|
Readers,
As many of you know, I have no real schedule as to when a new
newsletter comes out. It has a lot to do with a mix of my time in
the office and the batch of letters written by you with clear,
important questions others might be interested in reading. Well,
the stars were in alignment a little earlier than usual this time
around, so here is the latest installment of the continuing saga of
The Tolerancing Engineer (serving the GD&T community since 1982).
James D. Meadows
Editor
Subject: Compound Datum Question
Dear Mr. Meadows,
I have a question maybe you could answer. If you position a hole (X)
back to a compound datum (A-B) with MMC on both datums, do you get
the bonus tolerance for the position of (X), from datum A and datum
B or just the one datum that is furthest away from the MMC
condition? In this question, datum A and datum B are holes on a flat
part. Hole (X) is positioned back to the compound A-B.
Chad
Chad,
What you are entitled to is what is called a pattern shift/datum
shift which is different than what is commonly referred to as bonus
tolerance. Pattern shift refers to the pattern of holes positioned
to the datums moving as a group. Bonus tolerance refers to the
individuals holes in the pattern each receiving an additional
positional tolerance.
A somewhat simplified answer would be that you get the smallest
amount of pattern shift from only one of the two datum feature
holes. But it is actually a little more complicated than that.
Since both holes generate a central datum axis half way between
their virtual condition boundaries, the best way to think about it
is that you have two gage pins on a plate made at the virtual
condition size of the datum features. As the actual datum feature
holes grow around those gage pins, the amount of pattern shift for
the holes that are positioned to them is derived from the amount the
part could actually shift around on those gage pins. This would
simultaneously control pattern shift and pattern rotation.
Hope this helps,
Jim
Subject: Converting Plus and Minus Tolerancing to Geometric
Symbology
Hi, Jim.
I was a student in your recent GD&T class in Milwaukee this past
May. I've
taken a drawing and converted it from plus/minus tolerancing, to GD&T.
This
is my first attempt at GD&T with a part made by the company I work
for.
Could you take a look at the AutoCAD attachment and see if what I
did makes
any sense. We are locating 3 light emitting diodes (LD1-LD3) on a
circuit board with respect to the centerline of the three .115-.125
holes. I would very much
appreciate any advice and comments you would give.
Thank you
Chris
Chris,
First of all, you need to stabilize the part by laying it on the
surface with the most surface area. That should be your primary
datum feature. None of the features you have selected have enough
surface area to stabilize your measurements.
The edges of the part you have chosen to position the holes to (A
and B) would make good secondary and tertiary datum features after
you have stabilized the part onto the primary datum feature.
Then, there is a passage in the Y14.5 standard that says: Datum
features are identified on drawings by means of symbols. These
symbols relate to physical features and are not applied to
centerlines, centerplanes or axes.
So, if you want to make one, two or all three of the .115-125 holes
datum features (such as a pattern datum consisting of all three
holes), you can. Then you can reference (position) the diodes to
the primary stabilizing datum and the datum pattern of three holes.
But you can't draw a centerline between the three holes and label
the centerline as a datum plane. That is illegal.
Jim
Subject: Composite Position Tolerance Question
Dear Mr Meadows,
Assume we have defined A, B, C datums. We have 4 holes with
Ø.164±.010. In the first case, we define the upper segment of the
composite position tolerance as Ø.080 with respect to datums A|B|C
and lower segment as Ø.008 with respect to A. In the second case,
the upper segment is the same, but the lower segment is Ø.008 with
no datums. What will be the difference in the meaning of these two
cases?
Thanks in advance,
Best regards,
Huseyin
Huseyin,
Both of the Composite Position Tolerances you describe control the
location of the holes to the datums to within the larger position
tolerance of .080. Both also control the hole to hole position
tolerance to within the smaller position tolerance of .008.
The control with the A referenced in the lower level feature
relating tolerance zone framework (FRTZF) of .008 refines the
orientation of each hole to datum A. If the orientation depicted is
perpendicularity, then the perpendicularity is refined to within
.008 to A. And, of course, the control that does not reference
datum A in the lower level (FRTZF) control does not refine the
perpendicularity tolerance to within the .008, but instead holds it
to within the larger pattern locating tolerance zone framework (PLTZF)
of .080.
Hope this helps.
