|
Subject: Tolerancing a Potato Chip
Jim,
In today's world of mathematical models and the kids that run
these Catia
stations you never know what they are capable of drawing ....producible or
not!
What I have not seen in the Foster books or the Y14.5M 1994 is 2004 technology? With air vehicles looking like potato chips....there seems
to
be BIG questions and ambiguity even among BIG companies dealing with
advanced programs of how to deal with GD&T and Mathematical surfaces.
Can
you shed any light on the logic of applying tolerance to complex
surfaces
relative to the 'normal' holes that pierce these parts?
Thanks,
Roy
Roy,
Everyone believes that tolerancing oddly configured
parts is extremely difficult because the shape is complex. As an old
die maker that was raised on automobile panels, I don't think it's anymore
difficult than other more common shapes. First of all, datum targets
can easily stabilize the oddly configured part and form the coordinate
system (datum reference frame) that any holes are to be related to.
All you have to do is show their basic relationship to the imaginary datums
constructed by the targets (usually done in the CAD model) and then assign a
position tolerance to the holes or a profile tolerance to the free form
surface. In the automobile panel industry, datum targets are usually
used to establish a primary datum plane, a round hole is used to establish a
location axis (secondary and tertiary datum planes construct that axis) and
a slot width or another round hole establishes the tertiary datum feature
(fourth datum plane used to orient measurements). Once the datum
reference frame is established, all the tolerancing person has to do is show
the relationship of all features to those three planes and give tolerances
(usually tolerances of profile or position).
To be honest, I have always thought this type of part
was actually easier to tolerance than simple geometries in that you usually
follow the format described above. There were less choices to make.
Datum targets, position of holes, profile of the free form surface.
Not that I'm promoting it, but in the 1994 version of
Y14.5, it even allows for these free form mathematically defined surfaces to
be used as datum features, as long as you show in the CAD model how they
form a coordinate system from which to measure other features. The
holes in the free form surface are related with basic dimensions and angles
to the coordinate system and tolerances on this ideal relationship added in
the form of Position tolerances (or whatever geometric characteristic
relationship best describes the situation).
The goal is to stabilize the part, form imaginary datum
planes or axes from physical features, then relate everything to the datums
with geometric tolerances.
Now, I know these oddly configured parts are harder to
manufacture than a washer or a rectangular block with holes in it. But
that is a manufacturing difficulty that every maker of air foils, hip or
knee implants, automobile panels, (potato chips), or any free form surface
has to deal with. It is the nature of the parts they have chosen to
specialize in. But harder to manufacture, doesn't necessarily mean
harder to tolerance. I have a section in my textbook and workbook on
Geometric Dimensioning and Tolerancing that deals with sheet metal, plastic
molded parts and
free state
variation in flexible parts. I teach an entire course called,
Geometric Dimensioning and Tolerancing for Flexible Parts at
Daimler/Chrysler Corporation and other companies and have for years now.
Maybe being a journeyman die maker trained on these types of parts in my
youth gives me a different perspective. But, I don't think they are
harder to tolerance, just harder to manufacture.
In fact, if you think of a part with no holes at all
(holes make great datum features on complex configurations), a Profile of a
Surface All Over control can be used to just wrap the CAD model of the part
up in a tolerancing blanket that follows the basic configuration of the math
CAD model and forms inner and outer tolerance zones for the potato chip
parts. Datums can be thought of as optional. In inspection, the
part is scanned by a probe, all scanned points compared by a software
package to the CAD model, and the part determined to be either in or out of
tolerance. You can build fixtures to hold the part in a restrained
condition that duplicates how it fits into the assembly (if appropriate)
that reflects the detailed datums and restrained condition note on the part
drawing.
Or if you need to see how much spring back you are getting
out of a pressing operation, to determine if the die needs reworking, you
can make it clear that your first measurement is to be taken in the
free state
. If the spring back is acceptable, and the part is to restrained in
the assembly, you can add a "to be inspected in a restrained state in
the following manner" note to the drawing for all subsequent
measurements. The note should be as detailed as possible to describe
exactly how the part is restrained by the assembly, to make certain it is
restrained in the same manner when it is inspected.
