Subject: GO Gages for Measuring Maximum Material Condition

Jim,

Measuring a hole (ID) at .126 plus .005 and minus .000.  I use a .126 (plus) plug gage and the gage pin does not enter the hole.  I assume the hole is undersize and out of specification.  The actual plus pin is .1262.  My supervisor says the hole is within specification because I am suppose to use .126 (minus) plug gage.

The actual size is .1258.   Is this true?     I think the gage pins should not be smaller than .126.  I think the minus pins are for the NO-GO and the plus pins are for the GO.  Maybe I am wrong, so please enlighten me.

 
I finally found your web site. I've been a loyal James D. Meadows fan since the workshop you held in Half Moon Bay , California .  I attended your ANSI-Y14.5M-1994 training in August 1995.   I do not have any more people to ask technical questions of.  I will return to your website often and have registered to receive your newsletter.

Sincerely ,
Ken

Ken,

Jim called in from the road and dictated his response to your question.

"Although the ASMEY14.43-2003 Standard - Dimensioning and Tolerancing Principles for Gages and Fixtures does not dictate gaging policies individual companies must use, the preferred gaging policy, as defined in the ASME Y14.43 standard, is called the 'Absolute Gage Tolerancing Policy'. 

The Absolute Gage Tolerancing Policy says all gage pins are plus tolerance for GO gages and functional gages and all gage holes are minus tolerance.  So, you are correct in saying your gage pin is a diameter of .126 all plus tolerance and no minus tolerance. The recommended tolerance on gages is 5-10% of part tolerance.  In this case, it would be 5-10% of the size tolerance on the hole being gaged.

The reason we do not prefer gage pins to have a minus tolerance is that we (ANSI/ASME) do not want the gages to accept bad parts.  The down side of our policy is that it is possible for a borderline, technically-good part to be rejected."

Nice to hear from you.  I hope our paths cross some time in the future again.

James D. Meadows, Chairman

ASME Y14.43-2003 Standard - Dimensioning and Tolerancing Principles for Gages and Fixtures

 __________________________________________________________________________

Subject: Roundness

Jim,

How are you doing?  I hope all is well with you.  Jeannie called on Friday and I am waiting for the powers that be make a decision on bringing you here.  I hope they make the right decision.

I have a question on roundness:  Does an air gage truly check roundness or just size?

Thanks,

Greg

Greg,

It depends on the configuration of the air gage.  Generally, they are configured to probe just two opposite points on the diameter or three points at 120 degrees from one another at a time.  These configurations mainly check the size.  Technically, size is supposed to be inspected for violations of a maximum material condition envelope with a simulation of a GO gage.  For a shaft, this would be a cylindrical gage hole that is as deep as the shaft being inspected is long, and with a diameter of the MMC of the shaft being gaged.  Then, a two-point opposing point measurement checks the least material condition (LMC).  Most air gages are only properly configured to accurately measure LMC. 

As far as roundness is concerned, if enough opposing points on the surface of the cylinder being measured are taken and found to measure the same in size, it is a rough check of roundness.  It can be fooled into believing that some parts that are not round meet the roundness requirement, but is a reliable rough check for most produced configurations.  Rough checks of roundness are also taken by micrometer measurements (many) on shafts or by putting a shaft into a V-Block and rotating it under a dial indicator probe.  Since none of these techniques stabilizes a central axis from which measurements are taken, all can be fooled into believing parts that are not round meet roundness requirements. 

For a more reliable roundness measurement, the axis of each circular cross-section being tested must be stabilized, then each circle of the surface swept with a probe.  Each circle is re-zeroed, since this is not a cylindricity measurement.  This can be done with a chucking device and a dial indicator, or if this is a critical, tight tolerance, a roundness checking machine should be employed.  There are many of these machines available on the market, and they are very accurate and built just for the purpose of checking roundness.

Hope this helps,

Jim

__________________________________________________________________________

Subject: PpK Tolerance

Mr. Meadows

I received your name from a DCX supplier development engineer.  We have a question, and I hope you have a short quick answer.

Question:  In determining a capability (Ppk) of a hole position, which has a MMC in the  GDT block attached to that feature?

Example:
Position tolerance of a diameter 1 mm MMC to |-A-|-B-MMC|-C-MMC|
and the hole diameter has a tolerance of +/-1.0 mm.