Jim
Subject: Primary datums and form
Jim,
If the primary datum feature is a sphere or a width type should only
a size tolerance be applied? Should circularity be applied to the
sphere?
Todd
Todd,
This is an interesting question. Since spheres aren't all that
common as primary datum features, Y14.5 has never assigned a
geometric characteristic symbol specifically for them. On the other
hand, just as straightness in all directions controls flatness,
circularity in all directions controls "sphere-icity". So, that is
one option. Another (Option 2) is that you abandon the plus and
minus size tolerance and assign it a basic dimension for size then
apply a profile of a surface control. This would control size and
three-dimensional form. That's another option. The third (Option
3) is that you do what you originally said and just assign the
diameter a plus and minus size tolerance and rely on Rule #1 to
control both size and form. A sphere is one of the shapes that have
always constituted a feature of size and has always fallen under
Rule #1. Personally, I like Option 3. But it falls apart if you
want the size tolerance to be larger than the form tolerance.
Widths are also interesting. Straightness of the derived median
plane is an option. But, in fact, that could make it worse than
just letting the size control the form. Straightness of the derived
median plane releases you from Rule #1 and would allow the feature
to bow even at MMC. I've tried both options and don't like the
straightness control much in this situation. So, even though both
are available, unless the size tolerance is huge (and for primary
datum features, it usually isn't), I prefer to let the size control
the form. As an odd, out of left field option, it is also possible
to assign the size dimension as a basic dimension and with leader
lines pointing at both surfaces of the slot, assign it a profile of
the surface control. This would control the size and form all
within the profile tolerance for each surface.
These are difficult decisions. I hope this helps.
Jim
Subject: Use of Profile Tolerance Using a Center Plane Datum
Jim,
I am checking a part with a GDT condition that I believe to be
erroneous but am assured that is correct. Without a drawing I will
try to adequately explain the callouts.
The overall width dimension of the part is a feature of size +.030
-.010 and labeled as a datum D.
On the top surface a rectangular cutout is dimensioned using Basic
dimensions for the length and width of the cutout. There are no
locating dimensions from any edge, surface or whatever. There is a
profile tolerance with primary, secondary and tertiary datums using
the above D datum as the secondary datum (at MMC).
This approach is assuming the profile tolerance locates the cutout
symmetrically about the datum D therefore not requiring location
dimensions for the cutout. I have never seen anything like this
before. Is it acceptable?
Thank you for your input.
John
John,
Yes, it's fine. The fact that you were able to interpret the
drawing requirements without confusion is the proof one needs to
determine the drawing is correct. Since I don't actually have an
illustration to go by, I can't say for certain the drawing is
correct, but from what you have described, it sounds fine to me.
Using centerplanes for locating at a basic implied zero dimension
for either symmetrical or coaxial situations is really quite
common. See pages 123 and 378 in my yellow hard cover text book for
examples of position and symmetry being used to locate features in
the middle of datum features of size. Profile is allowed to do the
same. Profile of a Surface is more versatile and powerful than
either position or symmetry (both capable of controlling angles and
location), so has their capabilities and more (Profile of a Surface
can control all four things that geometry is capable of; 3D form,
size, angles and location--and it sounds as though in the case you
describe it is doing all four).
Jim
Subject: GD&T / Inspection Questions
Jim,
Hope business is good! I have some questions regarding complex
plastic parts:
1) On complex surfaces/ profiles in which you would want to use
a profile control, what is the industry common inspection technique?
(Our manufacturing reps are looking to learn how to do this.)
2) Minimal dimensioning and the use of profile. We are wondering
if we can call out profiles and then not fully dimension them on the
drawing (force a referral to the CAD file), your thoughts here?
3) Can you point me to some specific drawing examples, on any of
this?
4) Where do we look for metrology standards?
Thanks for any help or advice you can give here!
Brad
Brad,
1. Commonly complex surfaces that are profiled are inspected with
CMM's. It depends on how large they are. There are some pieces of
equipment with the capability of scanning the surfaces of smaller
parts with lasers and mapping the surface by digitizing thousands of
points and comparing them to the CAD model. Even CMM measurements
work better with a scan probe (either contact or non-contact) in
that with 3D surface controls such as profile, many points are
required to have a sufficient level of confidence that you have met
the profile tolerance specifications.
