Close Window

CLICK FOR ARCHIVES

The Tolerancing Engineer Newsletter - September 2013
...by our client company personnel and James D. Meadows using our ‘GD&T HOTLINE’

REGISTER NOW FOR
A UNIQUE PUBLIC WORKSHOP PAIRING…
both courses presented by GD&T ‘expert’ James D. Meadows

Geometric Dimensioning and Tolerancing [per the ASME Y14.5-2009 and 1994 Standards

...and the Differences between them] (2 ½ days) December 9-11, 2013 – in Huntsville, AL

and/or (take one or both courses)...

Tolerance Stack-Up Analysis [for Plus/Minus and Geometric Tolerancing]

(2 ½ days) December 11-13, 2013 - in Huntsville, AL

See details or call (586) 677-0555 to register and inquire about discounts.

 


Subject: Questions regarding Simultaneous Requirements and Position without Datum References

Jim,

Hope this email finds you doing well. Things are good here. Our company was recently bought by another. Big changes are coming, I’m sure.
We are continuing to create standards here to minimize confusion and we’ve bumped up against a question that we can’t agree on.

As you know, we have, in the past, relied on a consultant (not my choice) that is intent on “Profiling the world” (to quote you). It is one of the things he advocates that I just can’t agree with, although I find it difficult to find a strong argument against.

We do rely on profile heavily. It makes sense for much of what we do, but there are many times where position, perpendicularity etc. are equally viable and clearer, in my opinion.

The question comes in two parts:
First, does the simultaneity principle (making multiple features and patterns of features a simultaneous requirement-shifting only as a pattern, measured in the same set-up or with one gage) apply to profiled and positioned features if their datums and modifiers are the same?

Second, is there a requirement for datum(s) on a positional callout (ignoring the concentricity special case)?

The argument is that a position without a datum is simultaneous with all the profiles without datums (assuming there are no modifiers) and that the datum isn’t required for the profile.

Hope this makes sense.
Thanks for your time.

Scott

Scott,

It’s good to hear you are doing well. I’m also sliding along in greased grooves.

1. Simultaneity does apply equally to position and profile controls located from the same datums with the same modifiers.
To quote the current Y14.5-2009 standard section 4.19 page 76: “A simultaneous requirement applies to position and profile tolerances that are located by basic dimensions, related to common datum features referenced in the same order of precedence at the same boundary conditions.” In fact, in Figure 4-39 the title is Simultaneous Position and Profile tolerances. No simultaneous requirement exists if no datum references are used. In such a case, to attain a simultaneous requirement between position or profile of a surface controls, the local note SIM REQT may be used.



2. There is no requirement for datum references in a position control. There never has been such a requirement. If two holes within a pattern are located at a basic distance apart and their position tolerance references no datums, the two holes are positioned to each other. In fact, all position tolerances used on patterns of features (such as holes) position the features to each other before they position them to datums. The datum references are additional requirements, after the holes are positioned to each other within the pattern. What often happens is the two holes are positioned to each other, then they become datum features, from which all other features on the part are either positioned or profiled. I thought when Figure 7-59 was added to the 2009 Y14.5 standard showing two shafts positioned to each other without datum references, then showing the shafts becoming a pattern datum, which is then referenced in a position control by other diameters on the part, that people would stop saying position has to reference datums. But, it seems that since Figure 7-59 shows two coaxial diameters, someone at your place thinks this is only a special case for coaxial diameters. It isn’t. The two diameters could just as easily be side by side with a basic dimension other than the implied basic zero dimension separating them.



I hope this helps.
Jim Meadows
 



Subject:GD&T for Pipes, Hoses or Tubing

Hi James,

Could you please help me in interpretation of below symbol used for Position tolerances of Brake Pipes?