In the process, I produce the part to +1.0/-0.0.  Can I then add 1.0 mm to the position tolerance when I calculate my Ppk?

Hope this is clear and to hear from you soon.

Regards

Tom

Tom,

Yes, you can.

Jim

__________________________________________________________________________

Subject: Coplanarity

Jim,

Can you let me know if you  believe the following method is valid for checking coplanarity and why or why not. Personally I don't believe it is but cannot come up with a valid reason.  The feature in question is a series of 500 pins with a coplanarity requirement of .006.

There are 2 similar methods being used:

1) The pin heights above the board are being measured and if the delta of the highest and lowest pin is .006 or less it is considered acceptable.

2) The top of one pin is "zeroed" and if the T.I.R. from that zero is .006 or less then it is considered acceptable.

Neither of the methods establish any sort of  reference plane with respect to the pins, the reference plane used is the opposite side of the board. What I've seen in the past is that a reference plane is established either using a surface plate setup or a CMM and then the TIR of the "surface" is measured.

Thanks,

Bob

Bob,

Both methods are correct for acceptance.  Since the orientation (you didn't mention a datum reference) is unimportant, if the delta between the highest and lowest points of all probed points is .006 or less, the coplanarity is met (that's all the control is really asking for).  Also, if the full indicator movement/total indicator readout isn't greater than .006 for all points, then the tolerance requirement has been met.  If a datum had been referenced in the coplanarity control, then the relationship to that datum would also have to have been met.  But without a datum reference, both methods are capable of determining the parts are good.

The only thing to be cautious of is if the delta or the TIR is greater than .006, it is still possible that the parts are good. If the points probed are graphed out and the data is manipulated for orientation (angle) and found to be able to fit within a .006 tolerance zone, then the parts are in compliance with the tolerance.  By setting the part up on a surface that is not a datum feature, an additional error of orientation to the plane formed by that surface is introduced.  Since that is not part of the requirement, if the additional error is great enough, it could cause a compliant part to fail.

Jim Meadows

__________________________________________________________________________

Subject: Question about "TOLERANCE STACK-UP ANALYSIS"

Hello, Jim

I have purchased your book "TOLERANCE STACK-UP ANALYSIS" and have a question about one of the exercises.

Exercise 8-5, problem #1 "answer" page.

I am confused with the .130 pattern shift D(m).  I would expect the pattern shift to be .050.  I come to that conclusion by reviewing pages 8-2 and 8-3, looking at the addition as shown of sheet 8-3.

Can you please review this and explain to me what is going on.

Thank you.

Matt

P.S.  I attended your class 2 years ago.  I have found your book to be very helpful.  I am now trying to perform the tolerance analysis (stack up) to verify functions and fits.  I have realized so far that this is not an easy task to perform.   Your book "TOLERANCE STACK-UP ANALYSIS", I find to be very useful.

P.S.S.  Please call me if would like to discuss this over the phone if that is easier.

Matt,

The figure on page 8-1 has a secondary datum feature of size with two different virtual conditions generated by two geometric (position) tolerances.  One relates to the datums A, E and D, while the other relates from hole to hole and to datum A only.  The trick is to know which one applies to the pattern of 28 holes being positioned back to this datum feature (datum feature B).  The answer is that the pertinent tolerance (and virtual condition) is the one that applies to the datum(s) that precede datum feature B (that is referenced at MMC in the 28 hole pattern's feature control frame).  The only datum that precedes B in the 28 hole pattern's position control is datum A.  Therefore the pertinent geometric tolerance that can be derived from B is found in B's position control that uses only the A datum.  That tolerance is zero at MMC, but .010 (bonus tolerance) at LMC.  So, the maximum pattern shift is a diameter of .010.  Figure 8-1 follows:

For the Exercise Figure 8-5, datum feature D has only one virtual condition generated by one geometric (position) tolerance.  It is .080 at MMC, but .130 (.080 plus .050 bonus tolerance) at LMC.  So, the maximum pattern shift that can be experienced by the four hole pattern is a diameter of .130.