All parts are able to be toleranced. I've worked
on parts that are so flexible they melt if you touch them. That just
means I added a note to the drawing explaining to the manufacturing and
inspection personnel that the part could not be touched due to the heat of
the human body.
I hope this helps.
Jim Meadows
_______________________________________________________________________
Subject: European GD&T
Jim,
I am looking for reference guide
for the differences in the tolerance standards between the
Germany,
France,
England
and
USA.
Can you give me a source.
Thank You
Terry
Terry,
I am unaware of a single document that spells out the
differences between the four standards you mention. To be honest, I
doubt such a document exists. The only thing I can think of is to
contact ANSI in
New York City
and see if they sell those standards.
Jim
_______________________________________________________________________
Subject: GD&T molded plastic parts
Hello Jim,
I have a book on ANSI Y14.5M, Dimensioning and Tolerancing
for Engineering Drawings. The examples shown are of clamps, collars,
shaft arms, etc. Can you recommend any books on dimensioning and
tolerancing compression- and injection-molded plastic parts such as
encapsulating cases / potting cups, toroid mounts, and bobbins? I'm
interested in dimensioning the plastic parts themselves, not the molds from
which they are manufactured (although information on the latter wouldn't
hurt).
Also, would you recommend ANSI Y14.5M, or ASME Y14.5M, for
dimensioning molded plastic parts? What's the most recent revision
(date) either way?
Thanks for your help.
A. Saupe, Jr.
Mr.
Saupe,
The current revision of the Y14.5 standard on
dimensioning and tolerancing is ASME Y14.5M-1994. It is always best to
work with the latest revision of the standard, since it is considered the
most evolved. I am not aware of any textbooks that are specifically
only about plastic molded parts. Although, I do discuss molded
and cast parts and what makes them unique in my books. Most textbooks
deal with common geometries that exist in all industries and cover how those
parts are defined whether they are molded, cast, machined or whatever the
manufacturing technique used to create them. What I would recommend is
a comprehensive textbook that covers as many examples as possible. I
have four books on the market that are current. The ones I would
recommend are called, Geometric Dimensioning and Tolerancing, Applications
and Techniques for Use in Design, Manufacturing and Inspection (the hard
cover textbook) and then the workbook by the same name. The textbook costs
$69.75 and is 624 pages long. The workbook costs $39.95 and is
350 pages long. Together they should cover just about any situation
you can run into. They are available at
http://www.dekker.com and do a
search for either James D. Meadows or Geometric Dimensioning and
Tolerancing.
If you want information specifically related to how to
tolerance your products, you can have me out to your facility either to
conduct a training course on how to tolerance them, or hire me as a
consultant to do the tolerancing myself (with input from key people in
your company on design requirements, manufacturing needs and inspection
techniques to be used).
If you have more questions, please feel free to email
me at jdmeadows@geotolmeadows.com or phone
at (615) 824-8644.
James D. Meadows
_______________________________________________________________________
Subject: Position
Mr. Meadows--
In reading your book (Geometric Dimensioning & Tolerancing), at one
point I saw a position call-out with no datum reference, although I have
lost its location in the book. I have seen this before and to be honest, it
confuses me. Is this a legal call-out ? Does it mean that, say, 2 features
are related to each other? Any help would be appreciated.
Thanks,
Greg
Greg,
Yes, you are correct. When a pattern of holes has
a position tolerance without a datum reference, or one that has a datum
reference that only serves the purpose of perpendicularity, the position
tolerance is binding the holes within the pattern to one another. It
is a hole to hole tolerance.
This is quite common and if you think about it, all
position tolerances that are used on hole patterns bind the holes within the
pattern to one another before they also bind them to any datums that are
referenced. So, we could consider the hole to hole requirement the
essence of what the position tolerance is trying to accomplish and datum
references as additional requirements.
Jim
_______________________________________________________________________
Subject: GD&T question
Jim;
I have found your textbook to be an excellent reference. Therefore I hope
you can answer my question.
