Close Window


The Tolerancing Engineer Newsletter - January, 2012 our client company personnel and James D. Meadows using our ‘GD&T HOTLINE’


Subject: Inner/Outer Boundaries

Mr. Meadows,

I recently began working through your Workbook and Answerbook for Geometric Dimensioning and Tolerancing to start learning the basics of GD&T. The first problem in the workbook asks to convert specifications to equal bilateral toleranced dimensions generated by their inner and outer boundaries. The first specification is a 20 +/- 2 diameter hole with positional 2 at MMC referenced from datums A, B, and C at RFS.

It seems to me that the inner boundary should be 16 and the outer boundary should be 24 but the answer shows 16 and 28 respectively. I do not understand where the (22+6) comes from and I have not been able to find anyone who can explain this to me. Could you please clear up this matter for me?

Thank you for your time.



When features of size are referenced at MMC, as they depart from MMC a bonus tolerance of position is gained. This is to protect the virtual condition boundary. The virtual condition (inner boundary) is, as you’ve pointed out, 16. So, the MMC is 18 and 18 is allowed to move out of position by 2 millimeters. 18 minus 2 is 16. So, you’ve got to ask yourself, “What if the hole was produced at its LMC of 22? How out of position would it be allowed to be before the 16 millimeter inner boundary would be violated?” Since the LMC is 22, and 22 is 4 millimeters larger than the 18 millimeter MMC, a 22 millimeter hole would be allowed to be out of position 4 millimeters more than if it was produced at 18 (MMC). In other words, 18 minus 2 is 16 and 22 minus 6 is 16. So, a 22 millimeter hole is allowed to be out of position 6, and when 22 and 6 are added (instead of subtracted), you get 28.

If you think of the 16 millimeter dimension as the size of a gage pin located at “true position” to A,B and C and an 18 or 22 millimeter hole was produced, all you’d have to do is ask yourself, “How much could each hole move out of position before hitting the gage pin?” The answer is 2 millimeters for the 18 millimeter hole and 6 millimeters for the 22 millimeter hole.
I’m glad you are learning this. It sounds like no one around you knows the basics of GD&T. Bonus tolerance is one of the first things one learns. When you get a little more practice, everyone should be coming to you for the answers.

Jim Meadows

Subject: Idea Thieves


My boss steals all my ideas and passes them off as his own. He constantly calls me into his office to ask what I’ve come up with as solutions to technical problems faced by our company. Once I’ve told him, he calls a staff meeting, invites his boss and tells everyone who will listen what a great idea he’s had to quell the storm and calm the waters. He does this when I’m in the room.


The way he says it, without ever looking at me, I think he even believes that these ideas are his, once he steals them from me. Everyone thinks he’s a genius, but he has no technical knowledge at all. He has a degree in business (probably business ethics) and has no idea what should be done, other than to cling to me like a giant sucking creature, draining my ideas like a like a vampire sucks bags at a blood bank.

The good side to this is that, as long as he’s my boss, I’m in no danger of being laid off. He gives me a decent raise each time I come up for review, and he says I’m a reliable worker.

The bad side is that he tells everyone that I’m “task oriented” and that although I can carry out specific orders once he’s decided what should be done, I’ve never had an original idea in my life.

As the man warns me, “Times is hard. Jobs are scarce. I’m lucky to have a job.” But it just grinds me the way a person in his position can use this to lie, steal and cheat his way to success. I have to admit that violent thoughts and dreams have begun to dominate my days and nights. I used to work at the Post Office.



Although, sometimes in life, violence is the answer, in this case, technology might work against you. It’s just like my old friend Dead Man told me recently. He said he used to carry a gym bag with a sawed off shotgun inside, because he just never knew when the urge to rob a liquor store would strike. But he had to give it up because there are video surveillance cameras everywhere these days. They’re outside the store, inside the store and at every stop light. Dead Man says, “You can’t get away with anything in this electronic age!”