Hope this helps,

Jim Meadows

__________________________________________________________________________

Subject: GD&T Problem for Door Hinges

Jim,

 I was forwarded your contact information from Jimr at DCX, as he suggested that you might be able to help our group resolve a GD&T issue with door hinges - specifically flatness on the mounting surfaces. Our issue is plainly this, for the mounting surfaces of the hinge which attach to either the pillar or door, we currently have a flatness callout attached to each corresponding hinge surface. However, the assembly plants are finding that when the flatness of the part moves to a convex nature - it can produce "rocking" in the hinge when the bolts are driven one at a time. This results in repeatability issues.

We think that the best way to solve this is to ensure that the hinge mounting surfaces are always "flat to concave" in order to eliminate this "rocking" from a convex part.

Attached is a proposed GD&T scheme to try and specify this type of control. Could you take a moment and review the attached GD&T scheme and forward your comments / recommendations?

Thanks in advance for your assistance on this,

Brad

Brad,

First, I don't understand why you are using a profile control on datum feature A.  It looks like one continuous planar surface.  It seems like a simple flatness control would serve it best.  The problem with applying profile of a surface to it and referencing datum targets A1, A2 and A3 is that they will form datum plane A and the profile tolerance zone is equally split on either side of datum plane A.  This isn't always a problem, but it could have the effect of denying you half of your tolerance zone if the datum targets happen to contain the highest or lowest points on the surface.  If that was the case, the zone outside of datum plane A (half of the 0.3 tolerance) would contain none of the surface, and the other half of the zone (the other 0.15) would have to contain the entire surface in order to be in compliance with the geometric tolerance.  If datum feature A is just one continuous planar surface, a flatness tolerance would be less restrictive, allowing the entire surface to occupy the 0.3 tolerance zone.  This flatness control would reference no datum.   After that, if you feel you need datum A for some other subsequent surfaces (or holes, shafts, etc.) to reference back to, you could still establish datum targets A1 through A3 if you want to.  But they would have nothing to do with this control.

The other issue is one that I have run into quite a few times.  On the two coplanar surfaces you definitely need a profile of a surface for coplanarity control.  Calling each of them flat, or calling one flat and profiling the other back to the first makes very little sense (since they work together acting as though they are one surface).  The solution you propose is interesting.  Let's talk through it.  Since you are going to set up on the three datum target areas, the tolerance zone will split at the datum plane and become equal bilateral (plus and minus 0.3).  This would mean that the middle of the part could still be the highest points.  Since the tolerance zone is a total wide profile zone of 0.6 (according to the illustration you sent me), that means the middle points could still be 0.3 higher or lower than datum plane B.  The last illustration you show says that condition would allow the part to rock over onto one of the two surfaces and give you a 0.43 degree angle and a high of 1.41 from one surface to the other.  If this situation was unacceptable to you, the proposal you show for a change doesn't seem to correct the problem.  It seems to leave you in the same boat.

Now to correct the problem.  Hmmmm.....pretty tricky situation.  Here are some possibilities.  1) Just tighten the coplanarity (profile of a surface) control to something that you can live with and get rid of the datum targets (since they don't seem to be helping).  2) Call out the two surfaces coplanar (using profile of a surface) to within 0.3 (or something) without the datum targets (so that you get to use the entire 0.3 tolerance zone without it splitting), then make one of the two (entire) surfaces a datum feature and reference the other parallel to it to within a tighter tolerance than 0.3.  3) Use the coplanarity control (again, I can't see the need for the datum targets, but of course, that's up to you), then below the control say "SEE NOTE 27" (or whatever number the note is) and in this note (which I would actually show as an illustration) convey the same concerns you show in the "rocks" illustration you sent to me.  But instead of that illustration, show the limits of angle (something considerably smaller than 0.43 degrees, I assume) that you are willing to put up with, when the part does rock.  I like this approach because it lays out your specific concern, sets the limit for the rock you will accept as a maximum number of degrees and clarifies the coplanarity control better than the limits of geometric tolerancing symbology have evolved to yet.

That's all I can think of right now.  If this isn't helpful, feel free to write again and I'll take another crack at it.

Jim

__________________________________________________________________________

Subject: RSS

James,

Is there a percentage probability of the RSS use in tolerance stack-ups? What does RSS really tell us? Is there a sigma value?

I am getting beat up over this by my manager. Help me Please. Thank you.

