Refinement to positional tolerance

[prdave00]

I have a differing of opinions on a tolerance scheme best described in the attached file. Basically it is over some nuances regarding what a colleague calls a "composite" feature control frame (I think incorrectly), and what I would simply call 2 single segment control frames.

The part has a post that I want to control location and orientation in general, and then refine the location & orientation in one direction.

We are using ASTM Y14.5M-1994, but I'm curious if it breaks any rules of the 2009 version.

 

[Belanger]

First a couple of minor things -- The note should say "ASME Y14.5M-1994."
And your intent says position of .010 at MMC, but the feature control frame shows .10. I'm sure that's just a typo, but better to catch it now...

Neither sketch is what we would call a "composite" feature control frame. For composite, one position symbol would be shown, centered. And any datum references on the bottom part of a composite callout would have to be repeating a datum referenced in the upper part, and in the same order of precedence.

I suppose it's OK to say "compound" position tolerance when verbally discussing GD&T; I don't think that term is used in the standard but it gets the idea across that there's more than one position tolerance invoked. (Both the 1994 and 2009 standards would refer to all this as "single-segment" feature control frames.)

Your colleague's explanation #1 isn't strictly true. It sure makes sense to have the MMC modifier but it's not required (FYI -- in the 2009 standard that would be called the MMB modifier). It's the function of the part that dictates "M" or no "M" ... not the gauging.

Explanation #2 isn't really true. Since it is two single-segment position tolerances, you can do whatever you want regarding the datum references. It's not common to have a tertiary datum suddenly become primary, but it's legal.

And explanation #3 is not true at all. Without a diameter symbol in front of the number, a position tolerance reverts back to being two parallel planes. There are times when that's needed. However, I think that the position tolerance of .05 should be in the right-hand view, so that it is clear what direction those parallel planes lie in. Datum C sort of conveys the idea, but it's best to show it in the view where the position actually operates, unless it's multidirectional.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[dingy2]

I will probably be saying that same thing as JP but here goes anyways.

1 - Wrong - MMMC may or may not be used on feature of size. It depends upon the situation.

2 - Compound Feature Control Frame?? What is that? I think that you mean single segments feature control frames.

3 - A diametrical tolerance zone only applies to feature of size that are round except when bi-direction tolerances are applied. One can also delete the diametrical tolerance zone on round feature of size and it will mean that tolerance is applied along the X and also the Y axis. We would end up with a square tolerance zone similar to co-ordinate tolerancing.

Dave D.

http://www.qmsi.ca

 

[drawoh]

prdave00,

On both drawings, I do not understand your datums A and B. I think they do the same thing. Perhaps Datum_A should be the long bottom face, and datum_B the Ø.25" hole!

The upper toleranceing scheme makes sense to me, as long as you want your feature located accurately to the Ø.25" hole and located less accurately to the width.

On the bottom tolerancing scheme, the first tolerance block requires a Ø.01" position with respect to datum_C, rendering the second block redundant.

On the upper tolerancing scheme, I agree with Belanger that the diameter symbols are not appropriate.

JHG

 

[prdave00]

JP: Thanks for the quick response. It looks like I wasn't firing on all cylinders when I wrote my OP. I did mean ASME not ASTM for the standard designation. Also this part is a simplification that I put together of a much smaller molded part with additional features which is reason why .010" slipped out for the actual part instead of .10" as in my example. Regarding the material material boundary (borrowing terminology from 2009) and my reference to hard gauging, I've heard from suppliers that the boundary condition doesn't come into play when inspecting parts on a CMM for example unlike the material conditions in order to apply bonus tolerances. Is that accurate? I guess I've only heard MMB coming into play when designing a gauge and I need to unlearn that. Regarding your comment on explanation 2, I've just never see it the way my colleague wants it and wasn't able to find any examples in the usual sources (Y14.5M-1994, Y14.5-2009, Tec-Ease website). How do you interpret his tolerancing versus mine?

