Close Window


The Tolerancing Engineer Newsletter - November 2009 our client company personnel and James D. Meadows using our ĎGD&T HOTLINEí


Subject: Shaft Runout



You taught a class here at my company a year or so back and I found it to be very informative.

I have a question on how to specify shaft runout to the axis of rotation of a motor and specifically how to label a datum.


Would you say that attached sketch is properly defined for checking individual shaft runout without a functional gage that would combine Perpendicularity, Concentricity and Runout?

Thanks for any insight you can provide on this.










Thanks.  I look forward to coming back to your company.


There is a rule in Y14.5 that states that datum features are identified on drawings by means of symbols.  These symbols relate to physical features and may not be applied to centerlines, center planes or axes.  This is avoid confusion about which diameter generates the datum axis.  An inspector must know what diameter to chuck up on, grab or probe to generate datum axis A.  So, putting the datum feature symbol on what could be the axis of several different diameters is not legal and it isn't specific enough.  You must pick a specific diameter, then attach the datum feature symbol to that outside or inside diameter.


Circular runout does not control the perpendicularity of a planar surface.  It just equalizes material on each side of the datum axis, so that it doesn't wobble when rotated.  Total runout does control flatness and perpendicularity of a planar surface to a datum axis.  So, if you want the planar surfaces to be perpendicular to datum axis A, just replace the single arrow (circular runout) with the double arrow (total runout).


Circular runout used on a diameter usually controls its roundness and its coaxiality to the datum axis.  But on your diameter, the size tolerance is so tight that it takes over the job of controlling the roundness, straightness and taper of the surface.  Rule #1 states that the size tolerance controls the surface form, unless overridden by a tighter control.  All that leaves for the circular runout to control is the centering (coaxiality) of that diameter to the datum axis for balance.  Total runout would be capable of controlling cylindricity (roundness, straightness and taper), but only if the total runout tolerance was tighter than the size tolerance.  Both total runout and circular runout control the centering (coaxiality) of the diameter to the datum axis.


I hope this helps, and that I get to see you again some time.





Subject: Re: Rule Number 1: Does it also controls form variation such as flash.


Hello James,


I enjoy reading your extensive info regarding G,D,&T.  It's amazing how some people are allowed to guess at the interpretation G,D,&T and of "Rule Number 1".  To help me end an argument and promote your expertise, can you help me convey the following.


This company seems to think the rule number 1 doesn't have any control over a form variation such as plastic flash.  Without additional notes, does rule number 1 in any way not apply to plastic flash?????  And, is there any quick reference you know of that states this???  And, is there an appropriate flash allowance note that you know of to supplement rule number 1 for the allowance of flash?


High Regards,







I hate to be the bearer of bad tidings, so I have attached the appropriate page from the standard ASME Y14.8-2009-Castings, Forgings, and Molded Parts.  It says, "Gates, riser stubs, flash, etc., may exceed perfect form boundary at maximum material condition (MMC) unless otherwise specified."






Subject: How Best to Purchase your Books and DVDís


Hello Jim,


When purchasing your G,D,&T books and DVDís for use, who Should I purchase it from to get the best price and speed of delivery?


High Regards,







Any of my books can be purchased from my website or by phone at (615)824-8644.  This is usually faster and the middle man gets cut out.





Subject: Senior-Level GDTP


Hello Mr. Meadows,

I hope this finds you well...

First of all, your Dimensioning and Tolerancing book (yellow cover) was my greatest resource - along with the Standard, of course - in passing the Senior-Level GD&T exam - a very well-written book.  I keep it at work.

I am starting to read my newest purchase - your GD&T book based on the new 2009 standards - obviously, yet another good book.

I have a few questions.

Before I continue any further with those questions, and it really is only a few, knowing your time is very valuable, do have a few moments to correspond with me, a fellow GDTP Senior Level "Club" member?





I am well, thank you.  I appreciate you purchasing and using my books.  It's always nice to get praise for my work.  We all need that from time to time.


I congratulate you on your success at being a certified GD&T senior professional.  Itís gratifying that I played a small part in your success in passing the test.  Iíve been receiving a lot of ďnotificationsĒ lately from professionals who have passed the Geometric Dimensioning and Tolerancing Professional Senior Level exam.  They are from people who wanted to thank me for teaching them what they needed to know to pass the exam and people like you who have gotten what they need from my books or DVDís.