Jackie

Jackie,

You have to understand, I don't really enjoy conversations about statistics.  I am not a "statistics zealot".  But the information in my books is well researched and time tested.  I convey information that has been created by reliable sources and add to them only the missing pieces of puzzles required to apply them to tolerancing (in this case, statistical tolerancing).

Now that I've bored you to death, I will quote from Quality Assurance Pamphlet AMSTA-P-702-116 (August 1967), entitled Statistical Tolerancing-A Solution to Procurement Problems-US Army Tank Automotive Command.  This extensive pamphlet is 59 pages long and has a bibliography too long to list here.  It says, in referring to the RSS method for calculating something it calls "natural tolerance", the tolerance likely to be consumed in an assembly produced to a Gaussian Frequency curve, "The dimension is then designated as the median, plus and minus 3 standard deviations  The total natural tolerance is therefore 6 standard deviations. The natural tolerance represents process capability and will include 99.7 percent of the dimensional values obtained with the process."  "This approach to assembly tolerancing is the "statistical" method.  Derived from well established basic probability theory, it may also be written as follows" it goes on to state the Root Sum Square formula here (the tolerance of the assembly likely to be consumed is equal to the square root of the sum of the tolerances on the individual components squared). Then says, "Examination indicates that this statistical assembly tolerance represents the tolerance that will be achieved on 99.73 percent of the assemblies..."  and from my own book on Tolerance Stack Up Analysis, in Chapter 11, "a) Using the derivation of the Pythagorean theorem called the RSS (root sum square) formula, calculate the statistical probability for the assembly (the natural tolerance likely to be used during manufacture)  b) Determine the percentage ratio between the statistical probability tolerance and the previously calculated 100% assembly tolerance and c) Determine the increased statistical probability tolerances to be redistributed to the assembly's component parts."

 There is much more information on this topic in the pamphlet and in my book, but I believe that is all you asked.  If you need more information on this topic, please feel free to write again.  I will be out of the office until the weekend, but will respond when I return.

 Hope this helps,

James D. Meadows

__________________________________________________________________________

Subject: RE: RSS

Thank you. Thank you so much. I will get my hands on the spec. and give it to him.

Jackie

Subject: Question on Page 45, Fig. 3-4, of Your Book on Geometric Dimensioning and Tolerancing?

WORKPIECE

 FUNCTIONAL GAGE

Mr. Meadows:

I am attempting to contact you because I have no expert to consult here at the office.  (It is my mission to become the "office GD&T expert").   I am studying your book, Geometric Dimensioning and Tolerancing: Applications and Techniques for Use in Design, Manufacturing, and Inspection, (11th printing)  and companion workbook on my own and I am confused by what I perceive to be an error on page 45, figure 3-4.  I think that the unilateral tolerances applied to the Ø.550 pins and the Ø2.994 I.D. should be swapped because, as printed, those features at MMC interfere with the MMC virtual condition boundary of the mating holes.  (Should be 5X Ø.550 +.000/-.002 and Ø2.994 +.002/-.000)  Am I correct or do I need to read it from the beginning again?

Respectfully,

Michael

Michael,

It is not an error.  Page 45 shows the gage, not the mating part.  The gage policy of the American National Standards Institute (ANSI) is to not accept a bad part.  We must therefore tolerance our gages to reject a few borderline technically acceptable parts.  The policy is that functional gage pins begin at the virtual condition size of the holes they inspect and are then toleranced with all plus tolerance (gage pins can only be toleranced to be larger than the virtual condition of the holes they inspect).  Conversely, gage holes begin at the size of the virtual condition of the features they are to inspect and are toleranced to be all minus, so as to accept no out-of-tolerance parts.  The type of gage tolerancing shown is called "Practical Absolute" gaging (described as a gage that will in practicality never accept an out-of-tolerance part.  It is best described in the ASME Y14.43-2003 standard on Dimensioning and Tolerancing Principles for Gages and Fixtures.

Hope this helps,

James D. Meadows

Chairman Y14.43

__________________________________________________________________________

Subject: Question About an Example on Pages 198 & 199 in Your Book.

WORKPIECE WITH 5 HOLES (Page 198)

CALCULATING MINIMUM WALL THICKNESS

Dear Mr. Meadows,

I contacted you earlier few times and you were very prompt in your responses and I sincerely thank you for that.

While I was going through your book, I have a doubt and following is the description to the best of my ability.