Your boss could have a state-of-the-art camera in his office recording everything you do. Remember, if you think ‘Times is hard’ where you are, it’s probably harder in prison.


Subject: Datum Question

Hi Jim,

I recently purchased your GD&T training course on the 12 DVD's. It took me the better part of a week to run through the DVD's and I've now kind of run through the book. I must say that it is a wonderful course!!! Thank you for all that you put into it. I know that I would do better going through the actual class live. I've been at this (GD&T) for a while, actually.

My question is regarding an actual relay that has locating pins, dowel pins, as well as flat head screws. It's a product that's been in existence for quite a while. Anyway, regarding the locating pins, which are the 2 diagonal holes on the 2 mating parts, that is seen on the left top side of section B-B. I'm wondering what the difference is when one datum is applied to the 2 holes & when 2 datums is applied, one to each hole.

I was thinking of making the mating planes the primary datums and then the center planes the secondary and tertiary datums to locate the locating pin holes and then use the locating holes as a datum to locate the other holes for the connectors, the guide pins (for the reeds), and the dielectrics.

[Side note: it has been recommended that one hole on the thin mating plate should probably be a slot or a larger hole, but this is what it is now.]

Thank you!


What you’ve described to me sounds like a logical approach. I assume you mean that the widths of the part in both directions will become datum features and generate the secondary and tertiary datum center planes from which you will locate the two cylindrical holes. As you know, you can’t just put a datum feature symbol on a center plane. It has to be put on the width which then generates a centerplane. If you do that, you should consider a feature control frame for the first width that states its perpendicularity to the primary datum. Then you should consider a perpendicularity control to tie the tertiary datum feature width to the primary and secondary datums.

Now, on to the cylindrical holes, which you will position to the datums discussed above. If you say that the 2 holes are a datum pattern and are referenced at their maximum material boundary, they will generate an axis halfway between their virtual condition boundaries. Think of two gage pins that are sized at the virtual condition (MMC minus their geometric tolerance). The datum axis of the two-hole datum feature pattern is halfway between those two gage pins.

If, instead, you make one of the holes a secondary datum feature and the other hole a tertiary datum feature and then reference the remaining holes to them in that respect, then supposedly the secondary datum feature is for location and the tertiary is for angular orientation (to stop rotation), and the datum axis is at the center of the secondary datum feature and the orientation (clocking) of the measurement is generated by the axis of the tertiary datum hole. But, according to the Y14.5-2009 standard, the gage would be the same as it would for the 2-hole pattern datum, and that would be the same as if you called each hole a separate datum feature, but referenced them in compound (such as D circled M dash E circled M).

The discussion of the “elongated hole vs. the round hole” for the tertiary datum feature is usually one that occurs when they aren’t certain manufacturing can hold the appropriate distance between the two holes and they want a larger positional tolerance for the tertiary hole’s position tolerance in that direction. It is done commonly on automobile panels, because they are so large and flexible it is difficult to hold the position of the tertiary datum hole. Generally, this isn’t needed for smaller, easier to manufacture parts. But, if they do that, it makes your decision easier on which hole locates and which one controls rotation. In that approach, the secondary round datum hole would be positioned to the planar datum and the two widths you were discussing. Then the tertiary elongated hole would be positioned back to the planar datum for perpendicularity, the round hole for location and maybe one of the widths to stop rotation. Then, subsequent holes would be positioned to the planar datum for perpendicularity, the round hole for location and only the width of the elongated hole for rotation. Try not to fall into the trap of making the entire elongated hole a datum feature, since the only degree of spatial freedom you need it to stop is rotation.
Hope this helps.


Subject: True position question - threaded hole

Mr. Meadows,

I’m not sure if you remember me, but you led a training session at our facility last year.

I was wondering if you could answer a question for me regarding using True Positioning on a threaded hole. I’ve attached a portion of the drawing for you to review ( I hope it comes through properly). This drawing is supposed to be interpreted in accordance with the 1994 Y14.5 standard.