Here's the tolerance zone I envisioned where the parallel lines would be parallel to the plane simulated by Datum C with a width of .05" and the diameter of the "(" & ")" entities would be .
___
(___)

drawoh: I think you have it backwards or I'm not understand your point. In both schemes the first tolerance block has a looser tolerance (.10") than in the second tolerance (.05") where I intended to refine the positional tolerance. Regarding the order of precedence, in use the part is slid over a post until the bottom surface (datum "B") makes contact and at that point the datum "C" centers the part between 2 posts. My order of precedence reflects that. Does my order still not make sense?

 

[Belanger]

Yes, I agree with your representation of the tolerance zone -- it is a diameter that is sort of chopped off on the sides because of the tighter tolerance formed by the two parallel planes.

The MMB modifier is essentially saying that in the function of the part, there may be some looseness or slop around the datum feature, and not only can we live with that, but we'll use that slop to make the feature being positioned appear to have more location tolerance. Notice how I'm phrasing it in terms of the function. Part are designed to function, right? Not to be gaged. (Gaging is a secondary process which must be performed but it is usually not the "driver" of the design process!)

So when you mention suppliers who say that "the boundary condition doesn't come into play when inspecting parts on a CMM for example unlike the material conditions in order to apply bonus tolerances," I can't say they're wrong. But that statement about the CMM process not a cause; it's an effect. If you deem that the function of the part will allow a little bit of slop on the datum feature, then their CMM program should be able to mathematically factor that in! Otherwise they are going to be checking parts with an "RFS" mentality -- which means exact mathematical center, not a boundary condition -- and perhaps rejecting parts that will function just fine.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[prdave00]

JP,

Thanks for the reply. I definitely need to unlearn my (mis)conceptions about material boundaries.

You had mentioned "since it is two single-segment position tolerances, you can do whatever you want regarding the datum references. It's not common to have a tertiary datum suddenly become primary, but it's legal", but I'm still unclear whether the way I specified the tolerance (bottom sketch) or the way my colleague suggested it (upper sketch) says 2 different things if my intent is to have the axis lie within the tolerance zone at MMC that I sketched. Do you think an inspection house would interpret ours the same way? I've attached a new file so we have the same boundary modifiers.

Thanks,
Dave

 

[Belanger]

To see if there is any difference, try to imagine the gaging. (I'll describe a physical gage setup just because it's easier to visualize; CMMs do the same but with mathematical simulation.)

For your colleague's sketch, the upper frame would require: a fixed-size gage pin of .15 inserted into hole A. Then stabilize the part by holding a flat plate against surface B. Now we have to measure the position of the pin's axis with respect to those degrees of freedom that A and B have constrained. (I might have put B ahead of A, but that's a different discussion!)

Now, the upper frame in your sketch is almost the same but you also have the tertiary datum C. (It sounds like you want C to constrain the last degree of freedom, which is the rotation around the gage pin's axis.) This is simulated in physical gaging by first contacting A and B as done for your colleague's sketch, but then having the part slide in between two plates spaced exactly 1.10 apart.

But basically, there would be no difference in the end result, because you are going to have the position to datum C be "trumped" by your lower frame. Thus, having C as a tertiary datum in the upper frame is not wrong, but it doesn't really add any value. The only value would be if there are other feature control frames on the drawing that reference A(M) B C(M) -- then I would leave C in order to imply simultaneous gaging.


John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[prdave00]

JP:

Thanks for addressing my question. I think your explanation including "simultaneous gaging" helped a lot. I do find it interesting that you say the datums in the lower frame trump the upper. I was under the impression that the lower frame only refines the tolerance zone but does not further constrain any degrees of freedom. Could the upper frame if it were |A|B| stand on its own if there was no lower frame?

As far as the the order and selection of datum features, I think I'm falling into agreement with you and Drawoh. In the actual smaller part (that I based this simplified model), the thru hole (Datum "A") is an hour glass shaped revolved cut and not cylindrical. In use, the part is slid over a pin and then moved down until it contacts the surface represented by "B". Then another part engages with the extruded boss and the surfaces that comprise datum "C" help to orient that added part. I based my datum selection and precedence on how the product is used, and not necessarily how best to constrain the part. Does that make sense?