The question is in reference to Example problem on Page 199 of your book Geometric Dimensioning and Tolerancing.

Movement of D due its change from MMC (VC) to LMC = 1.000-.600 = 400
It also moves additionally because of reference to datum B at MMC. This movement is equal to 5.000-4.990 + .030 as B (since it is a datum of size) moves from MMC (VC) to LMC = .040
(They are VC as they being secondary datums, should be considered at VC)

Therefore total movement of D is .440 instead of .400 as shown in the book. ?????????????

In other words, applying the logic item 2 given below on the same page, which states
“If D is related to B and the 4 holes are related to D, then the 4 holes as a pattern are related to B to within the sum of their relationship to D and D’s relationship to B”
4 hole relationship to D = 1.000-.600 = .400
D’s relationship to B = its own (1.000-.600) + Additional movement due to B “s change from MMC to LMC = .040 = .440.

In the next example, applying the same logic,
“.130 Allowed movement of feature D at LMC to C” is correct as C is a planar datum.

So I feel that since in the earlier example datum B is a feature of size and not a planar datum the value will be .440 instead of .400

I would very much appreciate your response at your earliest convenience.

Also I have two general questions for you as you are on the ASME committee:

1.        In Y14.5, why is it necessary to specify “R” for slots (It used to be R FULL earlier I think). If it is not R Full the R (radius) has to be specified. In other words,  if nothing is specified  it is R Full. (Figures 1-27, 1-28 and 1-35)
2.        Same question about THRU for holes. If not THRU depth has to be specified. (Fig. 1-34)

Regards,

Sundar
 

Sundar,

It's nice to hear from you again.  The answer to your primary question is that you have already used the .040 in the calculation of the Resultant Condition of datum feature B (4.990-.040=4.950).  In this case, you don't get to use the .040 twice.  To understand why, we must understand how B is represented in a gage that would inspect the center hole.  Since the gage would represent datum feature B at its virtual condition of 5.030, any pattern shift allowed for the center hole would be reliant on the slop/airspace created by the departure of datum feature B from its virtual condition size (of 5.030) in that gage.  Since we already used up that .040 in perpendicularity tolerance when we calculated the resultant condition of datum feature B (4.990 + .040=5.030), the gage would be the same size as datum feature B.  There would be no slop/airspace between the gage and datum feature B.  There would therefore be no additional pattern shift for the center hole.  Had we not used the .040 in the calculation on the Resultant Condition of the OD (datum feature B's calculation on the top of page 199), then we could have used it for pattern shift on the center bore.  But we don't get it twice. 

As far as the center hole getting .400 diameter position tolerance at LMC, it does (of course) get that much.  And as far as the four-hole pattern (.370-.375 holes) getting it again because they are referenced to datum feature D at MMC, it would.  The reason is that the four holes are measured from different datums than the center hole (for positional movement).  Every time you are positioned from different datums, you switch gages (or set-ups).  And every new gage (or set-up accumulates tolerance (error).  So, each new set of location datums means a new gage.  And every new gage begins anew and can receive the tolerance from any feature represented by the gage. 

So, the simple answer here is that perpendicularity does not react like position does.  Being out of perpendicularity on datum feature B, in this case, eliminates slop in the assembly and the pattern shift that the four holes would have been entitled to.  But had we assumed perfect perpendicularity on datum feature B, the .040 would not have been used to calculate the Resultant Condition of the OD (datum feature B) and would instead have been used as you describe it in your email, as pattern shift for the center hole, raising the tolerance for the center hole of .400 diameter for movement (due to the MMC symbol after the .000 positional tolerance) by an additional .040 for shift (due to the MMC symbol after datum feature reference B).  But with either usage, the final answer to the problem would have been the same, having used the total amount of tolerance.

As to your general questions, I don't see questions there.  I see statements right out of Y14.5.  And that is the answer.  Because the Y14.5 standard says those are the rules, they are.  I know people always hate that answer, but not everything is true because of logic in the standards.  Sometimes it is just true because that is what everyone could agree on the day it was written.

I am leaving on a road trip tomorrow and am not taking my computer.  If you have more questions, please feel free to write, but realize I won't be able to respond until I return next week.

As always, I hope these answers helped.

Jim Meadows

__________________________________________________________________________

Subject: Straightness and Circularity

Greetings, Jim...