I have a hole pattern similar to figure 17-4A on page 504 with the addition
of two 0.098 dia holes coordinated to each of the 0.375 diameter holes shown
(think nut plates). Is there a way to state that each two-hole pattern
is related to each of the .375 diameter holes without making each .375
diameter hole its own datum and putting a positional tolerance on each two
hole pattern?
Thanks;
Jim
Illustration from page 504
Jim,
There are a few really creative ways of doing such
a thing. But the way you describe sounds like the best possible way.
Creative way #1
You could always reverse the process and make the two
.098 hole pattern a datum pattern. You would start by positioning the
two .098 holes to each other and to the primary datum. Then below the
position control you would put a datum feature symbol. The two holes
would become datum pattern B or whatever. Then you would position the
.375 hole to datum pattern B at MMC (probably still including the original
primary datum as primary). See page 121 in my yellow text for
guidance. On this particular part, this would not be one of my
favorite methods.
Illustration
from page 121
Creative way #2
You could position the two .375 holes to each other and
datum A. Then below their position control you could put a datum
feature symbol (let's say B) and a note that says "2X
INDIVIDUALLY". Then position each set of .098 holes to A and B at
MMC. Then below that position control write another note that says
"2X INDIVIDUALLY". You might take a look at page 465 in my
yellow text for some
guidance on this.
Illustration
from page 465
Creative way #3
You could just call out some other features, such as
the edges or widths of the part, as your datum features, then position both
.375 holes and both .098 holes to them. That way all holes would be
related to the edges and to each other. All holes, even though they
are of different sizes and look like they are in different patterns, that
are referenced (located) to the same datum are considered a one pattern.
This in known as the Simultaneous Requirement rule and in the
gaging community, it is called the Simultaneous Gaging Requirement rule.
It means that all features located from the same datums are treated as one
pattern of features and must be inspected with the same gage or in the same
set-up. See page 459 in my yellow text for guidance on this.
Illustration
from page 459
All holes are
considered one pattern because they are located from the same datums.
Creative way #4
In fact, building on the theme in #3, once the edges
(or whatever) were made datum features, you could have a composite feature
control frame with two leader lines for each set of three holes.
Separate from the size limits of the .375 and the .098, from the position
control and instead show a composite position control that has two leader
lines (see page 461 my yellow textbook) one pointing at the .375 hole and
one that points at one of the .098 holes. The below the composite
position control write a note that says (3 holes). Do the same for the
other set of 3 holes. This will simply relate all holes in each of the 3 hole patterns loosely to the outside
edges (or whatever you have assigned as the datum features), but it will
relate the 3 holes more tightly to one another.
Illustration
from page 461
Non-Creative Way #1
I could go on, but the truth is that the way you
describe originally seems like the best way. Just make one of the .375
holes B and the other C. Then position one of the sets of .098 hole
patterns to A and B, and the other set of .098 holes to A and C.
Hope this
helps.
Jim
_______________________________________________________________________
Subject: Flatness
Jim..
Happy New Year!
I'm thinking flatness:
Hypothetical. I have a flange face, |flat|.1|
at a rate of |flat|.01/25 x 25|.
In your book, pp. 224, you state that
"..the orientation of the portions of the surface complying with [the
rate] may differ from the...overall surface measuring orientation..."
are you implying that after i set up to indicate the surface to ensure it's
flat within .1, i have to set up and re-indicate each and every square inch
of this flange? for a flange 25x25, i have to set it up an additional 625
times to measure each and every sq in? If so, gimme overtime!
And what about the square inch measured
inside .5, .5 to 1.5, 1.5? that's a different square inch. doesn't that
count? If so, gimme weekends, too!
Years ago at Pratt & Whitney, i learned
that each and every 'square inch,' even though it's treated separately, is
still part of the surface. isn't it better to have a 12.5 x 12.5 grid on the
surface table. indicating inside each group of 4 of these grids (=25x25)
with the indicator following the surface contour yields the results which
you document and enter into a table. you still treat the whole surface
within .1, but you watch the rate of change for each square inch to control
it to .01.
