|
Subject:
Re: Question on Measuring Projected Tolerance Zones
Mr. Meadows,
My Name Is Stacy. I’m from an aerospace company and I have a
question.
Can you measure a projected tolerance accurately using a threaded
hole?
The engineers @ Goddard Space flight center seems to think so...
Is there a method to check this?
Please advise.
Stacy
Stacy,
Projected tolerance zones are most often used on threaded holes, and
yes, they are easy to measure. I detail these methods in my text
books. A short description would be to get threaded gage plugs that
are split up the middle, so that they contract as you thread them
into the holes. This contraction will assure that the threaded gage
plug takes on the location and angle of the threaded hole's pitch
diameter. A CMM probe can then be used to probe the plug at a circle
where the plug is closest to the threaded hole outside of the hole.
Then another circle is probed at the height of the projection. If
both circles reap a center that is inside of the position tolerance
zone, the hole has met its projected positional tolerance zone
requirement. This variables data collection approach will tell you
how far the projected axis of the hole's pitch cylinder has strayed
from perfect (true) position.
If you don't have a threaded gage plug of sufficient height, then
probe it at the base and over whatever height you have and ask the
computer what it would have measured over the correct height of the
projected zone.
Also, functional gages can be designed to accurately give attribute
(good versus bad) data regarding compliance for positional tolerance
zones that are projected.
In my textbooks, I have illustrations and page after page of
explanations on this topic.
James Meadows
Subject: Datum Shift on a Restrained Part
Jim,
Datum Shift on a Restrained Part - Can you legally use "CHECK IN A
RESTRAINED CONDITION" note with a Profile or Position callout with
MMC (shift)? Can you have Shift on a Restrained Part? Sounds like an
Oxymoron or contradiction in terms at first look. Is there a way to
restrain a part and shift at the same time with fixtures (like clamp
on a movable plate) or in CCM?
Larry
Larry,
One thing has nothing to do with the other. Pattern shift or datum
shift as some call it, is an apparent displacement of the pattern of
features from the datum or datums. For example, it means that if a
pattern of holes is positioned to a datum axis, as the datum feature
of size departs from its MMC or virtual condition (as applicable),
the pattern of holes may shift as a group an additional distance
from the datum feature axis. What is actually happening is that the
datum feature axis (axis of the actual hole) has shifted away from
the datum axis (imaginary axis in space that can be simulated by the
axis of a gage pin).
I assume you already know that, but think of the part as not being
inspected in a gage. Think of it being restrained on a plate with
clamps. A Coordinate Measurement Machine can then collect variables
data about the datum feature's hole size and the location of the
hole pattern from the axis of the datum feature. If the hole pattern
seems to be shifted off in one direction more than the individual
position tolerances allow, the additional pattern shift tolerance is
then allowed to see if that is enough to shift them back (as a
group) into their individual tolerance zones. This data analysis can
be done after the part has been measured in a restrained state. All
the restraint does is try to secure the part, perhaps to keep it
from warping during the collection of the measurement data. Analysis
of that data ignores whether the data has been collected while the
part has been restrained or in the free state.
Jim
Subject:
Drawing Interpretation Issue
Hi Jim.
Perceptions are everything.
In the illustration above, my friend, Brad, claims the figure on the
right is correct, given the info in the drawing. Brad says, “Here is
an example of where perception goes wrong. The top hole is B the
bottom hole is C, it has |POS|dia 1.5m |A|Bm| It is very common for
people to believe the C hole is "not to print" in the right view.”
My claim is that because they share the same 'X' plane in the left
view, and the bottom hole is labeled -C-, the right view is
incorrect.
Please advise. Thank you.
Regards,
Ted
Ted,
In this case, Brad is correct. It doesn't matter that the hole
becomes a datum feature after it is positioned to A and B. When C is
being positioned, it has only to be perpendicular to datum A and
located from datum axis B for distance. Provided the distance is
maintained to within its positional tolerance, it can actually
rotate infinitely around the axis of B. Subsequently, I assume datum
C will be used to orient the planes that cross at (and create) datum
axis B. That's when you would orient the rest of the part to this
entire datum structure (A,B and C). In the procedure you have begun,
the next step would be to profile the outside of the part back to
A,B and C. In that way, the rest of the part would be oriented to
the common plane that runs between B and C, and the rotation you
show could only happen within the profile tolerance zone.