2. If you look in my yellow hard cover GD&T book on pages 148 and
150 (and many more in the workbook in the answer book section of
chapter 6) there are what the automobile industry calls "GD&T
sheets". These have an isometric illustration of the part and all
of the GD&T (the datum features and the geometric tolerances), but
very few other dimensions. References are then made to the CAD
model or other orthographic view drawings to get the rest of the
dimensions required. The common reference is that "UNLESS OTHERWISE
SPECIFIED, ALL CAD DIMENSIONS ARE CONSIDERED BASIC."
3. Answered in #2 above.
4. Metrology standards are commonly designated as B89 standards. I
am a member of the B89.3 committee. B89 stands for "Measurement"
and .3 stands for "of geometry". Any standards that begin with B89
will address certain facets of measurement. For example, B89.3.1
deals with the measurement of out-of-roundness. For more available
B89 standards, you should probably just go to the www.asme.org
website and browse through their standards.
Hope this helps,
Jim
Subject: GD&T Question - True Position Located With Non-Basic
Dimension
Hello Jim,
I attended the GD&T training and Tolerance Stack-Up Analysis
training sessions that you conducted last summer. I would
appreciate your feedback on a GD&T question that came up during a
recent design review:
Does ANSI Y14.5 always require that the true position feature
control block be located with basic dimensions?
As you can see on the attached drawing, the 0.25 true position of
the 4.88 thru hole is located with a non-basic dimension of 5 +/-
0.5 (the +/- 0.5 tolerance for this dimension is specified in the
general tolerance block that is shown on a different area of the
drawing). I would contend that this dimensioning scheme is
incorrect because the true position must be located with basic
dimensions. Am I correct?
Thanks for your help.
Best regards,
Kevin
Kevin,
Yes, Y14.5 does require that basic dimensions be shown from
specified datum features in such situations. The illustration you
sent is just a small portion of the entire part, but it looks like
what they want to do is to make the axis of the hole being
positioned intersect and be perpendicular to the axis of the (datum
feature) diameter it is drilled into. That is perfectly legal.
Then it looks like they may want a larger tolerance to apply to the
dimension from the surface you have questioned. I can't really tell
from the little piece of the drawing you sent whether that is one of
the datum features or not. If it is, the dimension should be
basic. Technically they can't do otherwise. But to do it legally,
with a larger tolerance of position to the plane formed by that
surface than to the datum axis would involve a two single segment
position control (one level ultimately responsible for the tolerance
to each datum). I have just such a position control shown in my
workbook for the answer to page 15-10. If you look at it, you will
see that it is fairly involved looking. Still, whatever surface is
datum feature A would need a basic dimension from it to the hole to
constitute a legal drawing (as shown from datums D and C in the
answer to page 15-10 below).
An illegal drawing may just want to leave the hole positioned to
the datum axis (of the diameter it is drilled into) and show a
separate plus or minus toleranced dimension from the planar surface
that would (in this less than perfectly legal approach) not be
specified as a datum feature.
Hope this helps,
Jim
Page 15-10 (See 19.5 Basic Dimensions from D and C)
Subject: Pattern Datums and True Position
Hi Jim,
The last time I saw you was when you came to my previous company in
Colorado to give a GD&T class. I tried getting you back for the
advanced class, but there wasn’t enough money. Well, I'm no longer
working there, I was laid off. I am now working at another company
in Colorado. I’ve been trying to get them to bring you in here
too. This is a much better job with much more challenging
geometries.
On to my question. I've attached a few files for you to see. There
is a part and an assembly print. There are 2 versions of each
print. A group of engineers here have been arguing over the best
way to accomplish this for the last month or so. The object we are
trying to achieve is to control the position of the 4 posts (on the
assembly print) as a pattern/group. The posts position is dictated
by the counterbore on the part. The second objective is to control
the position of the conical plugs (divots - item 4 on assembly
print) relative to the pattern of posts. The divot placed on the
front face should be at the theoretical center of all the posts.
Method one creates an origin to the pattern and controls the 3 other
holes from the origin one. Method 2 makes the 4 features datum B,
then assigns additional datums to define inspection instructions.
Some feel method one introduces more stack-up. Obviously we want to
avoid that if that is the case.