Thanks & Best Regards

Sukhdev

Sukhdev,


Whatever they are doing, it isn’t supported by the ASME Y14.5 standard on dimensioning and tolerancing. It kind of looks like they are calling out datum targets as datum features of size at Maximum Material Boundary. But, without looking at the drawing, I can’t be sure. We reference datum features in position controls, such as A, B and so on, but we don’t reference A1 or A2 or B1 in position controls. Someone has gone beyond what Y14.5 allows, but it may still be interpretable. It just could have been done in a more conventional manner. Also, I understand why we give X, Y and Z dimensions for the axis location of tubes. We’ve always done that. But, giving X, Y and Z separate tolerances that are all the samenumber is odd.


Why not just give it a position control with a diameter of 4 millimeters that confines the axis of the tube. If the tube is curved, this is done under the “BOUNDARY” method shown in Y14.5.Here is an illustration from one of my textbooks:

FIGURE 19-4 [Positional Boundary Concept Used on Hoses, Pipes and Tubes]


I hope this helps.


James Meadows
 



Subject: Bonus Tolerance vs. Datum Feature Shift

Hello Mr. Meadows,


I am looking at a tool drawing someone designed with the second hole referenced to the first hole with a datum modifier MMB and a 3rdhole referenced to the 2nd hole at MMB. My overall question is more over the concept of, “Is there a point to making a single hole have a Datum Shift Modifier instead of just providing the appropriate MMC alone to give bonus tolerance?” I can clearly see the necessity to use a Datum Modifier for a hole pattern in order to separate from what the individual hole tolerance is, but why for a single hole? I have attached a scan of a page from your book (1st and 2nd scanned pages). I understand the simplicity you used for the sake of explaining the concept, but otherwise, is there any practical reason to not set up the second hole to just have true position tolerance with extra bonus instead of a shift modifier?
 

Also, I have a question on the 3rd and 4th pages I scanned. So when there is a datum modifier, should I always consider the datum feature to shift with the type of tolerance in the original reference frame, like perpendicularity in the 3rdpage. I have seen some explanations from others that made it seem as if you took your example, it would be looked at like a positional shift (no matter if it originally referenced something like perpendicularity).

Best Regards,

Joey

The pages Joey scanned from one of my books:

A Difference between Bonus Tolerance (Growth) and Datum Feature Shift (Movement) of Tolerance Zones

One of the most often asked questions in measurement and also in tolerancing is, “Can we take tolerance from the datum feature referenced at MMB and give it as tolerance zone growth to the features being measured from that datum?” The simple answer to that question is, “No!”


Granted, there are some isolated cases where this strategy might work out, but many more cases where it will not. Certainly, for a pattern of holes referenced to a datum regular feature of size (such as one hole), as the datum regular feature of size departs from its virtual condition (Maximum Material Boundary concept), that pattern of holes may shift as a group an additional amount. This apparent shift of the pattern of holes is actually a movement of the datum feature axis away from its imaginary datum axis. But it will appear as though the entire pattern of holes has shifted/moved. This concept is thoroughly explained in other sections of this book.


In this section, let’s explore a situation that is very simple: one hole positioned to two datums. The planar primary datum will serve the purpose of perpendicularity control, while the secondary datum feature will be a hole which generates an axis that will be used to hold a 500 millimeter distance. So, datum A will be for perpendicularity and B will be for location in the following illustration.


FIGURE 5-29 [Part Drawing]

In the simple example depicted below, the following illustrations show correct distributions of the tolerances that would allow parts to pass the gage.
FIGURE 5-33 [Tolerance Zones]



Shifting vs. Growing Tolerance zones

FIGURE 7-20 [Shifting vs. Growing Tolerance Zones]

Many people feel the above two callouts (FIGURE 7-20, Examples 1 and 2) result in essentially the same geometric control. In reality, they are quite different. In Example 1, the shaft axis is controlled for perpendicularity within a diameter of 0.1 at MMC to datum A. As the shaft departs from MMC (is made smaller, but still within size limits), the tolerance zone will grow to permit a maximum out-of-perpendicularity of the axis to datum plane A of a diameter of 0.3 at LMC. Datum feature A has not, in this case, been controlled for flatness. Datum plane A is taken from the high points of the datum feature.