Jim
Subject: GD&T Profile Question
Hi Jim
I took a course that you gave several years ago here in the Toledo
area. It was sponsored by the local SME chapter if I recall
correctly. I enjoyed the course but have become a bit rusty over
some of the finer points.
The question I have involves a surface profile. Is it possible to
remove elements from the profile while still retaining the influence
of the control frame over the remaining elements? This is
illustrated in the attached JPEG. We wish to gain tolerance for the
radii of this profile - having them controlled by the drawing's
standard tolerance and have the control frame only apply to the flat
surfaces of the profile. If this is possible, is it necessary to do
anything more than remove the basic block from the radii callout?
Thanks in advance for your analysis and reply.
Greg
Greg,
Removing the basic dimension box from all radii wouldn't be clear
enough to get you what you want. Why not keep what you have and
either 1) Write a local note beneath the profile feature control
frame that says "EXCLUDES ALL RADII" and then make the radii
non-basic dimensions, or 2) Write a local note beneath the profile
feature control frame that says "EXCLUDES ALL RADII" and then call
out a separate profile control with a larger tolerance that says
"APPLIES TO ALL RADII" and keep the radii as basic dimensions?
Hope this helps.
Jim
Subject: Question Regarding Datums
Hello Jim.
I have a statement regarding cylindrical datums that I'd like you to
agree with or refute. There might be some honor involved.
I have a 12.0-12.6 cylindrical shaft that is datum feature A. I have
a cup in one end, 8.4-8.8, and position tolerance of a diameter of 1
at MMC to datum A at MMC. My gage will represent datum feature A at
a diameter of 12.6. On a similar part, I have the same cylinder and
cup sizes, but I can live with a straightness of 0.2 applied to the
diameter on datum feature A. Now my gage is a diameter of 12.8
(virtual condition).
I say that the position of the cup is measured to the axis of -A-,
not to the axis of the actual part. A colleague says "No. You
measure to the axis of the O.D. of the part."
I told him that you always take tolerance measurements from the
geometric counterpart of the piece, the Datum Reference Frame. In
this case (and every case) the x/y planes whose intersection makes
up the axis of the gage to inspect the part is where you take the
measurements from. He asked, "Who do you think you are, Jim
Meadows?"
On another note, I've been reviewing your old newsletters from the
late 90's. Some of those dudes who wrote to you are definitely OUT
there! I wonder if they still are. But the tips are invaluable.
Please respond if you can. Thanks, Jim.
Regards.
TK
TK,
You are correct. The reason you are correct is that the datum
feature is referenced at MMC. That means that the datum feature axis
(axis of the real diameter) may shift away from the datum axis
(imaginary axis) as the datum feature departs from its virtual
condition or MMC (depending on which example you described is being
discussed). The center of the gage represents the physical
embodiment of the imaginary datum axis and is the origin of
measurement. It is quite possible that datum feature A would not be
in the center of the gage.
If the datum feature had been referenced at RFS, you and your
colleague both would have been correct, since the gage would consist
of a contracting gaging element and there would have been no
difference between the axis of the datum feature and the datum axis.
Both would be at the center of the gage.
I can understand why your colleague thought what he did. Without a
gage to measure the part, one would commonly chuck-up on the actual
datum feature and measure from its axis. But, with A referenced at
MMC, he would then have to determine if the part checks bad using
that technique. And if it does check bad, he would have to determine
if the datum feature's departure from its MMC (or virtual condition
as applicable) would allow the part to shift into its tolerance
zone, making it a good part. A gage would automatically do this
shift for the inspector.
Hope this helps.
Jim
Subject: Reporting Profile
Hi James,
I've had the honor of taking a couple of your courses offered
through Chrysler corporation. I'm currently struggling with the
method of reporting the deviation for profile of a surface with many
of our suppliers. The method used at our facility is to double the
maximum deviation form the basic. To keep it simple 1.00 basic with
a profile of .01", part measures 1.004 / .999 reported profile
equals .008.
Is there any "written in stone" method of reporting this value? I've
been to numerous websites and GD&T forums that all express varying
methods of reporting this value. I value your insight and knowledge,
and would appreciate any guidance in resolving this issue once and
for all.
Thanks in advance,
Jerry
Jerry,
It's nice to hear from you. There is no "written in stone" method of
reporting the value of the deviation from the basic profile. I get
this question a lot, so maybe there should be one uniform way of
reporting it. Since there is no standard specifically about
measuring and reporting profile tolerance deviations, and since the
Y14.5 standard is not a measurement standard, there is no final word
guiding us to report this in any one way.