When we calculate the True Position of the threaded hole, should we be using the pitch diameter or the minor diameter? Is Bonus Tolerance applicable to both the pitch diameter and the minor diameter? Just to clarify, I’m not asking if I can combine any possible Bonus Tolerance from both the pitch diameter and the minor diameter, I would just like to know if it could be applied to either one of them.


These parts are machined from 7050 aluminum. We inspect every part before we send them out for anodizing and they all pass at that point. The problem that I am having is that about 20% of our parts are failing final inspection after plating because one or both of these tapped holes is out of tolerance by .0001”. I am uncertain of the correct way to check the true position of a threaded hole. I was taught to use a best fin gage pin in the minor diameter and our QC department is using a threaded plug but I do not believe that they are making any allowance for Bonus Tolerance – if it is applicable. Any insight you could offer would be greatly appreciated.

Thank you,



Threaded holes derive a negligible, non-quantifiable amount of bonus tolerance from their pitch diameter. When the threaded holes are given a geometric tolerance like a positional tolerance that uses a projected tolerance zone, bonus tolerance is best utilized by using fixed-sized threaded gage pins that thread into the holes as part of a functional gage designed to check the position tolerance (or perpendicularity, angularity or parallelism tolerance) of the threaded holes. When the threaded holes are measured using the minor diameter, there is no way to utilize the bonus tolerance, since the minor diameter of the hole isn’t the functional portion of the thread that is engaged by the mating screw. In other words, any bonus tolerance derived from the minor diameter is not functional, therefore is a mistake functionally (and technically).

It is possible to measure the threaded holes position tolerance with a projected tolerance zone that uses a fixed size threaded gage pin when using other measurement techniques, like coordinate measurement machines, but it is difficult in that the inspector would be expected to use the clearance between the threaded hole’s pitch diameter and the threaded gage pin to “wiggle” the threaded gage pin’s axis into the projected position tolerance zone. That description is the best one to describe the amount of bonus tolerance the threaded hole is entitled to.

Hope this helps.

Jim Meadows

Subject: Symmetrical Parts

Hi Jim,

Here's what I'm wrestling with that I tried to describe to you yesterday afternoon. The rectangular bosses need to be in line. I'm thinking of perhaps Profile for the outline in the detail view. Do I then use basic dims from cut out to cutout? And what about the 3 to 1 rule you sometimes use when assigning tolerance relationships between the datum features?

Many very grateful thanks!,



The approach you used seems sound, so far. You worked your way in from the outside using centerplane datums. Measuring in from the edges would have worked, if you didn’t have symmetry concerns. Then you made a two hole pattern a datum feature pattern. That works. Another approach would have been to just make each hole a different datum feature and reference them as secondary and tertiary in subsequent controls.

The cutouts that are elongated can be positioned, but then there is the rest of the cutout to deal with. As you point out, you can control the entire cutout with profile but that means you can’t use plus and minus dimensions for the size. Basic dimensions would have to be used for the size and would make it harder to gage and be a more restrictive control, in that you would then have to use profile of a surface as the geometric characteristic symbol to tolerance the basic sizes as well as the orientation and location basic dimensions between the holes and the datums. If you position them instead of using profile, plus and minus dimensions can be used to show the size, and then basic dimensions would be used to locate the center of the elongated features. So, plus and minus tolerances would apply to the sizes and the position tolerance(s) would apply to the orientation and location.

The 3 to 1 rule is just for measurement repeatability. It is often overridden by fixed and floating fastener formulas and cost considerations. The rule is one I made up and use to remind me that the thing you measure from should have the tightest tolerance. It’s not a rule, just a rule of thumb. If the primary datum feature has a larger tolerance than your secondary datum feature (which is measured/related from the primary) then getting repeatable measurement data is difficult, in that you might be rocking on the primary datum feature more that the tolerance you are trying to hold to it.


Subject: Maximum Material Boundary (MMB)

Hi Jim,

How have you been?