 

[Belanger]

The lower frame only trumps the upper frame in that it holds the feature to a tighter tolerance in the direction of that datum (in this case C). It doesn't really constrain different degrees of freedom, but just refines how accurate the feature is relative to that degree(s) of freedom.

Your datum sequence makes sense. The only reason I was thinking twice has to do with the MMB modifier on A. If there is any looseness around datum A, which is permissible by MMB, then datum B will stabilize the part flush on that bottom surface (3 points of contact), sort of making B the main datum. But it's not wrong, and the new standard actually shows this practice in Fig. 4-21(d). It means that if datum feature A is at .15, then surface B may only make contact at one point. So I guess you can leave it as is...

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[MechNorth]

I mostly agree with the postings, but here's a couple things I noticed;

Datum A removes 4 d.o.f. [x,y,u,v]; Datum B takes away 1 d.o.f. [z]; which leaves 1 d.o.f., the rotation about Z [w]. If Datum C isn't referenced in the top fcf, then there is no rotational constraint on the inspection setup, and you can be at a substantial angle to the inclined mating face (i.e. rotated about Datum-A) which would produce a significantly different part though acceptable to the tolerance.

Material modifers on the two datum fos's (A and C) are subject to the functionality of the part; if those datum features are going to mate to something with permissible slop/mismatch, then MMB modifers on the datum references make sense. On the flip side, if those datum features are going to mate intimately then RMB is more appropriate.

It's true that many inspectors don't consider MMB or LMB when they're CMM inspecting ... but they should. As I recall pretty much any software under 10 years old at this point should be able to handle MMB or LMB datum modifiers without a hiccup ... as long as it's not on a surface profile control. The value of using MMB or LMB is still there regardless of whether or not a CMM is used as it provides a better means to fit the part features.

"Compound" was commonly used in the bad old days by instructors and laymen who didn't know the standard particularly well, and it still percolates through the system. "Composite", "Single Segment" and "Multiple Single Segment" are the terms used correctly. Calling a multiple single segment fcf a "compound" fcf may lead to misunderstanding it as a composite control.

As for the shape of the tolerance zone in the second single-segment fcf, it makes sense for the functionality you seek; a cylindrical tolerance zone would not add anything beneficial.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[prdave00]

Jim,

I get how it uses probed points to determine a feature's size in order to determine and apply a bonus tolerance, but I still can't get my head around how a CMM factors in the material boundary of the datums. Like I said in one of my easier postings, I've always associated applying material boundaries in the design of functional (attribute?) gauging. Maybe the disconnect for me is that a gauge is tangible counterpart to the part to be inspected while construing surfaces based off of a cluster/pattern of points is on the abstract side of things. Would you be able to humor me with an example of how a CMM algorithm applies MMB, LMB, etc.?

 

[MechNorth]

I don't know the specifics of the math, but in essence the CMM is able to mathematically "float" the point cloud to establish that it is within the limits established by the datum displacement (datum shift). I met a fellow about a decade-plus ago that did some of the very early related work at one of the big-3 automotives; the company wasn't interested so he spun a derivative functionality off into a lucrative business which has made him some coin. Sorry I can't be more helpful than that, but the math isn't my forte.

For comparison, do some visualization exercises based on the design you submitted. If you engaged the workpiece with a hard gauge, you could shift the workpiece or the gauge around within the limits established by the allowable datum shift. It's usually a fairly small shift, but it can be substantial if the tolerances so permit. As you move the piece or gauge wrt the other, if you achieve a mating condition wherein all constraints are satisfied, the part is good. Fortunately the human brain is still the most versatile computer we have, so spatial reasoning is a doable for most engineers. For the CMM, it's all processing power and algorithms. I would suspect that the algorithm tries to float the first modified datum while achieving the best fit of the workpiece within the tolerance zone, then progressing from there ... which is essentially what we do cognitively in hard-gauging.



Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dtmbiz]

I have encountered a similar case for a weld stud location tolerance composite FCF at our facility also.

There is a composite callout with the upper segment having a diametrical tolerance zone of 0.72 mm and a refining perpendiclarity to datum A of diameter 0.36 mm tolerance zone.