I've read your section on "pattern datums" (page 86 & 121, in your
GD&T book) and section 16.3 (pg 487, implying a manufacturing
sequence and using compound pattern datums) and I have had a few
other engineers read it too. After all that, we still can't figure
out the best scheme. The 2 versions I sent are based on the
preference of our quality guy, and the preference of a senior
engineer.
Because we still haven't solidified our scheme, there are some
errors on the geometric tolerances (missing diameter symbols, no MMC
callouts, and so forth).
A little background on the parts. These are used during hip/knee
replacement surgeries and act as a reference frame for the position
of the patient’s bones. The assembly is screwed down to the
patient. There are reflective spheres that snap on to the posts. A
machine transmits infrared signals, and the spheres rebound that
signal. The system then can extrapolate the location of the
patient’s bones. All the tools the surgeon uses also have spheres
on them. All this data is then displayed on a computer screen. The
surgeon can look at his screen and see his tools relative to the
patient. The divots are used to calibrate the location of the
spheres during/before surgery.
Thanks for any help you can provide.
Victor
Shown below is one version of the four tolerancing approaches that
Victor sent.
Victor,
I'm sorry in advance for this response. It will be brief. I'm
swamped. I've been in town since Friday and have spent the entire
time working on a project I'm consulting for.
All of the options are viable. The ones that use a pattern datum
are only easily viable if datum pattern B is referenced in
subsequent controls at MMC. I will explain this more later. I like
the options that use secondary and tertiary holes as datum
features. They can easily be measured with or without a fixture or
gage. It has a very stable primary datum feature (4 surfaces for
datum feature A). The flatness control is not correct, though. If
there are 4 surfaces, in order to make them coplanar (as well as
flat) they need a profile of a surface control. The secondary datum
feature is one hole held perpendicular to the primary datum. The
tertiary datum feature is a hole positioned to the primary and
secondary datums. Then three other holes are positioned to the
three datums and the periphery is profiled to the three datums.
This is a simple and popular tolerancing methodology used throughout
the world in a wide variety of industries. The threaded holes are
held coaxial to their Individual counter bores (you need to write 4X
INDIVIDUALLY beneath the positional control). Is there any chance
that the two upper holes that are aligned with one another may be
selected as secondary and tertiary, instead of the ones on a
diagonal to one another? It will save you a lot of explaining.
Datum feature holes on a diagonal are not the easiest things to
interpret on a drawing. The weakness of the "secondary and tertiary
holes as datum features" approach is that all subsequent features
are only related directly to two of the holes, instead of all four.
And as you said, there is a chance for an accumulation of tolerance
error that is not possible with the pattern datum approach. There
are ways around this. Take a look at pages, 329 and 517 in my
yellow textbook (or page 17-5 in the yellow workbook). There are
many variations on that theme (for example, instead of positioning
two of the holes to one another and to datum A as page 517 and 17-5
does, you could do something similar to what page 329 does and use
perpendicularity on the first hole, then position on the second
hole-which could become the tertiary datum feature-then position and
profile everything else back to these datum features (A, B & C) as a
simultaneous requirement (all part of the same pattern to be gauged
with the same gauge).
There are some oddities with the tolerancing schemes you show. For
example, do the counter bores actually locate the part, or are you
just using them as the datum features because threaded features are
hard to establish a measurement from? Should the threaded holes use
a projected tolerance zone? Still, this is a good approach.
963-864 has a strange primary datum feature on both drawings.
However, if the tops of those pins actually dictate the stability of
the part in the assembly (body?), and act as the seating surface for
this interface, then they would be most appropriate (I hope not, in
that they don't make as attractive and stabilizing a primary datum
feature as other features on the part). If used, they also would
not use flatness, but coplanarity using a profile of a surface
control.
