Close Window


The Tolerancing Engineer Newsletter - December 2014 our client company personnel and James D. Meadows using our ‘GD&T HOTLINE’

Subject: New DVD training series’ for Geometric Dimensioning and Tolerancing and Tolerance Stack-Up Analysis available from Website


I recently visited your website and saw you had added two new film/DVD series. One is entitled Tolerance Stack-Up Analysis and the other is, of course, Geometric Dimensioning and Tolerancing (per ASME Y14.5-1994 and 2009). How do these differ from your older GD&T DVD series?

John from San Jose


GD&T DVD series: The old DVD GD&T series was filmed in 1994. The new one was filmed and edited this year. One difference is that I was much younger and agile then. Another is the new GD&T DVD series is based on everything we knew prior to 1994 and everything we’ve learned since, as displayed in the ASME Y14.5-2009 Dimensioning and Tolerancing standard. Also, I’ve personally learned a lot in the last 20 years, and I think some of that knowledge shows up on the new DVD series.

Tolerance Stack-Up Analysis DVD series: This course shows several of the most logical and mathematical approaches to understanding how plus and minus and geometric tolerances stack up in assemblies, and how to analyze these stacks. Three different methods for doing “stacks” are on display in this DVD series. All are useful in different situations. Tolerance Stack-Up Analysis is just one of those topics they should have taught most mechanical engineers and designers in college, but didn’t. It provides a valuable understanding of GD&T that GD&T courses don’t have time to delve into. It is a must-have piece of the GD&T puzzle that is essential to thoroughly understanding Geometric Tolerancing.

The website allows you to buy the entire GD&T or Tolerance Stack-Up Analysis series, or individual lessons can be downloaded from our online store here.


Subject: Flatness and Perpendicularity of a Center plane vs. a Surface


I saw the attached on one of our supplier's drawings. I just want to get your take on the Flatness and Perpendicularity requirements and how to interpret them. Or possibly they are an unacceptable fashion of modifying.




I've attached a couple of illustrations from one of my textbooks to explain the difference between Flatness of the Derived Median Plane and Perpendicularity of the Centerplane.

Since the flatness control requires the inspector to find the median points by probing the surface on each side of the width (normal to the actual mating envelope), then averaging the readings to find the flawed median plane, and perpendicularity just wants the inspector to probe the actual mating envelope simulator (a gage block in the illustration I've attached), they can be used together.

If they were both looking for the same thing and used the same tolerance, since perpendicularity is the more restrictive control (also controlling the angle to the datum referenced), the flatness control would be redundant. So, if these were surface controls (flatness of a single surface vs. perpendicularity of a single surface to a datum) the flatness control would be redundant. But that isn't the case on the drawing you sent me.

Although what they asked for on your drawing is unusual, it is legal and not redundant.


FIGURE 6-5 [Measurement of Flatness of the Derived Median Plane]

FIGURE 7-13 [Perpendicularity of a Centerplane’s Actual Mating Envelope to a Datum Plane]


Subject: Gage Measurement vs. Probing

Mr. Meadows,

Thanks for taking the time to read this. A very long time ago when I worked for Dana Corp, I was a student in one of your seminars on gaging in Milwaukee.

I’m stumped on measuring a particular part while still in the lathe without the aid of any type of scanning or probing device. Any advice would be much appreciated. See attachment.



This would be relatively simple to design a gage for, if the MMC symbol (circled M) was used after the geometric tolerances and the MMB symbol (circled M) was used after datum features B and C that are referenced. That gage would consist of two large shafts with a smaller connecting rod between them. The connecting rod would allow at least one of the larger shafts to slide (see sliding fits in ASME B4.1 and B4.2). The large shaft simulating datum feature B would be represented at a diameter of 8.873 (the virtual condition of B) and the large shaft simulating datum feature C would be simulated at a diameter of 8.994 (the virtual condition of C). The smaller connecting rod could be at any size, since it is the sliding fit that matters.
The problem is that no circled M’s are used, so no gage is viable. You need probing or scanning devices, unless someone changes the part’s design requirements.