This method allows you to measure overlaps
from square to square. in other words, you measure around the inside of (4)
12.5 squares, then move over 12.5 and measure the inside of the next 4
squares, etc. (instead of measuring 0 to 1, 1 to 2, 2 to 3, you can also
measure .5 to 1.5, 1.5 to 2.5, 2.5 to 3.5 etc...all in one single setup.)
I also believe the number of setups required
in your method greatly enhances the chance of operator error which could
lead to a 'leaker' or worse.
And, since you state on pp224 that "any
feature being controlled for flatness may be (and often is) a datum
feature..." rotating the surface to get each sq. in. 'level' would
'break the plane' of the datum.
Think about this Jim. And please get back to
me.
Best regards..
Ted
Illustration from textbook
Ted,
The statement is true. The overall flatness
tolerance zone has an optimal orientation. Every 25 x 25 (or whatever)
flatness tolerance zone within that overall tolerance zone has an optimal
orientation. Each optimal orientation of every square may be different
than every other square. That does not mean that you have to reorient
the part every time you measure a different square. You may choose to
orient the part one time and measure every flatness requirement for the
overall and every square. And you may be satisfied with the results
because every square checks within the tolerance. So, if all you are
looking for is attribute data (is it good or is it bad), the only time you
may consider reorienting is if things are checking bad and you think a
reorientation of the square you are checking will get it to check good.
Speaking theoretically though, if you want to know the
actual value of how flat each square is precisely, either a software virtual
reorientation of collected data points within a square or actual manual
reorientation of the part would probably be necessary. And if you were
anal enough to want it to be perfect, you're right, you would retire on that
job and have to will the remainder to your descendents, because there are an
infinite number of squares depending on where you start and what overlaps.
So, on the one hand we have theory (what we would do given infinite time and
resources) and on the other we have reality (what do you really need to do
to satisfy your own set of standards to convince yourself that the part is
either good or bad).
The truth is, measurement is always guesswork.
Even in a simple one level flatness control, the inspector is supposed to
tell us that every point on the surface is within the tolerance zone.
In order to do this, he would have to probe every point (which he won't do)
and even if he did, what size probe did he use, and if he is using a CMM,
what sort of filtering algorithm is employed by the software program?
How you measure something is up to you. But first
you must comprehend the theory of what it is you are trying to prove.
Only then can you make the decisions on how you will compromise this theory
to blend with your harsh reality.
Besides, isn't it too soon after the New Year to be
involved in such deep and disturbing subjects. You should still be
trying to take enough aspirin to muffle that banging New Year's eve hangover
most are suffering from.
Jim
_______________________________________________________________________
Subject: Thank You
James,
Just wanted to say thank you again for your expertise, time and patience in
providing the valuable training in the Principles of Dimensioning and
Tolerancing for Gages and Fixtures
at the
University
of
Milwaukee
.
I always leave your classes/seminars with
more knowledge and a better understanding on the subject of GD&T
and its applications.
It is professionals like you that contribute
more to the advancement of industry than some people will ever realize.
You are definitely one of the great names in the History of Geometric
Dimensioning & Tolerancing.
I look forward to attending your class on
Tolerance Stack-up Analysis next year.
Thank you again for your time and expertise.
I hope you and your family have a Merry
Christmas and a Happy New Year!
Respectfully,
Perry
Perry,
I appreciate the compliment. The week went a lot
faster and was more interesting because you were there. I hope to see
you in the Tolerance Stack-Up Analysis course.
Jim
_______________________________________________________________________
Subject: Measuring Flatness on a Rate Basis-Another Way?
Jim,
In a flatness control that applies on a per square inch
basis, since there are an infinite amount of 1 inch squares on a surface
this makes the measurement of the refined flatness note almost impossible.
Is there another way to refine the flatness without having to re-level each
1inch square?
Jerry
Jerry,
No one measures all possible squares. Even a
simple flatness control would make the inspector responsible for all points
on a surface, and no one will measure all points on a surface. And
even if they did, the edges of the surface may be chipped or even filed to
relieve sharp edges. This alone would technically be enough to make
most surfaces fail a flatness requirement. Usually we are just looking
for an acceptable level of confidence that any feature being inspected has
met a requirement well enough to perform the function we intend.