The secondary and tertiary datum feature holes are the most common
approach, but lose some of the power of a pattern datum. A pattern
datum of 4 holes has the strength of relating all holes to one
another and then you can relate all other features to all holes by
just referencing (A for orientation, then) B for location. The
advantage of using a pattern datum is its power to relate all
features to all others without accumulated error. The disadvantage
of a pattern datum is it is difficult (almost impossible) to measure
without a fixture or gage to represent the pattern datum. One note
on that is that unless the pattern datum is referenced at MMC (B at
MMC) in subsequent feature control frames, the fixture or gage would
have to have expanding pins to simultaneously engage all 4 holes at
once. So, my advice is to either reference B at MMC (so they can be
represented at their virtual condition size in gages or fixtures) or
get rid of the pattern datum. In your drawings that use the pattern
datums (on 963-864 and 963-864-01) a datum feature C is then
established (and very oddly on one of the drawings). I can't figure
out what good it does. If you stick a fixturing pin in all four
holes while the part rests on datum feature A, all spatial degrees
of part freedom are eliminated. Therefore, a datum feature C is
unnecessary. Either way, this part like the last would need a
profile of the surface for the part periphery (unless that is
handled at another drawing level).
I don't have any more time today, and tomorrow I'm off to work on
the war machine (military base). If you have more to discuss, write
back and I'll try to get to it when I return.
Good luck,
Jim
Subject: Design and Manufacture of Fixtures and Gages
Dear Sir,
Would you please suggest a book on Designing and Manufacturing of
Fixtures and Gauges for the Geometric Dimensioning and Tolerancing
parts? We are particularly interested in learning the gauging
strategies to be followed for the manufacture or gauges to check the
parts which are Geometrically Dimensioned and Toleranced.
With Regards,
S.Rathinasamy
Mr. Rathinasamy:
There is a standard that was published in 2003 entitled ASME
Y14.43-2003-Dimensioning and Tolerancing Principles for Gages and
Fixtures. It is 101 pages long and costs $75. It can be purchased
at www.asme.org in their codes and standards publications section.
James D. Meadows
Chairman Y14.43
Subject: Countersunk Screws in Tolerance Stack-ups
Jim,
I just took your Tolerance Stack Up Analysis class in Milwaukee and
have a fastener that we did not cover. I need to do a tolerance
stack up where flat head (countersunk) screws are to be factored in.
Knowing that the point of contact will be between the angled surface
under the screw head and the angled face of the mating countersink,
is it even necessary to consider the tolerances accrued between the
clearance hole and the side surface (major diameter) of the screw,
or would I only consider the tolerances that affect the position of
the screw hole and ignore the gap between the screw's major diameter
and the mating part's clearance hole? What do I do in an instance
where the screw may not be perpendicular and the countersink may
only be locating on a single side?
Thank you for any help you can offer.
Tony
Tony,
It's a good question. Technically, countersunk holes constitute a
"double fixed fastener assembly" condition. The threaded hole tries
to center the screw and the countersink tries to center the screw
and since both can't, one fails. The one that fails is the
countersunk hole and that is why the screw ends up with its head
resting on only one side of the countersunk hole. Although once the
countersink engages it does lock the part more firmly into place,
what I consider important is what happens before the countersink
engages. Since the ability to assemble is not dependant on the
countersink, but rather the clearance hole and the screw mounted
into the threaded hole, I ignore the countersink and do my tolerance
stack-up. As you said, the screw may rest on only one side of the
countersink, which means the clearance hole and the screw mounted in
the threaded hole have made it do that by how each is positioned on
its part. The countersinks get there too late to have an effect on
whether or not the parts assemble. So, they must follow what the
clearance holes and the mounted screws dictate. That often results
in the screw head seating on one side of the countersink and maybe
not even entirely buried.
Hope this helps,
Jim
Subject: Threaded Holes and Their Chamfers
Jim,
My colleagues have a part that is threaded into another and stops on
a shoulder. There is a requirement for some wires on the opposite
side of the part being threaded in to have a certain angular
orientation. They want it to engage in a different attitude, I guess
is the best way to describe it---the wires need to be 90 instead of
say 60 degrees.
So---the theory is---put some more chamfer on the thread--it will
engage in a different angular orientation.
What do you think?
Greg
Greg,
That's a very odd theory. I've never heard of it before. Not that
it couldn't work. I really don't know. It just sounds kind
of...makeshift and unprofessional, like they are trying to make
something that has been either poorly designed or poorly
manufactured to work anyway. It seems they would want a more
permanent fix.
Jim
Jim,
I agree.
Greg
Subject: Question on Using Both Inch and Metric Tolerances
Jim,
I have a question not directly related to GD&T but it does have to
do with Tolerancing.