I've looked in both the ASME standard and your book to try to confirm or refute an idea of mine. I couldn't find anything to challenge my thinking, so I thought I'd ask you.

Can straightness and/or circularity apply to a hole?  If so, how does one measure it?  If so, what does one use for virtual condition?

Form tolerances for a pin in a (virtual condition) hole for inspection, I understand. I think that size and location are enough to control a hole. Comments?

Best regards..

Ted
 

Ted,

Straightness and circularity can most certainly apply to a hole.  Circularity can be inspected by a CMM (best using a constant contact scanning probe) or even a dial indicator attached to a rotating spindle.  Straightness is a more versatile control and can be used on a hole as a surface, axis (derived median line) or center plane (derived median plane) control.  If used as an axis or center plane control at MMC, it can be inspected with a gage made at the virtual condition (MMC minus the geo. tol. at MMC) size.  If used as a surface control, straightness, like circularity (which is always used as a surface control) generates no virtual condition and must be contained within the size limits (may not exceed an envelope of perfect form at MMC-according to Rule #1).  These controls (circularity and straightness) can be inspected with a dial indicator or CMM.  Of course, a roundness checking machine is made for the circularity measurement.

Size tolerance, under Rule #1 controls roundness, straightness and taper, unless you override it with a refinement surface control, or refine or loosen it with a control of straightness on the axis or center plane.   Then, position tolerance controls angles and location.  So, I would agree that size tolerance and position tolerance is usually sufficient to control most holes.  There are only four things that geometry can control, they are size, form, angles and location.  A hole's size tolerance controls its size and form, and a position tolerance controls angles and location.  That's all there is.

Hope this helps,

Jim

__________________________________________________________________________ 

SUBJECT:  Really Badly Applied Dimensioning and Tolerancing

Jim,

I was recently fortunate enough to find another job with the defense industry.  Having been laid off from the automobile industry, along with thousands of my co-workers, I was worried I would end up flipping burgers and wearing a paper hat.  But war is in now, so the country needs more equipment (tanks, guns, ship, jets, etc.) and disposables (bullets, bombs, grenades, etc.) with which to conduct it.

I'm grateful not to be poor and homeless, but I'm shocked at just how poorly the products I'm seeing are dimensioned and toleranced.  Don't get me wrong.  Things were far from perfect in the automobile industry, but the situation in the defense industry is ridiculous.  How do these products ever work?  From some of the nightly news shows and some of the reports I've personally seen, I think the answer is that they often don't.  And when they do, it is because each piece is hand fitted (ground, filed, bent and forced to fit), even though we are sometimes making them in large quantities.  How inefficient is that?  We could never have gotten away with that in the auto industry.  The cost of every mid-sized sedan would be $150,000 or so.  But they get away with it here!  Our tax dollars at work.  These people need training, and a lot of it.

Is there a solution to this problem that's likely to be implemented in the near future?

Ken

Ken,

No, there isn't.  Training is, of course, the easy answer.  But, tolerancing is something that is so complex, it takes a long time to learn to do it well.  And most companies, including those doing defense work, look for a quick fix.  I recently had a request for a 1-day "refresher" course from a Director of Engineering for his group.  I told him 1-day courses simply don't provide enough information, but I would be happy to do a longer course.  He wrote back and said his people only needed a refresher, because they already knew the topic.  And he said he had personally attended 1-day courses in the past that were very successful.  There are so many thing wrong with that statement, I hardly know where to begin.  But I'll try.

1.  Applying dimensions and tolerances to an assembly is a job as complex as any other profession.  You can't learn to do any job well in 1-day, unless it's on the level of learning to replace the cap on a toothpaste tube.

2.  If you think your group needs a "refresher" course, you must have noticed they aren't very good at using GD&T.  Noticing these problems should have alerted you to the fact that they aren't knowledgeable and don't just need a "refresher" course. 

3) If people are going to be any good at this, they need a series of full-blown courses.  Not even a full week of training is going to teach them to do this job well.  It takes at least several courses administered at calculated intervals.  The course should be of varying levels of difficulty (basic, intermediate, advanced) and with different job emphasis (design, inspection, manufacturing, gage and fixture design/use, tolerance stack-up analysis, etc.). 

4) This topic should be treated as though you were educating the people as thoroughly as in any major in college.