Both bores are press fits, thus, RMB. Really, the problem is these’re made in a lathe instead of a large machining center. They have to flip the part to make it, adding set up error in the second set of operations and the potential for a failed inspection.

I think we’ll probably buy a couple of your books and I’m going to lobby to have our quality inspector go to one of your seminars in Milwaukee.

Thanks for your insight.


Subject: Coplanarity vs. Flatness, Parallelism and Perpendicularity

Hi Jim,

I took your course in Huntsville Alabama a couple of years ago. I recently started working for a company that makes the glass refrigerator and freezer doors for grocery stores, gas stations, liquor stores, Walmart… and they have for around 56 years. They have many extrusions and one that I’m working with looks somewhat like the figure attached. The GD&T on it is a bit ambiguous to me. The extrusion sits on the radii as it is positioned in the attachment and there is a wall on the left side of it where it is placed for its function. The first/top figure is what it looks like on the old drawing and the second/lower figure is where I started heading with it. Your direction would be greatly appreciated!

Do you address this type of situation is any of your books or training? I have several of your books and the video training from 1994. I’m curious about the newer training that is on your web site.

Many Thanks!



It would appear that they have one gap in their knowledge. Flatness, perpendicularity and parallelism are not capable of controlling coplanarity (putting multiple coplanar interrupted surfaces in a single continuous tolerance zone). If you want coplanarity for any of these 3 controls, you must replace the flatness, parallelism and perpendicularity symbols with a profile of a surface control. Datum references required for any angle control are used with the profile of the surface control. The profile controls will state the number of surfaces being held (coplanar and parallel, coplanar and perpendicular or coplanar and flat) to that requirement by using 3X or 4X or whatever the number is near the control. Stating 3 SURFACES or 4 SURFACES or whatever number of surfaces is also acceptable.

I do cover this in my books. If you have the grey textbook, look at the section on coplanarity in chapter 8.
Hope this helps,


Hi Jim,
Is my second figure on the attached doc correct? (The bottom of the part is not what I originally thought. I noticed when I looked at another view on the drawing.)



It’s correct Melinda. It isn’t the same exact sequence of controls they used. I was wondering why they assigned a datum feature A and never referenced it. You cleared up that problem by referencing datum A in one of your controls. One thing I would suggest is that you hang the A and the B above or below the profile controls used on the surfaces that define A and B, but only if you want datum planes A and B to be created by multiple surfaces. Right now, I’m not sure how many surfaces are used to create A and B. The way you have it, the answer looks like just one. If that’s not what you want, it needs to be corrected.

Hope this helps.


Subject: Calculating the Correct Least Material Boundary (LMB)


I’m doing a tolerance study where I’m trying to determine the correct LMB of Datum feature G (see below) in determining the position tolerance of the pin in Section S-S.

I am unsure whether to count G’s 0.15mm position tolerance or only to count the bonus tolerance of 0.05mm. Please advise.
Thanks in advance.



Since G is a shaft, the correct LMB is to the datum that precedes it in the control under consideration. In the control under consideration, only D precedes G. So, the correct boundary is the one generated by the positional control on G. LMB just means the Virtual Condition. Virtual condition under the LMB concept is the constant inner boundary of the G shaft. Unfortunately, since G is implied at RFS in its position control, it has no constant boundary. But it does have an inner boundary. That inner boundary, if G is not banana or snake shaped (no axial curvature), is the LMC minus the applicable geometric tolerance at LMC. The LMC of G is 4.43. The applicable geometric tolerance at 4.43 is the same as it is at all sizes (RFS) 0.15. So, the inner boundary you should probably consider is 4.43 minus 0.15 equals 4.28. However, if G is banana shaped, the inner boundary could be as small as 4.28 minus 0.05, or 4.23.


Subject: Calculating “Bonus Tolerance” and Virtual Condition


I’m hoping you can help me answer the question in the picture below? What is the bonus tolerance on the dimension below? And what is the virtual condition? This will help a month long back and forth with one of my suppliers.




