Hole Position Usage 2

[lecuyero]

I have been following this forum for a few months now and thought I had a basic understanding of GD&T. I have a book as well and have read it cover to cover. We had a drawing review session last week and one of my drawings came up for question. The other drafters picked out my GD&T and marked it up.

There are 2 issues that I need clarification about. I thought you could declare positional tolerances with 1, 2, or 3 datums (or 0 but bad things can happen). In my drawing the relationship of the holes to the edges of the surface is not important. To save manufacture cost I did not call out the other datums. My book says this is OK to do but my colleagues do not. Which is correct?

Second issue is regarding projected tolerance. Am I missing something or is this correct usage of projected tolerance? The part that mates up to this part is 1" thick and the holes are .266+.003 and have a positional tolerance of 0.005

http://files.engineering.com/getfil...eb0-4f54-8c83-4411e80c95c6&file=gdt_usage.JPG

 

[dingy2]

In the diagram, there is a blind threaded hole and one cannot confirm the perpendicularity of this hole unless it is shown in a projected tolerance zone. I would assume that a threaded stud will fit in the hole. What is the length of this stud that will protrude beyond the surface? That will be the minimum size of the projection.

The first part of your question will raise a little controversy here.

It is legal the way you originally have it so that the positional tolerance is within a pattern (FRTZF) and the pattern location is shown with linear tolerances. That is legal.

The alternative to this method would be to have the composite positional tolerance from the face and sides (create datums B & C) and then within the pattern. The top section of the composite feature control frame (PLTRZF)should have a tolerance larger than .008" and the bottom section (FRTZF) .008. That would do it.

Again, I would keep the projection though.



Dave D.

http://www.qmsi.ca

 

[Belanger]

Yep ... as Dave said, everything on your original print is technically OK. Datum A's only job is to impose perpendicularity. And since there is a "2X" preceding the feature control frame, the position tolerance controls is still valid because it controls the distance between the two threaded holes. The location of the holes on the overall part is given by non-GDT tolerances. While legal, I would maintain that this does leave ambiguity regarding which of the outside surfaces is the primary datum and which is the secondary. (This is why Dave alluded to some controversy depending on who you ask.)

But think of it this way: In the left-hand view, if the bottom-left corner is not exactly 90º, do you want the inspector to flatten out mainly on the short surface or the long surface? This is not clear, and this might be why your colleagues prefer to have more datums. As Dave said, "composite position" can be used to make everyone happy.

A projected tolerance is not an absolute requirement, but it usually makes sense for holes like this because studs or bolts will protrude and that's the real "position" that is of concern.

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

 

[PeterStock]

One thing to keep in mind is that the height of the projected tol zone should be the max thickness of the part(s) being attached. Also what is the new datum C that appears to be the same surface as datum A? Your colleagues are correct in that there probably should be more datums referenced, which ones depend on the function of the part. It may be that the hole pattern should be the secondary datum (this would completly restrain the part and a tertiary datum would not be needed).

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services

http://www.infotechpr.net

 

[dingy2]

I would suggest that the Designer here use the term "MINOR DIA" under the feature control frame with projection is not incorporated. Leave that term out if projection is utilized.

One can check a minor diameter on a threaded hole but the projection requires a threaded checking plug to be threaded into the hole and one would check the OD of the plug at the top and bottom of the projection.

Dave D.

http://www.qmsi.ca

 

[dingy2]

I would suggest that the minimum length of projection is the length of the threaded stud that protrudes beyond datum A. I will assume that the threaded stud will assemble a mating part and then beyond so that a nut can be threaded.

A lot of Designers would place a composite feature control frame in this situation but I am not a Designer while J-P is from the design background. I have used drawings and try to understand the functional features so that we might be able to control them better and more frequently. Non-important features would not be controlled as well.

If you placed a composite feature control frame, I would assume that both the pattern location and also the holes inside that pattern are both important to its function. I would then have 2 checking fixtures built and I would be wrong. Only 1 is needed.

Inside the pattern of the two (2) holes to themselves and perpendicular to datum A is important. The hole pattern to the sides is not. I would use your original method except place a projection tolerance. The holes location can be easily measured from the bottom and also the side and I have actually performed this on a CMM many, many year ago. Since the part is symmetrical, it really doesn't matter if it is the left or right side. I don't find your original method ambiguous at all. I actually find that it reflects your needs as your stated.



Dave D.

http://www.qmsi.ca

 

[Belanger]

Dave, what do you make of the situation in my earlier post where the bottom corner is not exactly 90º? You keep saying that you come from the functional side and I from the design side, but isn't the precedence of the two implied datums a very practical question that renders the coordinate tolerancing system useless because of the ambiguity?

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

 

[lecuyero]

Thanks Dave. That is what I fear may happen. I changed the drawing to satisfy management but feel this new tolerancing will be added work on the inspector's part (at increased cost to us), all for a "form" that is not critical.

Would I be wrong to assume this second method is going to increase the cost of the part?

 

[KENAT]

Just wondering, how does this tally with ASME Y14.5M-1994 5.2 such as:

5.2.1.1 "The location of each feature...is given by basic dimensions."

I'd been taught to generally locate features controlled by position tols from datums, obviously excepting if the features themselves become the datums or the like.