And engineer here wants our metric and inch standard tolerances to
match. So he wants the 3 place inch tolerance of +/-.005 to match
the 2 place metric tolerance of +/-0.10. We, as designers, think he
is a little off his rocker. We know that metric and inch do not
match directly when converted. I would much rather add and subtract
whole number, such as .005" and 0.10mm that .005 and .13mm.
So, what I am wondering are thee any standards that I can look at
that will help me explain this to him. He has gone and put in, what
we call a corrective action, and that means I have to search out all
possible answers. I have looked in all the books I have and have
found nothing. If I can find a standard for anything like this it
would help me greatly.
I enjoyed your GD&T class very much. I’m looking forward to taking
another class with you in the future.
Jeff
Jeff,
In previous versions the Y14.5 standard on Dimensioning and
Tolerancing it was allowed to put both metric and inch tolerances on
the same features. Usually they were separated by a / (slash) or
one of the tolerances was put in brackets. This got into a legal
problem where parts would meet one tolerance, but not the other.
So, in later revisions of Y14.5, that practice was abandoned and it
was determined that parts would have tolerances specified as either
millimeters or inches, but not both.
The problem, as you point out, is that the two tolerances are not
usually exactly equivalent.
I am unaware of a standard that tells you how to deal with this,
other than as described above. Choose one, either millimeters or
inches, and go with it. If those encountering your designs have to
do some converting, leave that up to them, but let the drawing stand
alone as the legal last word without ambiguity.
Hope this helps,
Jim
Subject: Clarification on Chapter 6a from your Tolerance Stack-Up
Book
Dear Mr. Meadows,
I recently purchased this book and found it very relevant and
interesting.
May I ask you a question? While going thru chapter 6b (Max overall
dimension for crankshaft assembly: factors and non-factors); the
calculations did not account for center bore/shoulder's
perpendicularity callout and the calculations did not calculate VC
and RC boundaries for center bore/shoulder.
As per ASME, virtual conditions do apply (apart from position
tolerance) for other controls such as orientation. So, why this
exercise did not account for perpendicularity? Isn't that a factor?
In the first chapter, you mentioned that this book does not account
for out of straightness situations? Is this one among them, like the
feature tend to lean OR just because the length of center bore /
shoulder is small therefore there is no chance of out of squareness
relative datums?
I guess, by accounting orientation tolerance, the max overall
diameter could change.
I request your views on this.
Regards,
Raj
Shown below is the Two-Part Assembly Raj
is referring to from my book on Tolerance Stack-Up Analysis
Raj,
The technique you are asking about is one that takes into
consideration only the factors that would contribute to the maximum
overall gap/housing requirement for the two part assembly being
analyzed. If the central bore and shaft were
out-of-perpendicularity, the slide of one part up would be less (and
the overall housing requirement smaller) than if the bore and shaft
(datum features B and D) were perfectly perpendicular. We were
looking for the maximum gap/housing requirement, therefore wanted
the most clearance between the bore and shaft. This occurs when the
bore and shaft are produced at their LMC and perfectly perpendicular
to their primary datums.
As far as referencing ASME Y14.5 to tell you what and what does not
apply, you can forget that. This stuff is light years ahead of what
Y14.5 is going to tell you how to do. Think of Y14.5 as a
dictionary that tells you the meaning of all the symbols and what
the general engineering documentation rules are. Tolerance stack-up
analysis will require analytical reasoning and a careful
consideration of what is physically possible, which is what the end
of chapter 6 and all of chapter 7 (as well as all of Chapter 9) is
about.
You pick a tolerance stack-up analysis approach (hopefully from the
several I explain in the book), employ it, reason out which
dimensions and tolerances contribute to the gap you are analyzing
(and which do not), work the method, get an answer, then stop and
think about any other contributors could come into play that you
have not considered yet. Draw extra pictures. It always helps.
See chapter 8 for some of these final considerations. And good
luck.
Jim
Dear Jim,
Thank you very much for the detailed reply. I really appreciate your
time writing so much in detail. In fact after going thru chapters 9,
it was more clear.
I enjoyed the last chapter on statistical tolerancing; especially
reintegrating statistical tolerances back into the assembly. I am
interested to know more on this and please let me know if you have
more material for sale on this.