All measurement is guesswork. It's just that some
guesses are better than others. Given a limited amount of time and
flawed inspection hardware and software, we make the best estimate of
compliance we can.
For this flatness on a unit/rate basis type of control,
even though the optimal results would be gained by re-leveling every square
that is measured, I'm really surprised to hear anyone is actually
considering doing that. Most inspectors just re-level when the part is
checking out of spec without re-leveling. If one takes the approach
that he/she is just looking for attribute data (a good vs. bad part
decision), then very little re-leveling is usually called for. Of
course, if you need to know the actual value of how flat each portion of the
surface is, your task is going to be much harder. If that is the case,
I would look for a CMM software program that is capable of re-leveling each
area under test after a constant contact scanning probe has collected a
sufficient number of points on the surface to achieve a level of confidence
that is acceptable to all. Just remember that all software usually
employs some sort of smoothing algorithm that just uses your raw data to
render a version of the surface that it deems more appropriate for
evaluation. The programmers will all tell you this is necessary to get
rid of readings that are caused by dirt, vibration and a thousand other
contributors. In addition to that, probe size, the number of points
probed and the distribution of points all lend to measurement
uncertainty.
Maybe you and the others involved just need to sit down
together and discuss what is needed to attain an acceptable level of
confidence that the part is either compliant or not, based on the functional
needs of the product. After all, you are all on the same team, trying
to achieve what is best for the customer.
Jim
_______________________________________________________________________
Subject: GD& T questions
James,
I just had a course from you and I have couple of follow-up questions.
A pattern of holes get additional tolerance due to datum shift if the datum
is
referenced at MMC in the pattern's feature control frame. Will it get
additional shift if there is another datum referenced at MMC?
e.g. Tolerance available from B(m) but is there additional tolerance
available from C(m) also.
One more question
A threaded hole won't get bonus tolerance due to its size variation. Will
it get additional tolerance if it's positional feature control frame has
a
datum referenced at MMC condition?
e.g: There will not be any bonus tolerance due to size but is it available
from B(m) and C(m).
Sam
Sam,
Thinking about this stuff already?
As to your first question, if the two datum features
you are referring to are holes or shafts, then the tertiary datum feature
that is referenced at MMC won't add to the pattern shift tolerance that is
given by the secondary datum feature referenced at MMC. It will just
try to limit it. To see what they allow, try picturing a gage pin in
each hole. The gage pin in the B hole is a fixed size (virtual
condition). The gage pin in the C hole is also a fixed size and
capable of sliding toward (or away from) the B hole. As each hole if
produced larger than its gage pin, airspace is created between the gage pins
and the holes. The part can move only in the ways allowed by the
constraint of the gage pins within each hole.
The answer to your second question is yes. A
pattern of threaded holes that reference a datum feature at MMC may shift as
a group an amount equal to the datum feature's departure from its virtual
condition (provided the datum feature is not a threaded hole). This
additional tolerance gained from the datum feature is for the group of
threaded holes, not for the individual holes within the group.
I hope this helps. Stay in touch.
Jim
_______________________________________________________________________
Subject: JIS standards and GD&T
Mr. Meadows,
I'm looking into purchasing your book on GD&T along with the workbook.
Since we are a Japanese owned company and primarily machine parts for the
Japanese Automotive Market my management would like to know how this
conforms to any JIS standard there might be for GD&T. I've looked
but not
had any luck in finding such a standard. Can you help me? Is there such a JIS standard?
Would your book conform to any such standard?
Sincerely,
Ben
Ben,
My books are written to conform to ASME and ANSI
standards, such as the ASME Y14.5 standard on Dimensioning and Tolerancing.
In my books, I often mention areas where the rules of these standards may
differ slightly from ISO rules. Individual countries, such as
Japan
also have standards on Dimensioning and Tolerancing and they all have
small areas where the rules differ slightly. Most of the rules,
however, are the same. Generally, if a drawing is drawn in the
United States
, it is drawn to conform to the ASME Y14.5 standard, even if the
company is foreign owned. I have done work for a lot of Japanese owned
companies and have not found the minor differences to be a problem in
creating and interpreting the drawings (since all are essentially patterned
after the ISO documents).