So, as with many situations, you will have to decide as a
corporation the best way to report it and then go about trying to
get all your people and suppliers to comply.
In May of 2007 an ASME Y14 subcommittee was approved to begin work
on a standard that would “standardize” methods of reporting measured
values such as profile. So, this problem is being addressed by ASME.
Good luck.
Jim
Subject: Question Regarding Perpendicularity, Projected Tolerance
Zones and Total Runout
Hi Jim,
My name is Derek and I had a couple of GD & T and stackup courses
from you MI a couple of years ago. I'm currently working for in
Whitehall, MI and have run into a problem I'm hoping you can shed
some light on.
Below I have a simplified version of an armature with a press-fit
pin which rides in a tight-clearance housing. Functionally, I care
about maintaining a consistent gap between the bottom face of A and
the top of C. I need to know the best way to control the armature
print (A) so that the perpendicularity of my press fit hole is held
to the bottom face. My first instinct is to make the bottom surface
datum A, and call out the hole perpendicular to it. However, if I
gage it as close as possible to how it functions, I'd put a best fit
gage pin equal to the length of B in the hole, place the pin in a
V-block, and measure the total runout of the bottom surface of A as
I spin the part.
Can I do this with a projected tolerance zone, or wouldn't this
approach work?
Thanks for any insight you can provide.
Regards,
Derek
Derek,
Either method should achieve what you want, given the proper
tolerances and notes.
I like the idea of inspecting total runout of the bottom face of
part A (while the part spins). The problem that method faces is that
you can't simply put a projected tolerance symbol after the datum
feature you reference in the perpendicularity control on the bottom
of part A. What you could do is, first position the hole on the part
to other datums and give it a projected tolerance zone. Then assign
it a datum feature symbol of its own. Then, when you reference it as
a datum in the perpendicularity control on the bottom of A, you
should probably write a short local or general note to explain what
you explained to me about inspection (To be inspected by putting a
best fit pin into datum feature B that is equal to the length of the
depth of the hole plus the projected tolerance zone height of datum
feature B, then placing the pin into a V-block, and measuring the
total runout of the bottom surface of part A while rotating about
the axis of the gage pin). This type of note isn't absolutely
necessary, but since this is an unusual control, it might expedite
the measurement procedure and assure they are inspecting the part in
exactly the way you feel duplicates the way it functions. Another
option is to show parts A and B already assembled and position pin B
to other datums, then reference B in a total runout control used on
the bottom of part A.
The other option of simply positioning the hole on the part to the
bottom of A and other appropriate datums, then giving it a
refinement of perpendicularity (to the bottom of A) with a projected
tolerance zone is easy and also good. They wouldn't inspect the part
while it spins, but the results should be virtually the same. This
method is more conventional.
Hope this helps.
Jim
Subject: Query regarding Wall thickness calculations
Dear Sir,
We are part of Mahindra & Mahindra ltd. At present we are offering
Engineering services in Commercial Vehicles to Global Customers.
Keeping in view of importance of GD & T we have purchased a set of
12 DVD's on GD & T prepared by you 5 months back. While going
through these DVD's & text book we came across following
difficulties related to Minimum Wall thickness calculations (page
number 198 to 200) related to Fig. 9-24.
Here the Allowed movement of feature D at LMC to C is .130 & again
the same value is used for displacement (pattern shift). As Datum C
is non feature of size, how this effect of allowed movement of
feature D at LMC to C comes in calculation for minimum wall
thickness?
We request you to clarify these points. Waiting for your early
reply.
Regards,
Shrikant
Shrikant,
In both examples datums have been switched. When datums are changed,
error is accumulated. In both these examples, the holes within the
pattern are measured from D. D has a position tolerance of its own.
So, the first .130 is because D moves out of position (to the datums
it is related) the allowed position tolerance (and the holes
measured from it follow D).
The second or .130 is because the pattern of holes positioned to D
are referenced to D at MMC. This MMC symbol after D means D is
represented at its virtual condition to the datum that precedes it
in the hole pattern's position control. Therefore as D departs from
its virtual condition (toward its LMC) the holes as a group can
shift away from the center of D another.130.