Itís interesting to me, in that I donít teach or write books specifically to pass the exam.  Itís just that what I teach and write apparently allows people to easily pass the exam.


I'm like a lot of those people, just a technical geek who found a fit between things that interest me (math, logic, a blend of manufacturing, inspection and design skills I've both studied and picked up along the way) and a subject that I can make a living at.  I enjoy being able to work on a wide variety of products as a consultant and learning from those professionals I work with and teach.


I'm always here for you if you have a technical question or just want to verify something you think is true, but aren't certain of. 


Best of luck.


Jim Meadows


Subject: Conical surface as datum


Dear Mr. Meadows,


One question left unanswered in my training is the use of a revolved surface, other than a cylinder, to establish a datum axis. For example, I would like to assume that a Datum on a leader attached to the surface of a cone would establish the axis of the cone as the datum. I might also place an "all around" symbol on the leader to insure the horizon line of the cone is not mistaken for the datum instead of the axis. I would greatly appreciate your feedback on this subject.






Ps. Is the price structure for your on site training listed on your website?





I've attached a couple of illustrations from one of my new books to explain conical features that are used as datum features.  Don't worry about attaching an "all around" symbol to the leader.  When you specify a cone as a datum feature, you always generate a datum axis at its center and also a plane at the apex of the cone from which to measure.  I've also shown an illustration of how the ASME Y14.5-2009 dimensioning and tolerancing standard allows us to override the plane at the apex of the cone, if you want to establish another datum from which to measure distance in that direction.


The ASME Y14.5-1994 version of the dimensioning and tolerancing standard didn't mention cones used as datum features (although it wasn't specifically forbidden).  The ASME Y14.5-2009 standard shows that conical features can be used as datum features (as I've shown in the attachments).


On-site workshop quotes are handled by Jeannie Winchell from my office.  She would be happy to send you a quote, but would need to know how long a course you would like, how many people would be attending and specifically what course you would want (basic, intermediate or advanced), what year of the Y14.5 standard you'd like covered (1994 or 2009) and when the workshop would be held.  She would be happy to call you or it could be handled entirely by email if you'd prefer.


Hope this helps.  The illustrations follow.



Illustrations of a Conical Datum Feature


Means this:  Datum feature A generates an axis (which consists of two planes intersecting at a 90 degree angle) and (from a point) a datum plane.  This means that conical datum feature A generates three datum planes.  The 12.5 holeís axis must intersect datum axis A and be 38mm from the tertiary datum plane also constructed by datum feature A to within the holeís position tolerance of a diameter of 0.1 at MMC.


Specifying or Overriding the Degrees of Spatial Freedom-A Truncated Cone



One of the most practical uses for overriding spatial degrees of freedom created by datum features is for the conical primary datum feature shown above.  Cones are designed into many product lines throughout the world and sometimes are the most functional feature on the part from which to locate. 


Since the conical primary datum feature, as shown above, not only generates an axis for positioning the 10 millimeter hole, but also a datum plane at the apex of the cone, it creates a situation where one may wish to choose another datum feature for location of the hole along the axis of the cone.  The problem is that since the cone is the primary datum feature, that longitudinal (z) degree of spatial freedom has already been stemmed by the plane at the apex of the cone. 


Overriding that degree of freedom is now possible per ASME Y14.5-2009 by listing the degrees of freedom controlled by the conical datum feature A [x,y,u and v], but not listing the spatial degree of feature down that axis [z].  A subsequent datum feature is referenced, in this case B, and the z degree of freedom is listed as being controlled by it.  In this way, we can have the 10 millimeter hole be perpendicular to datum axis A and intersect datum axis A, but hold its 24 millimeter basic location from datum plane B (all to within the positional tolerance of a diameter of 0.2 regardless of the feature size).




Subject: Question about Tolerancing a Slot Pattern


Hi Jim,


I would like to ask you a question on slot location if you have the time.

Please see the attached powerpoint - a picture is worth a thousand words.


I am trying to geometrically tolerance slots from a datum and also control the two ends of the slot to each other. You must have seen this a thousand times.


Thanks in advance for your help. I am looking into taking your Geometric Dimensioning and Tolerancing class for the Y14.5-2009 standard.









The size tolerance on each slot controls their relationship for size and form. 