The virtual condition of the hole is a diameter of .286 (.306-.020).

There is a potential (depending on produced sizes) of a bonus growth in the hole’s positional tolerance of .010. Bonus tolerance always comes from the size tolerance of the feature.

There is a potential datum feature shift of the hole’s position tolerance (movement of the tolerance zone, not growth) of the difference between the LMC of datum feature A and its virtual condition in its relationship to datum B.

Unfortunately, I don’t see a geometric tolerance relating datum feature A to datum plane B (in that order), so this virtual condition can’t be calculated. The drawing needs to be corrected to include a geometric tolerance relating A to B in order to calculate this virtual condition. Even if B is related to datum A with a perpendicularity tolerance, since A is used after B in the feature control frame in question, we need to reverse this and relate A to B instead to calculate the virtual condition of A to B. In the meantime, it would be safe just to say the shift due to the maximum material boundary symbol after A is limited to the size tolerance of datum feature A.

I hope this helps.

Jim Meadows

Subject: Profile Tolerancing


You trained several of us in Huntsville, Alabama a while back and said that if we had a question to write you and you would try to answer it.

We have a part and we are trying to control the inside surface with a profile. The inside has a small step in it and we aren't sure of the best way to control the feature, we are having to use the AMSE Y14.5-1994 version. I have a generic part with similar features that I am sending in a pdf file, two views with different approaches, are either right? Do you see a better way to control the inside surfaces?

Thanks for any input,



The first example (on the left of the page) is better than the other, but the angle of the cone needs to be shown as basic. It could be two basic diameters (one on each end) or as follows:

The inside diameter would be likewise defined and then profiled to the conical datum. If you also want to use the end of the part as a datum feature, you can. Then define the location and depth of the slight rise in the conical surface with basic dimensions and state the extent of the profile control as including that. That might be done by putting an X on one end of the conical surface and a Y on the other and then below the profile control use the “between” symbol to show the profile applies between X and Y. That will eliminate the need to use the two profile controls you’ve shown that run vertically.


Subject: Measurement Data Reporting


I’m currently working to validate a part that contains a hole pattern with a composite positional tolerance. I’m entering the location and tolerance data into a spreadsheet to show pass/fail for the pattern. The 2nd line of the composite tolerance has me stumped as to how to best show pass/fail. Can it be shown in a spreadsheet or is it typically shown graphically? Please let me know if you are willing to provide your assistance and I can send you a sketch of the problem.




There is no standard on how to report inspection data. One is being written and will be ready for sale by ASME within the next couple of years. It will be designated ASME Y14.45. In the meantime, you are left to your own judgment as to how to most effectively convey the data. I used to plot it out and submit the representation of hole axis locations graphically.

Subject: Repetitive Features

Hello James,

I took your GD&T class in Huntsville, AL and I have come across a drawing that I am unsure how to dimension for parallelism. I have attached a PDF showing the surfaces that I would like to have constrained. Please provide any direction that you can offer.

Thank You,



Extend a line between two of the surfaces you want to be parallel to each other. Label one as datum feature A (or whatever you want). After or below the datum feature symbol for A, add a local note that says, “7X INDIVIDUALLY” (if you have seven sets of surfaces). Then point with a leader line at the other surface and make it parallel to A. After or beneath the parallelism control add a note that states, “7X INDIVIDUALLY”.

That should do it. It’s the same principle we use for counterbored holes. We position all the pilot holes as a pattern to A. B and C, then point at one and call it datum feature D (7X INDIVIDUALLY for example). Then we position the first counterbore to D (7X INDIVIDUALLY).

Hope this helps.


Subject: Measuring Screw Length Gage Laser Lines


I have taken all of your GD&T classes offered by James D. Meadows & Associates, Inc. and had a hopefully quick question about tolerancing on our Screw length gage laser lines.

