Position callout used to refine profile, position callout is redundant or is flat wrong 1

[greenimi]

Engineering released this drawing and I would like to fully understand what they would like to achieve with this part--see attachment:
The questions I have are:

1.) Top view we have 2 surface profiles .005 with A and B. I guess, having these 2 profiles the surfaces are now located WRT (with respect to datum A and B). Now, on the bottom view/section view we have a position of the 1.000 (feature of size) WRT datum A. I guess what they are concerned here is the middle plane. So, the question:
Is this feature already located ? (by the two profile callouts)
Or are they trying to refine this ? If that's true what would be the minimum position value for which this position callout would be valid (above certain value it's already achieved). Or maybe it's not refinement (refinement was just my assumption). They want the cut for these planes to be symetrical to the center of the cylinder - datum feature A.
Now, they added MMC at the position (I guess to relax the requirements, bonus tolerance) , but if that's true I don't see any relaxation--because the profile is the one to dictate.
What am I missing?

2.) Slot Position: Top view they have a position control of .005 at MMC with A at MMC/MMB (we are using Y14.5-1994 so would be MMC). Under that, they have a perpendicularity callout of .005 with B.
I am wondering (just from theoretical point of view) if we remove the perpendicularity and add datum B as a secondary datum on the position control would the effects be the same?
If no, what would be the difference?
I am thinking this, since position control also perpendicularity (orientation). Can we get the perpendicularity of the slot to datum B by having B as a secondary on the position callout?

The "proposed" positional requirements would be position of .005 WRT A at MMC and B – in red --

3.) Related with #1: 1.000 dimension (bottom view / section view) shouldn't be basic? Or, even better, reference since the profile is giving the size also.

4.) Related also with #2, the profile callout for the circular slot (section on the right view) does not have datum B (as a secondary datum). Wouldn't make for sense to have it there, since the part is assembled in one way--sitting in one position in the assembly-- and the profile callout to have the same datum reference frame as the two profile callout in the top view.
How this part can function in the assembly in a such of way that datum B is needed on the top view and is not needed in the right view?


5.) Realistically, if they measure this part on the CMM, do you think they would change the setup (coordinate system) for the profile without datum B as a secondary datum? Or they will use the coordinate system already in place when the two above surfaces were qualified.

Thank you so much

 

[fsincox]

greenimi,
1)I think, for a refinement, it should be less than .005 particularly since it references datum “A” at MMC and the profiles do not, I could see this more if it was the other way around and the number was less than .005.
2)I agree with you that the unified position is most likely a better solution but we do not know the function, here, so it is just assumption. The difference will be easier to describe as one is a single installation check, while the other requires separate checks, although it must meet both.
3)Yes, the bottom dimension should be reference or basic.
4)We might assume it should be there, without function we don’t know.
5)What someone might do is only an exercise in speculation.

 

[pmarc]

greenimi,
Allow me first to say that every time I see so many different datum reference frames on such relatively simple part (4 DRF's in this case: A; A(M); B; A|B) I automatically become suspicious if product engineer really knows what he is doing. It is really hard to imagine that part's function really requires such amount of DRF's. I am especially curious what is the reason behind having A modified by MMB/MMC in some callouts and referenced at RMB/RMC in the others.

And trying to answer to your questions:
1. As you noticed, there is a logic behind such profile & position combination, though IMO there are much easier, clearer and more standardized methods to accomplish the goal (like for example position callout as it is on the bottom view plus flatness tolerances on both side faces of the feature if size tolerance is not enough). As for refinement, current position callout cannot be considered as such due to one simple reason - datum reference in positional FCF is not a repeat of any of datum references applied in profile callouts (which by the way are located incorrectly). Out of curiosity, what is the size tolerance on 1.000 width controlled by positional callout?

2. As Frank mentioned.

3. See #1.

4. Probably it would make sense to have it there, especially that location of the slot in depth-wise direction is not controlled, but would also require additional basic dimension from the center of hole B to the center of circular slot. (What is basic .100 dim. on left view doing there? - seems to be meaningless at the moment). And like I already said, those different DRF's...

5. In theory, if the datum reference frames are selected correctly, CMM operator is obliged to change the setups even hundred times if needed. In reality different tricks are done to avoid re-installation. You would be really surprised how different and unfortunately how careless.

 

[greenimi]

Pmarc,

I agree with you that the DRF’s in this case could be consolidated (at least in part consolidated)
I was told that the reason for the A being modified at MMB/MMC in some callouts is to take advantage of the datum shift available. If this datum shift can be measured or not (without a functional gage) that’s another story, but the product engineer wants to be in line with the objectives of GD&T, to allow as many functional parts as possible.
The profile does not have MMB/MMC datum shift available as the stackup tolerance at assembly level does not allow this.

And to answer your questions: tolerance for 1.000 is ±.005.

This part has a shaft going thru Ø.253/.247 –datum feature A- hole which is doing the job of orienting the part in the assembly, another hole –datum feature B- a sensor going into that hole is removing all the remaining degrees of freedom. Then the part is “sanwiched” between 2 other blocks, and those blocks have a critical job of sealling the entire assembly.
As the part rotates around datum feature A, the sensors indicate the location of these additional blocks (angle of rotation is important) and also how far from the sealing surfaces these blocks are and the fluid/air flow that passes thru.


I have some follow questions if you don’t mind:

1.) What do you mean by saying “the profile callouts are located incorrectly”. What could be changed to be “legal” and how?