James Meadows
_______________________________________________________________________
Subject: GD&T Applications Hand Book
Mr. Meadows,
I recently had a chance to review one of your GD&T handbooks (GD&T
Applications & Techniques for use in Design, Mfg, and Inspection) during
a meeting with my Product Engineer at DaimlerChrysler, and I found your
handbook to be very informational. It is more detailed than the small
handbooks that I currently own, and would like to know how I can acquire a
copy of your handbook.
Have a Good Day!
Steven
Steven,
That book is available from Marcel Dekker, Inc. in
New York
. Their phone number is 1-800-228-1160. They also have a
website; www.dekker.com that you can
find the book on. Other sources are www.barnesandnoble.com and
www.amazon.com . I don't sell most
of my books, myself. The only book of mine that I sell is the one on
Tolerance Stack-Up Analysis. My website details the contents of all of
the books I have written. My website address is www.geotolmeadows.com
. If you would like more information, feel free to call me or Jeannie
Winchell at 615-824-8644.
Thanks for inquiring.
Jim Meadows
_______________________________________________________________________
Subject: Use of CMM for Inspection of Round Features
Dear Jim:
There is much debate at my company over the correct method to inspect
cylindrical bosses. These features regularly do not meet size
specifications when inspected via CMM and I believe this is due to probings
taken at tapered, pitted, worn areas, etc. However, the bosses often meet
specification when inspected with calipers or ring gages. Ring gages best
simulate how the part is used since the bosses are used to position female
bushings.
Is inspecting the part similar to the way it is used the correct method, or
should I be concerned with form, taper, etc. of the boss? Should there be
guidance on the drawing of how to measure the feature?
Perplexed in
Portland
Dear Perplexed,
You haven't given me the specifics of what you are
checking. Size, form, angle and location are the "Big
Four" things that geometry can control. You may be inspecting one
or a combination of these things. Still, I understand your situation
and feel your pain.
There are some generalities that apply to us all.
One of them is exactly as you suggested. All things should be measured
as closely as possible to the way they function. If this requires a
clarifying note on the drawing as to the exact way you want something
measured, then I am all for it. The Y14.5 standard has suggestions to
this effect when it talks about flexible parts being measured. Y14.5
and many other standards, like the old ANSI B4.4 standard (Inspection of Workpieces)
and the new standard-ASME Y14.43-2003 (Dimensioning and Tolerancing Principles
for Functional Gages and Fixtures) all say that since flexible parts
may be distorted by clamping them, if restraint during measurement is to be
used, a note must be written to describe how a part is to be restrained
including the maximum force used.
There was a situation in the automobile industry years
ago I remember, where sheet metal panels were being measured while fixtured
in a vertical position and they checked out great. Unfortunately, when
they were used in the vehicle, they were assembled in a horizontal position
and displayed characteristics that were not evident during inspection.
They sagged badly in the vehicle. You could liken it to the car roof
sagging down on your head. After that, the engineers came up with a
phrase to help remind them of this error, so that it didn't happen again.
That phrase was, "Don't fight gravity." It meant,
"Always inspect parts in the way they are used." In this
case, it meant always measure parts in the same orientation that
they fit on the vehicle.
So, for your problem, a note describing how the part is
to be inspected, or a written measurement plan would be quite helpful.
There was even a standard issued by ASME a few years ago called Measurement
Planning wherein it suggested that every part that is designed should have a
measurement plan that accompanies it.
CMM's are useful measurement tools. But everyone
should realize there are a wide variety of measurement tools available to
them, and not expect the CMM to be the best tool for every part. They
pick up discreet points on a surface (and as you point out, these points may
not be the ones you care most about). From these few points, they make
an educated guess about whether or not your part may meet the drawing
requirements. They also run those probed points through a filtering or
smoothing algorithm in which the raw data is altered, sometimes throwing out
the highest and lowest points to eliminate what it perceives as dirt or
other unwanted information. Sometimes this is good and sometimes not
so good. But certainly, the information given by the CMM is only as
good as the points it probes and the software it employs.
