple interrupted surfaces into a single
tolerance zone. Use profile of a surface to control both
coplanarity and flatness.
Jim
Subject: Print Interpretation
Jim,
I hope all is going
well with you. I took one of your GD&T classes last April and was
hoping you could help me clear up an interpretation issue we have
been having internally here.
We have made the
parts shown below and have run into an issue on how the true
position of the sphere diameter. should be interpreted. I had
initially made suggestions to make the .280 and the .10 dimensions
as basic and only check the sphere true position from datum’s A and
B. This would have to be checked in X, Y and Z axis, but internally
it is being challenged that we can check the sphere true position in
all 3 directions.
Is it proper to
check a true position of a sphere in all three directions? Or can it
only be checked in two directions say…. X and Y and then the .280
would have to be checked separately (which I feel should be .380
dimensioned from Datum A). I think some of the reason things are not
adding up in regards to GD&T is because our customer is doing some
value added operations after they receive the part from us and maybe
they are locating from the surface opposite of Datum A.
I know you are a
very busy person and I appreciate any help you can lend.
Regards,
Mark
Mark,
The deviation from true position of a spherical diameter's center
point is equal to 2 times the square root of the deviation from the
basic dimension on the X axis squared plus the deviation on the Y
axis squared plus the deviation on the Z axis squared.
Hope this helps.
Jim
Subject:
How to Control for Warp?
Hi James,
I'm not sure how is the best way to control the amount of warp for a
part. The attached drawing shows an example. The thickness of
the part must be controlled to a relatively tight tolerance of
±0.01. However, it is acceptable for the part to be warped up to
0.10 in the unrestrained condition. This is a unique situation
where size limits cannot control surface form since the surface form
is not controlled as tight as the size. I don't think flatness or
profile is appropriate because the amount of acceptable warp exceeds
the size limits. Any help would be appreciated.
Regards,
Gary
Gary,
Use straightness of the derived median plane if it is per ASME
Y14.5M-1994 or flatness of the derived median plane if it is per
ASME Y14.5-2009. Just put the straightness or flatness control
below the size limits of the feature. In this way, the straightness
control can either be smaller or larger than the size tolerance. It
eliminates Rule #1 and allows the part to violate the envelope of
perfect form at maximum material condition.
James
Subject: Datum Target Areas
Hi Jim.
I have a part that I need to hold flatness on Datum A
but only in specific areas; is the way I have used datum target
areas correct? I'm also using a constraint note due to the
part wanting to bow after being machined. Thanks for your help.
Eric
Eric,
Given the note, I think this will be fine. Normally, I would
recommend Profile of a Surface to control the flatness and also the
coplanarity between the areas. But since they are all on the same
surface, and you are inspecting it while restrained, it should be
okay. Just remember, for future situations, that surfaces can be
flat, but not necessarily lie in the same plane. For example, all
could be flat and not parallel and be at different heights. But,
with this situation it's probably fine.
Jim
Subject: 1982 ANSI interpretation of MMC
Mr. Meadows,
trivia questions for you (only because I not sure of the correct
interpretation).
Would it be
accurate to state that all drawings that were created & released
prior to 1982 are allowed/granted MMC for the actual feature
identified within a feature control frame due to the fact that MMC
was ”implied” on all drawings per ANSI Y14.5?
We continually
challenge ourselves on this subject but my understanding is since
MMC was implied, that the engineer(s) created such drawings without
using the MMC modifier knowing it was implied. Would this be correct
to assume?
Another note –
We’ve seen some drawings which were created before 1982 that use MMC
sporadically on the drawing which is interesting because if it was
implied why would the engineer feel the need to use the modifier on
certain feature control frames but not others? So even with the
sporadic usage, we would still imply MMC on features where it was
not identified just to be consistent with the ANSI standard.
Please feel free to
reply at your earliest convenience as this information would be very
helpful on future interpretations. If you have any questions or
require any additional information, please feel free to contact me.
Best Regards,
Mark
Mark,
Prior to ANSI Y14.5-1982, only position was implied at MMC. All
other geometric characteristic symbols were implied at RFS.
Jim
Subject: Question on your Measurement Book
Hello Jim,
I was looking over
your book preview (Measurement of geometric tolerances in
manufacturing) at Barnes & Noble, but it only showed the first page
of the list of contents. And the other pages I could view without
buying the book did not really show me what I was looking for.
We’ve got a bit of
an argument going at my company between engineers and inspectors
over the inspection of composite tolerances. According to Lowell
Foster’s book, for the top segment of the composite tolerance; we
can use the standard X and Y coordinates deviations to calculate the
actual positional tolerance (2 x square root of X2 + Y2).
But for the bottom segment it says we cannot use this method. The
inspector used the same method on both segments and is failing the
part based on the part not meeting the lower segment.
I’ve asked them to
use the paper plot method on the lower segment and it passes but
they do not understand it. I was wondering if your book gives a
mathematical method so that I can order it, or you if can reference
some software or calculator program that can do it.
Thanks,
John
John,
With two holes, it's easily done with simple math. With more than
two holes, it either has to be graphed, or you have to have a
pretty involved software program to calculate compliance. The
problem in hole to hole relationships without location datums is the
movement and rotation of the pattern of zones (or the collected
variables data to see if they will fall into the tolerance zones).
You can always pick two of the holes and pretend they are datum
features, using one to measure distance from and the other to clock
your measurements. This means the first hole is perfectly
positioned and the second is out of position in only one direction.
Subsequent holes are seen as out of position in both the x and y
directions established by the first hole and the common plane
between the first and second hole. The problem is that this method
isn't perfect. It doesn't allow the rotation and movement of the
pattern to match the data to the tolerance zones.
If you are willing to graph the results, either on graph paper or on
a computer screen, it's very easy to determine compliance and you
have a visual display for doubters. Yes, these things are addressed
in my purple "Measurement" book and my yellow GD&T book.
I can't believe your measurement people are pretending that the
datums existing solely for the upper level control also apply to the
lower level control and are rejecting parts on the failure of holes
to meet their relationship to those datums, when (in the hole to
hole tolerance level of control) none applies.
Good Luck.
Jim
Subject: Datum References within a Position Control
Jim,
I was wondering if
you could shed some light on a question about a particular use of
datums within a position control. I’m reviewing several drawings and
most of them have multiple coaxial diameters where one is a datum
(datum axis A) and the others are positioned to it. The question I
have is about an appropriate use of a secondary datum (datum B) that
is a perpendicular face to datum axis A. Just about every drawing
contains at least one coaxial diameter that is positioned to A(M)|B|
(as overly simplified below). Does the addition of B actually add
any value to this control? I assume if they were trying to control
orientation (perpendicularity) to B, they would make it the primary
datum. There are no basic dimensions from B, so I don’t see what it
adds. Am I missing something?
Thanks in advance,
Bob
Bob,
You aren't missing anything. Unless datum feature B is used as a
primary datum, it doesn't add anything to this control.
Jim |