Best regards,
Raj
Subject: Translating Statistical Analysis Results to GD&T
Controls
Hello Jim,
My company utilizes tolerance stack-up analysis in our mechanical
designs. Our products range from handsets to PCMCIA type wireless
devices. Many of our engineers started their ME careers at Motorola
which exposed them to 6 Sigma & tol-stacks. The trouble we're having
right now is understanding how to calculate boundaries for GD&T
controls, MMC, LMC, etc., in order to "enforce" our tolerance
stack-up analysis. The tolerances for the inputs in our tol-stacks
are bi-lateral...positional tolerance zone is cylindrical...how do
we translate the results from statistical analysis to GD&T controls?
I noticed that you have a new book on Tolerance Stack-up Analysis.
My guess is that this is the resource we need to answer our
questions. I've taken your Applications-Based GD&T Video Training
Series course while working at Denso International America in '00.
Your accompanying GD&T textbook and the corresponding workbook are
awesome...the best practical texts I've ever used. My hope is your
new book on tolerance stack-up analysis will be just as useful.
Sincerely,
Tony
Tony,
The first rule I set in my book and the courses I teach on Tolerance
Stack-Up Analysis is that in order to find any unknown, you first
must know what you are looking for. Tolerance Stack-Up Analysis
should begin by setting up a route of pertinent numbers to determine
an unknown quantity. That Gap might be minimum or maximum
clearances or interferences, overall housing requirements, anything
really. But to find it you chart the route. The route consists of
a series of toleranced features. If some have geometric tolerances,
you must decide which, if any, of the geometric tolerances are
factors. Once you decide that, if none of the geometric tolerances
are factors, you average the MMC and LMC of the features to convert
them to equal bilaterally toleranced dimensions to be plugged into
the route/circuit being run. If a geometric tolerance, such as
position or perpendicularity is a factor, you first calculate the
inner and outer boundary of the collective effects of the size
limits of the feature and the geometric tolerance that applies at
that size. These pertinent inner and outer boundaries are then
averaged to find their mean dimension and the equal bilateral
tolerance that surrounds it. Then these numbers are plugged into
the route just as though they were plus and minus toleranced
dimensions. Routes or circuits that are run are oriented to be X or
Y routes, but not X and Y. Therefore, for the Gap you are trying to
calculate, it doesn't matter that the geometric tolerance zone is a
cylindrical zone. When looking for a worst case Gap, only an X or Y
is being calculated at one time.
If the route is to be calculated using Statistics, instead of worst
case, you just decide which statistical methodology you believe in,
for example Root Sum Square, Root Sum Square with a safety factor or
Monte Carlo methodologies, or even data that you have tracked for a
particular manufacturing procedure. Then employ that method to
calculate the likely amount of tolerance to be used during
manufacture.
Depending on what you wish to do with that data, you can go several
ways from here. Maybe that's all you wanted to know, so you just use
the data you have determined is the likely amount of tolerance to be
consumed by manufacturing. Another avenue is to use that number
(commonly referred to as the "natural tolerance") to increase the
tolerance for the individual features that were part of the route
you used to calculate the Gap. In my book, I show you methods for
calculating this increase in tolerance and reintegrating this
greater Statistical Tolerance back into the assembly. When a worst
case Gap Analysis is done using the increased Statistical Tolerance
you have just assigned, you will find extreme numbers that
(depending on the type of Gap you calculated) might allow
interferences. But when you run a statistical analysis of that same
route, you will find that even with the tolerances increased, you
are likely to consume only the originally available arithmetically
calculated tolerance and that the interferences are unlikely to
occur.
As you probably already know, this is a difficult and involved
topic. The good news is that I have explained it all in my book on
Tolerance Stack-Up Analysis. The bad news is that it took me 350
pages to do it and I can't do it justice in the space I allocate for
an email answer. The most pertinent chapter for statistics is
chapter 11 (which is entitled Statistical Tolerancing).
Thanks for the compliments on my GD&T books. I really appreciate
them. I think the answers to all of your questions on Tolerance
Stack-Up Analysis are covered in my book on the topic. The truth is
that it is a very numbers intensive subject. I've written the book
to be useful as a self teaching text, but you could learn it much
faster if I was there to teach it to you. Please consider an
on-site course for the most expedient learning process.
Jim |
