Close Window


Written, with help from students and clients,  by James D. Meadows
The Tolerancing Newsletter July, 2005


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

 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.


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,

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


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.
Subject: Composite Position Tolerance Question
Dear Mr Meadows,
Assume we have defined A, B, C datums. We have 4 holes with ō.164Ī.010. In the first case, we define the upper segment of the composite position tolerance as ō.080 with respect to datums A|B|C and lower segment as ō.008 with respect to A. In the second case, the upper segment is the same, but the lower segment is ō.008 with no datums. What will be the difference in the meaning of these two cases?
Thanks in advance,
Best regards,
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.

Subject: Primary datums and form


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?

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.
Subject: Use of Profile Tolerance Using a Center Plane Datum
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.

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).
Subject:  GD&T / Inspection Questions


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!

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 website and browse through their standards.

Hope this helps,

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,

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,
  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 wasnít enough money.  Well, I'm no longer working there, I was laid off.  I am now working at another company in Colorado.  Iíve 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 patientís 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 patientís 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.

Shown below is one version of the four tolerancing approaches that Victor sent.

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,

 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,


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 in their codes and standards publications section. 
James D. Meadows
Chairman Y14.43
Subject: Countersunk Screws in Tolerance Stack-ups
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.

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,

Subject: Threaded Holes and Their Chamfers
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?

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.

I agree.

Subject:  Question on Using Both Inch and Metric Tolerances

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.  Iím looking forward to taking another class with you in the future.


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,

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.



Shown below is the Two-Part Assembly Raj is referring to from my book on Tolerance Stack-Up Analysis


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.

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,

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 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.

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.

Close Window