I have a question about MMB. It is on the attachment. The first three examples are OK, but figure 4 looks like an exception to the rule. I’ve stated the rule I believe is applicable below the title MMB Modifier Explained.

Gene Cogorno

Hi Gene,

The applicable MMB is usually the virtual condition to the datum features that precede the datum feature with the MMB symbol. But, in fact, that statement, although simple, is incomplete. There are exceptions that one occasionally runs into. Yours is one of those. When the datum feature is a pattern, one must first account for the position of the holes within the pattern to each other. As you noticed, perpendicularity can't do that. So, you had to revert to the positional control (which can).

I ran into another strange one when I wrote my gray textbook on page 374 and had to spend page 375 explaining it. One would expect the applicable MMB to be the one that has the tightest tolerance to the datum that precedes the one with the MMB symbol. But on that one it wasn't.

That's why I hate the word "always".

See my exception below.


Since this gage is used to measure the position of the four-hole pattern, the location of datum feature D is not a factor in the size of the datum feature simulator’s radii. Therefore, the datum feature simulator that represents D has radii that are altered by only half the profile tolerance to A (1 divided by 2 equals 0.5).

If this gage was, instead, used to measure the position of datum feature D, then the radii on the gage for the datum feature simulator for D would be altered by half the sum of the profile and position tolerances (1.4 divided by 2=0.7).


Subject: Noting abbreviations on prints


There is a debate here about abbreviations used on prints. I have always used lb for pound and in-oz for inch/ounces. We have an engineer who now wants to use LB for pound and IN-OZ for inch/ounces. He states the Y14.5M states it should be upper case for everything except for millimeters (mm). I cannot find it. Is he correct? Thanks for your assistance.



Y14.38 is the standard on Abbreviations and Acronyms for Use on Drawings and Related Documents. You can buy a copy at

Y14.5 says almost nothing on the topic. However, in Y14.5 section 1.5.4 (Combination SI Metric and U.S. Customary Linear Units) it states: Where some inch dimensions are shown on a millimeter-dimensioned drawing, the abbreviation IN shall follow the inch values. Where some millimeter dimensions are shown on an inch-dimensioned drawing, the symbol mm shall follow the millimeter values.

Y14.38 has 130 pages on how to show abbreviations and acronyms on drawings and in text.


Subject: GD&T Certification Test

Hello James,

I am preparing to take the ASME Senior GD&T certification test again, having scored in the low seventies earlier.

I have a question regarding purchasing one of your books, in lieu of attending your course which I would prefer, should I purchase your Geometric Dimensioning and Tolerancing-Applications, Analysis & Measurement per the ASME Y14.5 2009 standard or your previous book that is per the ASME 1994 standard. I understand the test is based on the 1994 standard which should be used in parallel.

Any suggestions in preparing for the test would be greatly appreciated.

Best regards,



On my website I sell a test and an answer book that is about three times the size of the one given by ASME. It would probably be the best supplement to just studying the Y14.5M-1994 standard. If you want to get one of my books to help you pass the test, that would be helpful too. Even the books per the Y14.5-2009 standard state which rules are per Y14.5-1994 and which rules are per Y14.5-2009 and which rules are per both.


Subject: Question about new profile tolerance


I have purchased Your “NEW Rules” for ASME Y14.5-2009 training manuals and your book “Geometric Dimensioning and Tolerancing” for Y14.5-2009.

I have found both of them to be very helpful.

I have a question regarding the new Unequal profile tolerance (symbol “U”).

I understand how it works going around the O.D. of a block.

My question is what happens when the profile is on a pocket in a block?

Do you treat it like max. material as shown in the attached drawing figure #2?

Please review the attached drawing and please let me know if figure #1 or figure #2 is correct.

Your books give an example of a block O.D., but does not show a pocket.

I want to be sure I understand it correctly. Thank You for your time.