Agree that it sounds like correct use of projected tolerance zone. If the part is secured by a screw & mating part is a max of 1" thick then 1.000 sounds correct. If a stud is being used then yeah, you probably need to allow for the total length of the stud projecting as during mating this will matter, however, I'm not sure why Dingy is so sure it's a stud, my first thought was screw.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[powerhound]

The lower frame in your composite FCF must be a refinement of the upper frame. In this case it's not so this wouldn't be a correct use of the composite FCF. Reverse the tolerances. Put .020 in the upper and .008 in the lower, also, reference A,B, and C in the upper and just A in the lower, This should get you to where you want to be.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X4
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[KENAT]

I think Powerhound means something like this:

http://files.engineering.com/download.aspx?folder=8d687aad-79c8-4cef-a38c-0dbfb5531d4d&file=FCF.jpg

Minor point, but check your leading and trailing zeros assuming you're working to ASME Y14.5 and using inches.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[KENAT]

Oh, and while I think of it, your tolerance is fairly tight for a threaded hole, especially with that much projection. Are you sure you need it, or can the mating clearance hole be made a bit bigger?

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[pmarc]

If you placed a composite feature control frame, I would assume that both the pattern location and also the holes inside that pattern are both important to its function.

Dave,
I would say they are both important for defining clear geometrical relationship within the part, not for function.
Fundamental dimensioning rule 1.4b says:
"Dimensioning and tolerancing shall be complete so there is full understanding of the characteristics of each feature."
Without upper segment the pattern can be anywhere and I can't really believe this is design intent.

That's why (if only perpendicularity is critical) I would specify upper segment with much bigger tolerance than the lower one. It would clearly inform design intent and in the same time no information about pattern's geometry would be missing.

 

[dingy2]

I know that I opened up this can of worms and I do apologize for that. I realize that we have had this discussion before and people can get quite worked up on it. Again, I do apologize.

Many who train in this subject suggest basic dimensions on each and every feature with only linear dimensions for features of size. Positional tolerances and profile of surface will be applied to everything and the tolerance applied might give the clue on whether the feature is important to its function and mating relationship. Default GD&T is now placed in notes although the datum reference structure may not be applicable to all features but we have our butt covered.

I found that the newest edition recommends this philosophy in the forward section but has so many contradictions of this philosophy throughout the standard.

J-P - Yes, the bottom corner may not be 90 degrees and even if we had a datum structure, we would assume it was 90 unless there was a qualification of some sort. The Designer in this situation stated that the pattern location is not important. While the standard recommends that we place a position tolerance on all features of size, it does not mandate it. One could have a linear tolerance and still be following the standard although there are no examples in either the 94 or 2009 standard. One might say that we are on the fringes of being illegal but are still legal.

Yes, we could have a composite feature control frame but are we relaying the design intent to the shop floor? Shop floor personnel would see it as two (2) requirements that requires two (2) checking fixtures. I would also review it in the same manner and I have been training in this subject since 1988.

Many years ago we had no to limited GD&T at all and I had to phone the Designer or Customer Quality to find out the how the part fits and functions with the mating part. We needed this information to develop the correct processes and Control Plan. In the situation under discussion, the Designer would state that the hole to hole position is important what the location of the holes to the sides is not. We would only develop one (1) checking fixture. I have a feeling that with the overuse of GD&T we may have to travel this route again.

Dave D.

http://www.qmsi.ca

 

[powerhound]

Dave,

Why do you think shop floor personnel would see composite position as two different requirements?

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X4
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[i2xtreme]

One other small thing.. you call out 1/4-20 UNC but what class? 1/4-20 UNC 2B? 1B, 3B? Also a depth of ±.010 is a bit tight, perhaps .75 min would be more mfgable.

 

[CheckerHater]

I am givng dingy2 a star for bringing importantant issue again.
I believe it was Gary Whitmire of Genium fame who figured that combining basic dims with FCF and "regular" dimensions may result in 6 different interpretation of FOS location.
No one ever answered my question, what if all 6 will result in a good part?
I agree with dingy, that conventional dimensions could be a good way to indicate less critical dimensions. Better than using special "critical dimension" symbol which is another 5-gallon bucket of worms waiting to be open.

 

[pmarc]

As Dave said, ASME Y14.5 is not giving any example of locating pattern of features with coordinate dimensions and I could agree that from purely legal point of view it is hard to judge whether this method is in accordance with the standard or not.

I would just like to mention that this dilemma is amazingly pretty nicely solved in ISO standards. ISO 5458:1998 clearly states that meaning of coordinate dimensions is not standardized in such applications and basic dimensions should be used instead to locate a pattern.

Why? I suppose they simply realized 'coordinate dimensions' method leaves plenty room for different interpretations and gives no possibility of clear and full definition of part's geometry.

 

[dingy2]

Please excuse my rant of yesterday. I do get worked up sometimes in this subject on its overuse.

I overlooked the fact that the FCF was in RFS (RMB now) and thus no checking fixtures would be allowed. All features would be given the same treatment and measured using a CMM or other variable measuring instrument.

Dave D.

http://www.qmsi.ca

 

[dtmbiz]

Dingy2,

Havent had time to think through this at length and it seems as if you have, so....

How does this mix/match work using a combined
+/- rectangular tolerance zone with a FRTZ cylindrical tol zone?

I do agree this would definitely classify as a "can of worms".