Composite Tolerancing (PLTZF)-First Level of Control-Pattern Locating Tolerance Zone Framework:

The position tolerance controls the relationship of the centerplane of each slot to the datums referenced in the pattern locating tolerance zone framework (upper lever position control).  The basic dimensions should be shown from datum F to the center of each slot.  It controls the movement (location) and orientation (angle) of the centerplane of the slot from the datums to within 0.04. 


Composite Tolerancing (FRTZF)-Second Level of Control-Feature Relating Tolerance Zone Framework

The location of the slots to each other is controlled to within 0.02 (this lower level of control is called the feature relating tolerance zone framework).  This is also a centerplane control. 


Everything would be correct if the basic dimensions were to the centerplane of each slot, instead of to the edge.




Subject: Gage Dimensioning and Tolerancing


Hello Mr. James Meadows:


Compliments, I am enjoying your "Workbook and Answerbook" for GD&T-2009.


Did you design the gage purposely this way?

I may not understand something? ISBN: 0-9714401-7-4 problem 50 (page-93) has a solution (page-248). Possible interference fit in a worse-case scenario of a hole size smaller than the corresponding largest worse-case shaft size.


Some feedback would be appreciated.







Functional gages are designed at the virtual condition boundary of the features they inspect.  The recommended gage tolerancing policy of the ASME Y14.43-2003 standard (a committee I chair) is to accept no out-of-tolerance parts.  Therefore gage pins are all plus tolerance and gage holes are all minus tolerance.  Since no out-of-tolerance parts are to be rejected, a small percentage of borderline, technically in-tolerance parts will be rejected by such a gage.  There are two gage tolerancing policies that fit this requirement. One policy is called Absolute gage tolerancing (which allows no bad parts to pass, even in theory).  The second policy is called Practical Absolute gage tolerancing.  The gage you are referring to in your email uses the gage tolerance policy called Practical Absolute gage tolerancing, which means that although a mathematical possibility of the gage buying an out-of-tolerance part exists, the gage will, in practicality, not accept a bad part. And, as you have noted in your email, this policy will reject some (very few), borderline technically in-tolerance parts. 


Functional gages check geometric tolerances (referenced at MMC and MMB) and the virtual condition boundaries they create (which is what the gage pins represent).


GO gages check maximum material condition and use the recommended gage tolerancing policy called Absolute that also says all gage pins have only a plus tolerance (no minus tolerance).


There are other gaging policies described in Y14.43, but not recommended.  One of those policies is called Optimistic gage tolerancing.  Optimistic gage tolerancing allows some borderline out-of-tolerance parts to pass inspection.  Optimistic gage tolerancing says that all gage pins have only a minus tolerance, no plus.


Tolerant gage tolerancing allows both a plus and minus tolerance on gage pins and gage holes.  This is the worst policy, in that the inspector doesn't know whether the gage is going to be made in the range of sizes that accepts borderline bad parts or rejects borderline good parts.


If you are really interested in gages and how they are designed, dimensioned and toleranced, please get a copy of ASME Y14.43-2003-Dimensioning and Tolerancing Principles for Gages and Fixtures, or a copy of the textbook that goes with the workbook of mine that you have.


Hope this helps,


James Meadows


Subject: Dimensioning Question about Runout


Hi Jim,


Hope things are going well for you.  We are busting our butts in the engineering dept here.  Production is kind of slow so we are busting it with design work.


I have a couple of dimensioning questions that need your help with.


1)   See picture below.  We need to know how this would be dimensioned on a drawing.  The shaft Runout is interpreted by us as rotating while the motor is fixed.  The shaft would be turning between the bearings fixed in the assembly.  The face runout would be that the shaft is fixed and then the motor is turned.  Same would be true for the Eccentricity.



2)   I have a tolerance analysis to do on the attached drawing to determine the stackup of the Circular Runout .  The customers spec is attached.  They wanted True Position, but our production line wanted something that would allow them to check it on the floor by using Runout.  The main concerns are shaft straightness and position of the Boss to the axis of the shaft.  Based on this would we get the same results and if so do I use Ĺ of the runout tolerance or not?  If not, can you help me understand how I do this analysis?

Thanks for your help.  We are still planning on trying to schedule you for a update training soon.  I have budgeted the money.






I hope you are doing well up there in that beautiful country.  I'll never forget my visit.  It was something to see.