FIGURE 7-21 [Tolerance Zone for Example 1 in Figure 7-20]

In Example 2, the controlled feature is the bottom surface of the part. That surface must be within two parallel planes 0.1 apart. These imaginary planes are perfectly perpendicular to datum axis A when datum feature A is produced at its MMC of Ø15.2 (which is also its Maximum Material Boundary). All elements of the controlled feature (bottom surface of the part) must lie between these two parallel planes. This controlled feature is not only controlled for perpendicularity but also for flatness to within 0.1. Since the surface being controlled by perpendicularity is not a feature of size, it is not allowed to be modified with the MMC symbol. Consequently, the 0.1 tolerance zone cannot grow under any circumstances. The flatness of the surface is controlled to within 0.1.

However, the datum feature is modified with the Maximum Material Boundary (MMB) concept using the . This means that as the datum feature departs from its MMB (is made smaller than 15.2, but still within size limits), a shift of the tolerance zone controlling the bottom of the part may appear to occur. The two parallel planes 0.1 apart, within which all elements of the actual surface must reside, may appear to shift (tilt) as a unit an amount equal to the datum feature's departure from MMB. In actual fact, the datum feature axis may tilt away from the imaginary datum axis by the diameter’s departure from 15.2. This has the effect of increasing the allowed out-of-perpendicularity; but at the same time, the flatness of the controlled feature is held to within 0.1 (unlike Example 1). For a visual depiction of this phenomenon, see FIGURE 7-22.

FIGURE 7-22 [Tolerance Zone for Example 2 in Figure 7-20]

Joey,


When you have one hole positioned to another, it is like saying that they work together, for example, they mate with the same part. If they mate with the same mating part, the MMB modifier used with the MMC modifier in the same control, is a way of saying that if either hole deviates from its virtual condition, the holes may deviate more from being perfectly positioned to each other. The larger the hole (without being more out of perpendicularity to a planar primary datum), the more each hole may move away from the basic dimension that connects them. Picture a gage with two virtual condition sized gage pins on a plate, one for the datum feature referenced at MMB and the other for the hole being positioned. As each hole grows (without being made more out of perpendicularity to the primary planar datum), that hole may move more before it hits the gage pin. Or, as each hole grows, it may be more out of perpendicularity to the primary planar datum. Or, a little bit of both, but no more than the gage pins would allow.


The gage described above would be different if the datum feature of size (hole) wasn’t referenced at MMB, but rather implied at RMB. In that instance, the gage pin simulating the datum feature would have to expand into the hole, locking it up, and allowing no shift.


As far as your other question, that the perpendicularity control shown on the third and fourth pages you scanned would somehow create a shift that would equate to a position shift, no, that’s wrong. There is quite a bit of difference between angle and location. Position controls both angle and location, but perpendicularity controls only angle. So, the shift on a perpendicularity control that references a datum feature at MMB would only allow an angular shift zone, since the relationship being controlled is only one of angle (not distance).


I hope this helps.


James Meadows


Thanks James,


That does help. I am still a little confused on the second concept I brought up and you explained, but this figure I attached actually illustrates my problem better than what I tried to use. For the hole on the right, does the datum modifier of -B- at MMB represent added positional shift (being in the original Datum Reference Frame) of the feature datum or perpendicularity shift (since that is what -B- has as a tolerance type) of the feature datum?


Best Regards,


Joey



Joey,


That one is positional shift. The relationship between the second hole being positioned and the first hole (which is what the second hole is being positioned to) is one of location. So, as the first hole (datum feature B) grows from 49 toward 50, the second hole may shift away from the datum axis of B by the growth of B. Any out of perpendicularity of datum feature B negates the shift it allows as it grows.