You get it twice because of the change in datum reference frames and
the fact that 1) as D moves the hole pattern moves with it and then
2) because of the MMC reference after D, the holes as a pattern can
shift away from D as the D hole grows from its virtual condition to
its LMC.
See the calculation of wall thickness to datum feature C below.
Hope this helps.
Jim
Subject: Question About Converting Inches to Millimeters
Hello James,
I have a question related to design tolerancing. I am doing the
project of converting a product from Inch to Metric. When we convert
inch tol. to Metric, can we convert directly into metric or do we
have any other procedure to convert? For example the hole dim is
3.507/3.515 (inch) and the shaft dim is 3.497/3.500 (inch). Thanks
in advance.
Regards,
Raj
Raj,
When we convert, we convert directly from one unit of measurement
into the other. When we do this, we must be cautious in that there
will be some error in the conversion. If we don't carry it out to
enough decimal places, this error could be a source of problems.
I don't know why people convert at all. It seems like it would be
more accurate (and less work) to simply work in the unit of
measurement that the part was designed in.
James
Subject: Tolerancing questions
Jim:
I was in your course in New Jersey on 22-24 Jan. I sat in the front.
We talked about Feynman, etc.
I have some tolerancing questions.
A major vendor does something repeatedly on their drawings and I
want to know for sure what it means and if they are doing it
correctly.
1)
In the sleeve. (I will fax it to you) they callout an inside
diameter 1.815/1.813 with a total runout of .002 to A, the
centerline. Does the 1.815/1.813 infer it is centered on the
centerline within the .002 or do they need the .002 runout callout
to state this?
They sent me a waiver saying they exceeded the total runout to .0028
but did not say they exceeded the 1.815/1.813. Is this possible the
way this part is dimensioned? If so, how.
I was under the impression that the runout callout usually specifies
a tighter tolerance than given by 1.815/1.813 but this company
frequently calls out a diameter and either circular or total runout
with the same tolerance as the diameter callout. Does this add
anything? (They use circular runout for surfaces without much
length.) Sometimes they use diameter callouts without a geometric
tolerancing box. What is the difference?
2)
The tee end screws onto a bar that sees considerable tension. I'm
concerned that the 1.500/1.495 legs are perpendicular to B, the
center line.
There are 2 position tolerances on the 1.500/1.495 diameter, .005 to
B and .002 without a datum callout. The part exceeded the .005 to B
but not the .002. What does this mean?
The drawings are proprietary, so I can't send the entire drawing.
Thanks for your help,
Paul
Paul,
It's nice to hear from you so soon. I hope everything is sliding
along in greased grooves in your world.
I'll answer question #2 first. The position tolerance of .005, as
you describe it, has not been met for the two diameters in their
positional tolerance (angle and location) to datum axis B. But it
has met the positional tolerance relationship (.002) of the two
diameters to each other. Apparently, the two diameters of
1.495-1.500 are coaxial enough (aligned) to each other, but not well
enough positioned to datum axis B.
The answer to question #1 is that the size tolerance does not
control the centering of the diameter. It only controls how big the
diameter is, and in this case, because it is a tighter form
tolerance than the runout tolerance, the size tolerance controls how
well shaped the diameter is. The size tolerance does not control the
coaxiality to the datum axis A at all. Therefore, any control of how
well centered the diameter is to datum A is toleranced by the total
runout control. Total runout normally control concentricity and
cylindricity. In this case, with the size tolerance so tight, the
total runout control only controls the concentricity (centering) of
the diameter (but it is still inspected as though it is total runout).
This is covered in the Y14.5 standard on Dimensioning and
Tolerancing. In section 2.7, it says the size tolerance controls the
form of a feature of size. For a cylinder, it controls the
roundness, straightness and taper. But it goes on to say in 2.7.3
that the limits of size do not control the orientation or location
relationship between individual features. It says that features
shown perpendicular, coaxial or symmetrical to each other must be
controlled with a tolerance to avoid an incomplete drawing
requirement. Specifically, to your situation, that means the
1.813-1.815 diameter needs a concentricity, circular runout,
position or total runout tolerance (as it has) to show how far off
center of datum axis A the diameter may be.
Hope this helps.
Jim
Subject: Measuring Parts While Applying Restraints
Hi Jim!
I’m from an Army facility.
I was asked about measuring flatness on a part that can be
restrained
for inspection.