In general, we want to have information about the
functional portion of a feature. Where that portion may be is not
always readily evident to the inspector. If a cylinder has a portion
that is tapered or even filed off to stop someone from cutting themselves
when they pick it up, these may be points that are probed by the CMM.
And if you don't want that to happen, a note saying so would be of great
help to the inspector. And maybe, as you say, the best tool to measure
your cylinders, is simply the tool that best simulates the way the part
functions. I am the chairman of the ASME committee on gages (the
Y14.43-2003 standard mentioned above), and if you say gages work better for
your parts than the CMM, I certainly am not going to argue with you.
Just write a note and tell the inspector the same thing.
Jim Meadows
_______________________________________________________________________
Subject: ASME Y14.43-2003
Dear Jim,
I have received a copy of the "Dimensioning and
Tolerancing Principles for Gages and Fixtures" (your hard-earned
masterpiece). Please accept my most hearty congratulations to you and that
'first team' committee for a magnificent job and in 'finally' providing the
methods, rules, guidelines and direction for the gaging community to do its
job better than ever before. New horizons have now been supplied and
tutorial guidance for all from beginner to expert are there. The new
and necessary ground now broken for the benefit of all users and the
gaging/manufacturing profession, can better proceed into the future
with greater confidence; it now has "a home of its own". The sort
of 'guessing game' basis of the past in gaging principles, now has a
nucleus of authority and a point of departure for the future. Be prepared,
of course, for the dialog, criticism, challenges and maybe changes for
improvement forthcoming in the future life of the standard. Such, are really
a form of flattery and departures for possible new progress with a
stronger and more knowledgeable using constituency. A permanent vehicle on
the subject is now there for all the world to see. The feeling of a job so
well done will give a long lasting good memory.
Enjoy the 'victory', you have all earned
"ownership" of a new ASME Standard. That is a real accomplishment!
; with the rewards, as you well know a bit intangible but very real' into
the future.
Thanks again and best regards to all,
Lowell
Foster
Thanks,
Lowell.
We learned a lot. And we learned much of it the hard
way. I shouldn't have gotten mixed up with the B89 committee in the
first place. Little did I know that they had an agenda from the
outset. They wanted to squelch any standard on gages, so that they
could pretend like CMM's are the only measurement method acceptable to ANSI
and ASME. I always thought both were necessary, each having unique
abilities lacking in the other.
But we won. We were going down in flames, however,
until you rode to our rescue. I didn't mind for myself so much.
I've always had a willingness to dive off a cliff, if I thought a wrong was
being done and the only way to alert others was to commit political suicide.
But I felt bad for the others on our committee that dove over with me.
I was surprised when so many did. Still, we just didn't have the clout
to win. We had only the ability to make a lot of noise and make people
mad. I was ready to settle for that. Then you started writing
letters and opening doors. I thought my letters were stinging, but
your letters to B89 were like daggers. I know if it weren't for your
influence, we wouldn't be a Y14 standard. It was like suddenly
discovering you have a big brother willing to stand up for you. I
really appreciate your efforts on our behalf and I'm certain the other
Y14.43 members feel the same. There was a phrase I remember from Y14.5
(and you, in particular) in years past. It was, "Fighting the
good fight". To me it always meant doing the right thing in the
face of adversity. I think this time, a good thing happened, in spite
of bad people. And we owe much of our success to you.
Thanks again.
Jim
Jim,
Thank you for your very kind response. You folks did
all the hard work and were the pioneers brave enough to "slay
dragons" in the interest of a mission of good works against all odds. I
confess that I was a little jealous that, as an old tool and gage designer
(real old), I could not have been one of your group to really help in the
nitty gritty details. Your work kind of fills a void in my wishes (now a
little rusty), long held, where gaging would become more of a 'known science'
rather than individual 'black magic' and have the respectable
power and order that it surely deserves.
Mission
accomplished!
Thanks again to you personally for all your work and
dedication to the difficult task.
Best regards and again congratulations on the final
victory.