Both Circular Runout and Total Runout are defined as a "surface to datum axis control".  If used on a diameter, circular Runout controls roundness and concentricity to the datum axis.  Total runout controls roundness, straightness, taper, and concentricity, if used on a cylindrical diameter.


Circular Runout controls balance of material on each side of the datum axis, if used on a planar (flat) surface.  Total Runout controls flatness and perpendicularity to the datum axis, if used on a planar (flat) surface.


In Figure 2 Verifying Motor Specifications, in what is called "shaft runout" if the motor isn't being centered on, and the motor's axis isn't being rotated about, the only thing it looks like you are measuring with that setup is roundness and (if you run the indicator down the diameter longitudinally) perpendicularity.  If you aren't rotating about a datum axis, you aren't measuring any type of runout.  You would have to be centered on another axis, to measure the runout of the shaft to that other axis.


In what is called "face runout", if you are centered on and rotating about the motor shaft, you can measure either Circular Runout of the face (which protects a balance of material on each side of the datum axis), or Total Runout (which protects flatness and perpendicularity of the face to the datum axis).


In what is called "motor shaft to pilot diameter eccentricity", that is actually measuring Circular Runout.  If the diameter on which the dial indicator takes its readings was longer and the indicator was moved down its length, then it would be measuring Total Runout.


Position, Concentricity, Circular Runout and Total Runout all allow you to be off center of the datum axis one-half of the amount that appears in the feature control frame.  So, if the geometric tolerance specification is .010, then any of the controls I listed would allow you to be off center a radius of .005.  Since indicators read how much you are off center in one direction as "plus" and 180 degrees from that it would read "minus", then if you were off center a radius of .005, your full indicator movement (FIM/TIR) would be plus .005 on one side and minus .005 on the other.  Your FIM would be .010, which is all it is allowed to be out for Runout controls.  And even though Position and Concentricity are measured differently than the Runout controls, they would not accept a part that was off center any more than a radius of .005 either.


If you need more information from me, I'll get back to you as soon as I can.


Hope this helps.





Subject: Re: GD&T questions about Combining Plus and Minus and Position Tolerancing


I took your advanced GD&T course last fall and I just had a couple of quick questions I was hoping you could clarify for me.  I attached a rough sketch to help convey the meaning of my questions:

1. (see attached Fig. 1) According to the 1982 standard is it allowed to have a regular dimension(.5+/-.1 in Fig 1) locating the edge of the part when a positional tolerance is used to locate the holes?  Can the dimension be non-basic as long as the hole to hole relationship is maintained or does the .5 dimension need to be basic?


2. (see attached Fig. 2) According to the 1982 standard is it allowed to use a compound axis as a reference in a profile tolerance?  Is it allowed to use the datum features being defined as a compound datum reference in the profile tolerance? (Only the dimensions locating the bottom surface of the channels are basic).


I hope the sketches are clear enough,

Kind Regards,






In Y14.5-1973, there was an example of what was called Combination Positional Tolerancing.  It allowed a combination of plus and minus tolerancing to locate the hole pattern and then position tolerancing was used to position the holes within the pattern to each other.  It was believed, at the time, to create rectangular tolerance zones for the hole axes from the "implied datum features" which were the edges of the part, and cylindrical tolerance zones from hole to hole (and for perpendicularity, since the primary datum feature was shown in the example and was for perpendicularity).


In Y14.5-1982, this example was moved to Appendix D Former Practices.  In other words, it was taken out of the standard in 1982 and replaced by Composite Positional Tolerancing as the acceptable method of accomplishing a larger position tolerance from the specified datum features and the planes or axes they generate and a tighter position tolerance from hole to hole.  Composite Positional tolerancing had been in the Y14.5-1973 version of Y14.5, but in the 1982 version, with the removal of Combination Tolerancing, it took on a more important role.


As far as Profile controls referencing a compound datum axis, it is most certainly legal and sometimes needed.  The example you show, profiling one side of the widths that create datum features C and D to datum axis A-B is okay.   I would think it is more common to reference A-B to locate the entire width of C and D.  The "or" example is even more unusual, wherein one side of the feature widths generating the centerplane of C-D are being Profiled to C-D.  Still, although not that common, it is perfectly legal.  You might also ask yourself if it is the best option though.


Hope this helps.



Close Window