2.) Please confirm to me, if you agree or not that as is drawn now, positional requirement is redundant. A positional requirement would make sense if the tolerance value would be .005 or less. Do you agree with the above statement?

3.) If the slot .252/.248 positional callout would be .005 with A and B ( RFS / RFB) would this revised callout take care of the perpendicularity to datum B? Or do we have to still use a separate perpendicularity callout?

4.) I have replaced .100 to .600 basic (from datum B). Would this new basic dimension make more sense?


Thank you again

 

[SeasonLee]

I am trying to reply your 1st question only:
A leader line of profile control frame should be directed to the feature surface, you can’t just put it under the basic dimension .500, the basic dim defined the the true profile of the surface, so the tolerance zone is on the surface.

SeasonLee

 

[fsincox]

1) I am not clear on that statement either

2) My quick analysis says the most the centerplane CAN be off now with the profile callouts IS .005 RFS so the position statement is not a refinement of anything it is added gibberish, that is the problem. If the number was smaller it could be argued it is a refinement that for some design reason was needed (basically, a tighter symmetry to the hole (datum A).

3) I doubt it would add any value; it is not the same thing but is it needed for the function?

4) There is nothing that locates the outside stuff, in two of the three directions, to the inside stuff.

 

[fsincox]

OH, Thank you Season, I see now why pmarc had an objection and agree, I just missed it.

 

[pmarc]

greenimi,
1. SeasonLee got my comment right.
2. Yes, positional tolerance value is redundant - at least I do not see any value added.
3. Yes, it would control perpendicularity to datum axis B. And as a matter of fact I would recommend it, since this would help in reducing the amount of different DRF's and in consequence the number of different inspection installations for this part. I am pretty sure that DRF containing both datum references also reflects part's functionality better.
4. Basic .600 dimension itself is not enough - you also have to add B reference to profile callout, otherwise the dimension will be meaningless. I might be missing something, but cannot see a basic radius of the slot. And just for clarity, I would recommend moving basic .550 dim. from main view to the section A-A view where other details of the slot are shown.

What is also missing is the relationship of part's length (currently only described by 2.000 dim.) to datum reference frame. I think the most logical approach would be to use the same method as is used for part's width - profile of surface applied to both ends plus 2 basic dimensions from datum axis B to that faces. Something similar should be done for height of the part (currently completely undefined) with the basic dimensions originating at datum axis A.

 

[greenimi]

Thank you pmarc,
I appreciate your help and you level of expertise.
If we change the length's and height's part definition (by adding four profile callouts, one for each of these surfaces, as you described above), wouldn't all of these six profile callouts (two existing + four new ones) be equivalent (has the same meaning and produce similar results) with only one ALL OVER profile, WRT A and B, applied for the entire outside surface of the part?
Just curious.
If the results are similar (which I am not sure and that's why I am asking you) I guess you would say that the ALL OVER profile is applicable/introduced only in 2009 standard and not in 1994? Right?

And yes, we are missing the basic radius for the slot depth.
Thank you

 

[pmarc]

Yes, profile all over concept can be used instead. You just have to make sure that absolutely all features you don't want to be controlled by that all over profile have different controls applied.

As a matter of fact the concept is also available in Y14.5M-1994 [see para. 6.5.2(a), page 167]. You can simply put ALL OVER note right beneath single profile FCF.

 

[sstemple]

Just out of curiosity, what is your general tolerance call out for basic dimensions?

We have a general profile gtol call out for basic dimensions. At times it can eliminate the need for so many DRF's and allows for better control of form and orientation than plus/minus tolerances

 

[greenimi]

sstemple,
I am not sure who you are asking, but since in started this thread, I will answer that we do not have a general tolerance for the profile dimensions. We have it for ± dimensions (2, 3 and 4 decimal places and the angle callouts)
Should we? Maybe, but that's beyond of my control.........
Thank you

 

[SeasonLee]

sstemple

I believe what you referred is general profile tolerance on the drawing, pls take a look on the link below for more details about the general profile tolerance. But, there isn't any tolerance on a basic dimension.

Link

SeasonLee

 

[sstemple]

Let me explain a little better... I attached an example of what we place on our prints to cover basic dimensions.

We use a general profile note for basic dimensions instead of ± dimensions (2, 3 and 4 decimal places and the angle callouts). Here's why...

The ± does not relate back to any datums like the profile tolerance does therefore the actual tolerance zone can move around during inspection depending on where you put the center within its tolerance zone. Each measurement is not repeatable or reproducible.

With profile the tolerance zone is centered on the basic surface relative to the referenced datums in the profile callout. GD&T applies the tolerances to the part features, something that may be touched or seen when inspecting, allowing reproducible measurements.

It may not necessarily be the correct path for what you guys produce, but we measure to the ten thousandths and even millionths

 

[fsincox]

sstemple,
I have wanted to do the same type of thing for a long time, how has it worked out for you guys? How long have you done it this way?

 

[sstemple]

We have been doing it for years, once we recieved formal training for GD&T. The instructor was the one who suggested it for us however I'm not sure if anyone actually fully understood it, it was just more of a CYA (cover your ass) note for most people. We have recently jumped into standardizing our whole department and while looking into our drawings and models we have gotten a better understanding of our gtols and dimensions.

In theory it seems more logical to use profile than +/-

 

[fsincox]

I don't disagree that it is better to have a state reference framework, I guess my real question is based on how homogenous are your parts do they range widely in size, and do they vary from machined parts to cast and welded? The kind of processes that might require lots of adjustment to the tolerance values used as the default?