The theory, as explained in Y14.5, is a little different than I explained it here, and a lot more like I explained it the first time with gages. The theory is that as datum feature B grows, its axis may shift away from the imaginary datum axis B. This is pretty easy to visualize, if you picture the gage I described with two pins on a plate. The first pin axis simulates datum axis B. If the hole B is larger than the gage pin (virtual condition), the hole B axis may shift away from its own gage pin axis. So, to someone holding the part in their hands, it will appear as if the second hole has shifted away from its perfect location from the first hole. But, the theory is that it is the first hole that has shifted. And because of this shift, the first hole’s axis (datum feature axis B) will not be coaxial with its gage pin axis (which simulates the imaginary datum axis B). The axis of hole B (datum feature B) has shifted away from the imaginary datum axis B (simulated by the axis of the gage pin).


James

 



Subject: Runout and Free State
 

Hey Jim,


I hope you are doing well. I have taken a couple or your classes in Huntsville, AL, and I would like to get your input on a of couple questions, please.


These questions are relative to ASME Y14.5M-1994.


As I understand it (6.7.1.1.1, p 189), Runout requires establishing an axis by chucking/touching the stated datum reference feature(s) and actually rotating the part to measure the FIM of an indicator (dial, ldvt,…). Figure 6-17 (p 169) seems straight forward with respect to free state, however, Figure 6-49 leaves me with some questions.


1) Is the Runout of Figure 6-49 (p 191) considered to be a free state measurement?


2) Assuming a lathe is used and is chucked on the datum reference surfaces of Figure 6-49, can Runout be measured while still in the lathe and be a valid Quality inspection, and would there be a note required (or is it already understood) on the drawing to “allow” the Runout to be measured while still in the lathe?


3) Considering the text implies the part is to be rotated about the simulated axis and the indicator to be in constant contact with the surface, for Figure 6-49, are the discrete points of a coordinate measurement machine a valid means of checking Runout if the part is not rotated?

Thank you for your time,


Dwight




Dwight,


1. Yes, the runout controls in Figure 6-49 are free state measurements. All measurements are free state unless a note is written to specify they are to be restrained while measured. Free state measurements are considered those wherein the measurement equipment (chucks, probes, etc.) do not distort the part to obtain compliance. In the gaging and fixturing standard (Y14.43, a committee I chair) we say, you will use zero measurement force. Still, we all understand zero measurement force is unattainable. But the goal is understood to be: not distorting the part or the equipment to an amount that significantly changes what the part would measure in an absolutely free state.


2. Yes, you can measure it on the same machine on which you manufacture the part. It isn’t considered a great measurement approach, since we try to measure parts on machines that are more accurate than those we manufacture them with. But, there is no rule against it. All measurement is flawed in some way. It is up to the company in charge of the project to decide how much measurement error is acceptable. A measurement plan may be written that states the part is to be measured on the lathe, but that isn’t necessary. It just might save some arguments from occurring later on.


3. Y14.5 isn’t a measurement standard. Y14 standards are documentation standards. B89 standards are measurement standards. For example: B89.3 standards deal with Measurement of Geometry. What you are trying to verify with circular runout on features such as are shown in Figure 6-49 is that the surface is round and coaxial. Circular runout generates a tolerance zone in these instances that is (an infinite number of) two concentric circles that are the geometric tolerance apart radially and centered on the datum axis. Any way you can estimate that the surface is in compliance with this, including using the CMM to do it, is valid, provided all possible effort is taken to properly establish the datum axis and enough surface points are collected (and enough circular cross-sections are measured) to reach a confidence level sufficient to satisfy the customer.

I hope this helps.


Jim

 



Subject: GD&T Dilemma


Jim,


I would like your opinion on an issue I can finally share. One of our design groups is trying to designate a pattern of rectangular contacts a pattern datum. They are finding one pin center, finding the relationship of that pin to all the others, taking some kind of average location giving them the “centroid”. They want the “centroid” of this pattern to be a datum from which other types of contacts will be located…INCLUDING THESE! If these contacts were cylindrical in design I would not have an issue with it in a different configuration (4 select locations), and I understand why they want to do it, but... They are working with a highly advanced vision system which, in effect, builds a new gage for every part checked by positioning a cylindrical zone on a basic dimension grid originating from this “centroid” (the features are positioned at RFS). The only pattern datums I have ever dealt with are a pattern of cylindrical features.