Here’s a snap shot of the print:

In the past, we have measured laser lines like this to the .197 dimension between each individual measurement (for example, measuring from the 100 to the 95 laser line, making sure it is between .187 and .207). Is this correct or should we be measuring from the end of the part (Datum A) and add the appropriate number of .197s to the 1.315 to get the total length from A? Please let me know ASAP.




Both, actually. The position tolerance applies from the datums referenced and between the features being positioned. If you measure each feature from datum A (by doing as you said, adding the basic dimensions together to get the perfect location from datum A), and the center plane of the feature is in the .020 tolerance zone (plus and minus .010 centered about that basic dimension you have calculated from datum A), then you have also verified the feature to feature requirements.

Hope this helps.


Subject: Calculating the Correct Maximum Material Boundary (MMB)

Hello Jim,

I got a question, if you don't mind. It is about size/shape of maximum material boundary D in case (c) in fig. 4-16 from Y14.5-2009. I am in a middle of a discussion with a person saying that in this case the shape of MMB is not a cylinder of dia. 7.5, but an obround geometry of 7.3x7.5.

His argument is something like this:
"The suggested interpretation does not match the set of allowable places 'D' could get to. If one took all the possible parts that met the requirements applied to D and transformed them to no longer include C, then it is an obround. Picture the view as if standing at the center of B; would D ever appear to be more than its MMC and perpendicularity tolerance wide? Without a reference to C, there is nothing that fixes the direction of the view and so nothing that causes adding a location tolerance to the width."

As you are a member of Y14 committee and most likely are well aware about the logic hidden behind the case (c), could you help me with understanding this?

Thank you very much.



The rules in the 2009 Y14.5 standard are very clear that every datum feature of size is simulated at its basic location (whether it is secondary or tertiary) and at its virtual condition. The question is really a gaging question. How would you represent B and D in this situation? The answer is that both would be represented at their basic location from each other and at their applicable virtual condition and by a gage hole or pin that is the same shape as the datum feature.

One could argue that it was not defined that way in the 1994 version of Y4.5, but it is certainly true in the 2009 revision. We had to change some of our gages in the Y14.43 standard (2011 revision) because of this rule change. It was also the reason that a datum feature translation symbol was added to the 2009 standard to allow the equivalent of datum feature D’s simulator to translate along a line toward and away from datum B. But without that translation symbol the gage pin and hole are stationary, basically located from each other and cylindrical in shape.

With the current rules, the 4-16 illustration is correct.

James Meadows
Chairman ASME Y14.43-2011 Dimensioning and Tolerancing Principles for Gages and Fixtures

Subject: GD&T Certificates vs. Geometric Dimensioning and Tolerancing Professional
(ASME GDTP Certification)

Good day James,

Can you please provide me with a little information regarding your Dimensioning and Tolerancing Certificate class? I understand that the University of Wisconsin at Milwaukee offers a Three day and a nine day course. Ultimately, I am seeking a ASME GDTP Certification.

What direction can you recommend for me.




The course that is offered early next year at UWM is a Level 1 GD&T course. I also teach an Advanced GD&T course there and a Tolerance Stack-Up Analysis for GD&T course and a Designing, Dimensioning and Tolerancing of Gages and Fixtures for GD&T course. A certificate of course completion is given by UWM for each course and a special certificate is given if 3 of the GD&T courses are completed by an individual.

ASME gives tests for Geometric Dimensioning and Tolerancing Professional certification. Two levels of this certification are available, a technologist level and a senior level.

How to prepare to take the ASME GDTP test is up to the judgment of the individual taking the exam. I’ve taken and passed the Senior Level Exam and would recommend to anyone wishing to pass either the technologist or the senior level exam to take at least a basic and an advanced GD&T course and to then study the Y14.5 standard, on which the test is based, for at least a month. Study of the standard should be intense, since many of the exam questions are rote memorization of the rules in the Y14.5 standard.

Good luck and I hope to see you at one or more of my GD&T courses next year.

James Meadows

Close Window

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

Site Designed & Maintained by VIRTUAL GOLDMINE