One of our inspectors is asking where in the ANSI Y 14.5 does it say
we
can inspect for flatness while we have a part restrained. I could
not
find any specific quote, or paragraph in any literature. Apparently
our
inspector does not have a problem measuring the dimensional
features,
but has a problem measuring the flatness feature in a restrained
condition.
What's your opinion; I don't see anything wrong with restraining the
part and measuring the flatness.
Thanks
Dan
Dan,
The most pertinent standard on measurement is ASME Y14.43-2003. It
does, however, reference Y14.5 in the passages that deal with
restraint. These two standards were coordinated to make the rule as
clear as possible in Y14.43. The key is that unless a note is
written specifying that restraint will be used during measurement,
all parts are measured in the free state. This is due to the fact
that if enough restraint is used, many parts that would otherwise
fail inspection can be distorted into passing. Distortion of parts
to obtain compliant measurement results is forbidden. If the
restraint used does not distort the part in a manner that
significantly changes the measurement results, then restraint may be
used. So, restraining a very rigid part may be okay, while
restraining a flexible part would not be okay.
See the attached page from Y14.43 for the rules in 2.8.1, 2.8.2 and
2.8.3.
Hope this helps.
Jim
Subject: A question Regarding Hexagons.
Hi Jim,
I hope all is well with you. I am a former student of yours and I’m
looking forward to your Comprehensive Advanced GD&T course in
Nashville in December. I have all of your books and I appreciate
your immense knowledge on all things GD&T. I named my first child
Jim Meadows. I think it's a nice name, but my wife is afraid she'll
get picked on by mean kids. Anyway...
A colleague and I are having a difference of opinion and I'm hoping
you could help us out. What we have is a part with an internal
hexagon bore (think socket head) cut into it. It is dimensioned as
".314 +.010/-.010 Hex" across the flats and it is given a depth and
positioned on a centerline. Is the dimensioning of this feature
complete? Do not consider design intent and assume there is no
general note regarding corner breaks.
One opinion is that the feature is fully dimensioned, and that an
acceptable part feature would be an internal hex - no part of which
violated the boundaries of two perfect hexagons at .304 and .324.
For instance a hex bore that was .324 across the flats would no be
allowed any straightness error, but rounds on the points would be
permissible so long as they never violated the perfect hex at .304
boundary. The thought behind this is that size limits control form
and they do so no differently on a hex bore than they would on a
cylindrical bore.
The other opinion is that insufficient details were provided by the
print - that a hexagonal bore is not one single feature and that
both the distance across flats and the allowable radius or break in
the corners must always be dimensioned. A print that only shows a
dimension across flats and a depth of hex must be rejected as
incomplete.
What do you think?
Thanks,
Mike
Mike,
In ASME Y14.5M-1994, in section 2.7.3 there is a rule that applies
here. It comes under the heading Relationship Between Individual
Features and goes something like, The limits of size do not control
the orientation or location relationship between individual
features. Feature shown perpendicular, coaxial or symmetrical to
each other must be controlled with a tolerance to avoid an
incomplete drawing requirement.
You can look it up to get the exact quote, but that's it within a
couple of words. The essence of the statement is that a feature of
size is cylindrical, spherical, two parallel line elements or two
parallel planar surfaces. And that your feature of size which is
several sets of "two parallel planar surfaces" are each controlled
for form (flatness, straightness and parallelism), but they aren't
related to each other, unless you say to within how much in a
control other than just a size limit. If there is a general
tolerance note on the drawing that says, Unless Otherwise Specified,
All Angles Are +1 degree (or some number of degrees), that would
relate the sets of parallel surfaces to one another to within that
tolerance. But even then, we would have to make certain that was an
acceptable amount of tolerance and then what about the location of
the hex on the rest of the part. Is it supposed to be centered to
some diameter, like the hex head on a screw is supposed to be
centered to the diameter of the screw? Or, are there other diameters
or widths or edges it is to be located to?
Usually, if such a feature is important enough to ask a question
about, as you have, it is important enough to completely dimension
and tolerance. I don't think a size tolerance is a complete
definition of the hex. I think you could position each set of
parallel surfaces to each other and to a datum reference frame by
simply applying a position control to the 3X .314+.010 dimension.
If you wanted to get really crazy, you could make the .314
dimensions basic then profile the hex all-around to a datum
reference frame (a complete set of datums).
That's my opinion. I hope it helps. Tell your daughter that I'm
sorry.
Jim |