Lowell
Foster
_______________________________________________________________________
Subject: Pins for locating assemblies
Jim,
I am a mechanical engineer at Varian Medical Systems in Palo Alto Ca and
have attended several of your on site classes as well as viewing your tape
series. I have a question regarding the use of pins to locate
precision
sub-assemblies within our medical machine. These assemblies must be
removable for maintenance a few times during the life of a machines
(approximately 15 years). For all intensive purposes, assume
that I would
like to accurately assembly one plate relative to the other (plate
"1" to
plate "2").
The solution I have proposed is to use a locating pin and a diamond pin on
plate "1" and 2 holes on plate "2". I have
assigned the flat mating surface
as the primary datum for both parts. Because the fit must me
accurate, yet
removable in the field I have suggested a "locational clearance"
fit, based
on American National standard, for the secondary datum's of plate
"1" and
"2". I have assumed that the tolerance method for both pin
and diamond pin
is the fixed fastener formulas i.e. (MMC hole -MMC shaft) = Geo. Tol.
to be divided
between mating features. The secondary datum for part "1"
and part "2"
would be the pin and hole respectively, with a perpendicularity control to
the primary datum and tolerance at MMC according to the fixed fastener
formula. The tertiary datum for part "1" and part
"2" would be the diamond
pin and hole respectively, with position control to the primary datum,
secondary datum at MMC, with a tolerance at MMC according to the fixed
fastener formula.
After I calculated the tolerance for the position control for the tertiary
datums of part "1" and part "2", I found that the
tolerance is unrealistic,
even with a bonus tolerance. Therefore, I decided to make the
preferred
metric fit, for tertiary datums, larger such as a "close running"
fit
according to the American National Standard and I still used the same fixed
fastener approach to the tolerancing. In terms of accuracy of the
assembly,
this larger fit should only sacrifice a slight angle offset at assembly.
My question to you is this...
1. Do you agree with this approach?
2. What additional recommendations would you make to this approach?
3. Am I correct in assuming that the gd&t of a diamond pin should be
made
with the Fixed fastener formula?
4. Does the diamond pin geometry give you any additional bonus in
position
tolerance that is not captured in my approach, or does the diamond pin
geometry simply avoid redundant constraining?
I would greatly appreciate your response to this matter as your insight is
valuable to our organization. Thanks.
Chris
Chris,
1. Yes Chris, I think this is the same type of
approach I would have used.
2. I have no additional recommendations at this
stage of the design. Of course, now you have to reference the datum
reference frame you have created. I assume there will be positional
controls that will follow and reference these datums. To recommend
additional controls, I would have to know more about the parts. But it
seems you have it well in hand so far. I have no reason to believe you
won't continue to do well.
There is one comment though. If you were to look
in my textbook (the yellow one) one page 150, you would see that I follow
the same type of approach you are using, but instead of a diamond pin on the
mating part, I use an elongated hole on the part with the holes on it.
This approach is widespread in the automobile industry and would work
equally well as the approach you have chosen. It isn't necessarily
better, just more common (well maybe a little bit better). The diamond
pin approach is actually more common to gage design than mating part design.
Illustration
from text page 150
3. Yes, these are all fixed fastener assembly
conditions.
4. As I mentioned in number 2, the
diamond pin approach is actually more common to gages than mating parts.
But, no to the additional bonus tolerance. I believe your goal here is
to treat the pin as though it is cylindrical and to just take advantage of
the reduced section of the pin to make certain it isn't controlling
location, but instead just controls rotation (just as an elongated hole on
the mating part would accomplish, if used instead of a diamond pin on this
part-Hint-Hint).
At any rate, it appears you are doing a great job.
You must have had a good teacher.
Jim
_______________________________________________________________________
Subject: Multiple Giant Floor Plates Drilling...(Y14.5M-1982)
Hi, Jim Meadows:
On multiple giant floor plates on
which I will drill thru holes and counter bore holes.
I am using positional composite
tolerance on basic A, B & C datums.
My question is can I repeat using
datum names A, B & C for the different plates? or do I need to create
new datum names for the primary, secondary & tertiary datums ?
I am creating new datum
names now: D, E & F and G, H & K and L, M & N and P, R & T
and U, V & X and Y, AA, AB.
Is this really necessary?
Thanks in advance.
| 