Thank you,



The tolerance number that appears after the circled U is the portion of the profile tolerance that adds material to the part. That means that cavities/holes/female features are allowed to get smaller by that amount and shafts/male features are allowed to get bigger by that amount. This statement now appears in my GD&T books written per ASME Y14.5-2009.

Hope this helps.


Subject: Questions on Runout


I have taken a few of your classes and at this point I’m studying for the senior level exam. A few people here have already passed the exam and have consequently made flash cards for the rest of us that have yet to take it. One of the questions they came back with that is said to be on the exam is as follows:

“Does runout control straightness?” … this doesn’t specify Circular or total. After researching I found that circular does not! While Total does. How is it that they can ask a question on the exam of that nature?



Both circular and total runout control straightness of the axis. As you point out, only total runout controls surface straightness.


Subject: Question on runout


I took your class many years ago when I worked for Bulova back in the 80's. I have moved on and now am at an aerospace company. I was wondering if I could ask you a question on interpretation. How is runout checked when the datum is a perpendicular face, and they want the bore runout to within .001 to datum A the face.

I hope you can help.



If the primary datum feature is the face and the secondary datum feature a cylinder, then orient the part perpendicular to the face and then set-up on the diameter to generate an axis to runout to, that is created by the minimum circumscribed cylinder about the secondary cylinder that is also perpendicular to the primary face plane (created by a minimum of three points of high point contact on the surface).

If there is only one datum feature referenced in the runout control and it is the face, then the control is simply wrong. Runout is to a datum axis.


Subject: Profile Tolerance inspection using CMM

Hi James,

I'm really enjoying reading all about GD&T in your books. I'm hoping, one day I can meet you and attend your GD&T class in the USA.

Anyway, I need your help for a better understanding as follows: Our CMM measured the surface profile and the results are shown below:

Let say:
Point 1:
X nominal=10
Y nominal=20
Z nominal=30

X actual = 10.1
Y actual = 20.1
Z actual = 29.8

X deviation = 0.1
Y deviation = 0.1
Z deviation = 0.2

Profile tolerance call out is 0.5

Actual profile tolerance deviation from basic (software generation) is 0.489

After checking, the software is using the formulae as below:

Profile tolerance deviation from basic= 2 times the square root of deviations in X˛ + Y˛ + Z˛

Just to confirm, is the above formula generated by our software correct or wrong? If wrong, what is the correct formula? Thanks again for your help.



To calculate a point’s deviation from its basic location in space in terms of a total width or diameter (for an equal bilateral tolerance zone), the formula is correct. However, there are other ways to express a profile’s deviation from basic. For example, it could be expressed as a radial deviation from basic, using the worst case for the largest plus deviation and the worst case for the largest minus deviation. The formula would then be the same, but to express each as a radial deviation, the “2 times” portion of the formula would be eliminated. This would tell you the direction of the deviation and the amount of maximum deviation in both the plus and the minus directions reported separately. Also, if the profile tolerance isn’t equal-bilateral, but rather unilateral or unequal bilateral, the formula would not show the deviation from the mean profile, since the mean profile isn’t shown.

The formula you are using is normally used to calculate the deviation from true position of the axis (center point) of a sphere. The software writers for your CMM have apparently used it to find a profile of a surface deviation of each point on the surface individually. Again, this would only work if the tolerance of profile was equal bilateral, and you wanted to express the deviation as being out an amount that could be directly compared to what is in the profile feature control frame. This formula is adequate in some cases, but wouldn’t tell you much about the deviation. For example, it wouldn’t tell you which way the point has deviated from basic. Also, to even tell how much it has deviated radially, you’d have to divide the answer by 2.

By the way, there is an ASME standard numbered Y14.45 currently being written to show how variables collected data should be reported. Until it is published, there is no standard rule on the reporting of measurement data.

Hope this helps,


Close Window

© 1997-2015 James D. Meadows & Assoc., ALL RIGHTS RESERVED

Site Designed & Maintained by VIRTUAL GOLDMINE