Of course, most companies and those supervisors, managers and directors in charge, will never believe that and even if they did, they wouldn't commit the time and money necessary to accomplish it.  That doesn't make them bad people.  It just means they don't comprehend the magnitude of the problem and the difficulty of training their people well enough to solve it at. 

Jim

__________________________________________________________________________

Subject: Gauge Tolerance and Part Acceptance

Jim,

After reading the appropriate sections of your book, "MEASUREMENT OF GEOMETRIC TOLERANCES IN MANUFACTURING", I believe I have an understanding of appropriate tolerancing for functional gauges. The question I have is can I backtrack from the gauge tolerance and say this gauge will accept a feature with a true position of a specific amount?

 
I have a .012 plus and minus .001 diameter pin connector located on .050 basic grid, with a true position tolerance of a diameter of .003 @ MMC to A and B (A being the lower row of pins, B being the left hand row of pins). Now if the gauge being used has holes the measure .018 diameter and are held to a true position of .001 (I'm not if this is at MMC so lets assume the gauge is RFS).

The Connector pin virtual condition is .016, in my opinion the gauge holes should be .016 +0000/-.0001, and the position tolerance should be .0003 at MMC ( or any combination of these tolerance). Since the hole diameters in the gauge measure between .017 and .018 and the holes in the gauge are being held to a position tolerance of .001 can I say that gauge will accept parts with a true position of  .0056  (the original .003 plus the additional .002 from the gauge hole sizes plus the .0006 additional position tolerance from the gauge).

 
Regards,

Bob

Bob,
I'm sorry Bob, but I just can't figure out what you are trying to do here.  The only sentence that I understood and really agree with is the one that says, "The Connector pin virtual condition is .016, in my opinion the gauge holes should be .016 +.0000/-.0001, and the T.P. tolerance should be .0003 at MMC."  If the pin has .013 MMC and a position tolerance of .003, then that statement is correct.  But the rest of it is difficult for me to understand.  If the virtual condition of the pins is .016, then the gage holes should be .016, not "between .017 and .018" (to check the position tolerance on the connector pins).  So, that's confusing. 

The gage holes are too big, so they will accept bad parts.  Gage tolerances don't add to the tolerances of the parts being inspected.  They subtract from it.  And even though the shafts being inspected are controlled at MMC, if these shafts are entitled to a "bonus" of position tolerance, they get it because they are produced smaller than their MMC, not because the gage holes have been produced too large.  So, the thing you are trying to do doesn't seem to be possible-taking the fact that the gage buys bad parts because its holes are too big and that the gage has tolerances and saying that proves the gages can accept pins that are out of position a certain amount.  This can't be determined. 

First, we don't know how much position tolerance the pins are entitled to until we know the pin diameter.  Second, the position tolerance on the gage holes subtract from the pins' tolerance, they don't add to it.  Third, yes their is some connection between 1) the gage holes are too big and 2) this affects the amount of position tolerance the pins may use and still be accepted by these (wrong) gages, but we can't know how much position tolerance the pins have used up, until we know what the pin diameters are as produced.  If you measured the pin diameters as produced and then subtracted that from the gage hole size, that would tell you how much out-of-position tolerance for the pins the gage hole will accept (if you subtract the position tolerance on the gage hole).

But, I have to say, the only solution that makes any sense to me here is to get new gages.

Jim

Jim,

I also believe that the supplier needs new gages.  In the meantime, I’m trying to quantify how much error will be accepted by the gage currently being used by the supplier.  From you previous response, I believe I can use the following formula:

Out-of-Position allowed by the gage=gage hole size minus actual pin diameter minus position tolerance on gage hole

So, in my case, we have:

Actual pin diameter: .012 (this is fairly consistent due to the manufacturing method)

Gage hole position tolerance: .001

Gage hole size:  .017 to .018

Out-of-position tolerance allowed by the gage=.017 minus .012 minus .001=.004

Since the actual gage holes vary from .017 to .018, I can say that the gage will accept parts out-of-positional tolerance between .004 and .005.

Bob

Bob,

That sounds right, unless the gage hole doesn’t use its .001 of position tolerance.  If the gage hole was perfectly positioned, you would have to add that .001 to the .004 to .005 of out-of-position tolerance (of the pins being gaged) that the gage holes would accept.

Jim  

Close Window