Is there a legitimate way to do this on the print? I have attached a basic drawing of the connector.


A bit more background…


• The customer does NOT trust gaging and has invested in this vision system…
• We have an internal spec which allows us to create a cylindrical tolerance zone for a rectangular contact feature based on the printed circuit board opening, but this does not necessarily allow us to consider the rectangular feature to be a cylindrical datum…
• It would appear that between ASME, ISO combinations and the customer demanding what they do not understand, it is very hard to maintain the specifications set forth. The customer wins…until there is an issue and we cannot prove we know what we made was acceptable based on an inability to interpret.


Any input you may have would be greatly appreciated.


Rick


Rick’s Illustration:

 

Rick,


First off, rectangular feature can’t have cylindrical tolerance zones. Y14.5 states:


7.4.5 Noncircular Features of Size


The fundamental principles of true position dimensioning and positional tolerancing for circular features of size, such as holes and bosses, apply also to noncircular features of size, such as open-end slots, tabs, and elongated holes. For such features of size, a positional tolerance is used to locate the center plane established by parallel surfaces of the feature of size. The tolerance value represents a distance between two parallel planes. The diameter symbol is omitted from the feature control frame. See Figs. 7-30 and 7-31.


The only mention of a square feature as a datum feature is in figure 4-46 shown below:

Normally, when a rectangular feature is used as a datum feature, we use two sides as the secondary (width) and two sides as the tertiary (width). Each generates one plane, the secondary and tertiary center planes.


As it affects your situation, although the use of the diameter sign in the feature control frame for the 20 rectangular features is incorrect (wrong), they can use the 20 rectangular pins as a datum feature pattern. It could also be said that the 20 widths in both directions could create a centroid center plane for X and Y measurements to use an the origin of measurement for the 16 pins. For example, if a circled M had been used after the 0.2 for the 20 rectangular pins and subsequently, a circled M used after the datum feature pattern reference B (in the position control for the 16 pins), a functional gage could be constructed consisting of 36 holes (20 made to the virtual condition of B and 16 made to the virtual condition of the 16 round pins).
 

The problem comes into play when they have to construct a centroid for the 20 rectangular pins as produced regardless of material boundary (RMB as it is called in Y14.5-2009). Y14.43 (the gaging and fixturing standard) states that in situations like that, the gage holes would have to contract at the same rate until the part is immobilized by the gage holes contacting the pins. The question is, how is the vision machine constructing the center planes of datum feature pattern B?


This not only seems extremely difficult to measure and hard to understand as a tolerancing scheme, but unnecessary, as there are other datum schemes that would give the same results, but be infinitely easier to measure and comprehend. In fact, in the Y14.5 and Y14.5.1 (Math) committees, they are currently trying to find consensus as to what it even means when a group of cylindrical holes or shafts are referenced as datum patterns RMB. There are at least four competing theories of how to construct the centroid, and those are round features. Yours are even more difficult, in that they are rectangular.
 

If they insist on this path, good luck getting anyone to agree on what is the proper method for constructing the center planes from datum pattern B.


Jim Meadows
 



Subject: Profile with a Refinement of Flatness


Jim,


Can flatness be used as a refinement of profile?


Hubert


Hubert


Yes, provided it is used to refine the flatness to within a smaller tolerance, where the profile control is doing more than just flatness within a larger tolerance. For example; if profile of a surface is used to make multiple planar surfaces coplanar (existing in the same plane), then each surface may use a refinement of flatness. This will have the effect of making the surfaces individually more flat than they are coplanar to each other.


Jim

 

Close Window

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

Site Designed & Maintained by VIRTUAL GOLDMINE