The "issue" is that there is "only one weld stud" and the argument is that the composite or multi segment callout (1994 std) refers to the top segment as the "PLZTF" and thus the argument as in the drawing example here and in my case..."one feature". The PLTZF is for a "pattern". The argument is that "one feature" is NOT a pattern.

I changed the callout for a location tolerance FCF and used a refinement of perpendicularity FCF under.

Comments regarding "Pattern Locating Tolerance Zone Framework"?

I also have a question regarding finding the "center of a pattern of holes" on the actual produced part; for setup on
CMM. Can show specific concerns on a sketch to clarify my question if neccessary. This thread or a new thread?

 

[MechNorth]

dtmbiz

new thread

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dtmbiz]

Thanks for response Jim.

Any comment on the "pattern" question? Would like your point of view.

New thread, good enough... tomorrow... gone for today.

 

[axym]

dtmbiz,

Specifying a composite position tolerance for a single feature isn't a good idea, but not because of the word "pattern" in PLTZF. This acronym is just a general guideline, it doesn't really define anything. The issue is more that a composite position tolerance doesn't add any value when applied to a single feature, and will likely just make things confusing.

The only thing that distinguishes a composite FCF from two single segment FCF's is that the lower segment of the composite FCF controls orientation only. This allows you to refine the orientation of patterns (orientation tolerances can only be applied to individual features). But if you only have a single feature, you might as well just use an orientation tolerance (in this case, perpendicularity). So changing it to a position tolerance and a refining perpendicularity tolerance was a good call.

Finding the "center" of a pattern of holes using a CMM is a whole other can of worms. A new thread would be best for that.

BTW, Jim nailed the description of CMM datum shift pretty well, considering he's a design guy ;^)

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[MechNorth]

Tks Evan. I tries but I sometimes fails. Yes, us design guys DO make mistakes...I'm still waiting for my "one" for this lifetime. =~}

One item from Evan's post; second and subsequent levels of a composite positional FCF refine inter-feature location as well as orientation to the datums referenced. So, if you used a composite control on a single feature, then you'd get orientation alone from the second level. Unfortunately too few people understand that position includes orientation and therefore can (technically) be used to control orientation. I've seen it on many prints, and while it is "technically" correct, it's not user-friendly and will not be understood ... hence ignored by most.
Two single-segment FCFs (both positional or one positional & refined with perpendicularity {option #2 is easiest for most people to understand}) is appropriate for what you seek.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[Belanger]

Jim -- I'm wondering about the last sentence of your most recent post. You say that option #2 is easiest to understand, but I would say that it's the only option, since we're dealing with only one feature. ( We cannot use the position symbol to control perpendicularity if the only quality being controlled is orientation.)

I'm not trying to nitpick -- and I know my statements here are in disagreement with a Tec-Ease tip -- but this is something that I've seen quite frequently. Granted, it's a minor topic, but I cordially suggest that paragraph 7.2 of the standard means that the position symbol must by its very nature always have an element of "location" involved.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

 

[MechNorth]

Hi JP, you're not nitpicking at all. Most people don't like & wouldn't advocate the use of a positional control as an orientation control alone; some don't believe it's legal within the definitions of the standard. The larger problem is that it's not illegal within the definitions of the standard, and therefore some people choose to do it.
If you want to take 7.2 (2009) at face value alone, then position wouldn't control orientation at all because it doesn't mention it. But, as the orientation of the feature's axis or center plane is constrained within the positional tolerance it is indirectly controlling the orientation as well, even on a single fcf. It's this "hierarchy" as Tec-Ease calls it which tells you that for some applied control you get some other lower-order controls for free.
I haven't studied the '09 standard as I have the '94, but I haven't found anything that precludes position's use in this way. Unfortunately that arguably makes it "valid" by extension of principles and thus technically legal. It doesn't mean that I like it or would ever advocate the use of it, but it is, strictly speaking, legal unless it violates some other aspect of the standard. I have had a number of my students ask me about using it and I carefully tell them that it is technically legal, but really bad practice. It is not widely understood to be used in that way, and therefore introduces interpretation error into their system ... with no upside.



Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com