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

 

[flash3780]

Dave's comment about referencing the MINOR DIA rather than the PITCH DIA is a mess to stack. I'd stick with the default. Projected tolerance should stay as well (try stacking the joint without it - a mess). The projection should be the length of the stud.
I think powerhound is correct in stating:

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

I do wonder what the maximum depth of the tap drill is, though. Hopefully the tolerance on the threadform depth is covered by the general drawing tolerances.

 

[dingy2]

I have thought about this for a while and will probably bring a bit of controversy again to this topic.

What is the design culture in your company? Is your company one that only applies GD&T where it is needed to reflect the function and mating relation? Your drawings reflect a blend of both linear and geometric tolerances. - OR - Does your company apply GD&T on all features whether applicable or not to the feature's function? In other words, no linear/polar tolerances at all. Most 1st tier automotive companies comply with the second philosophy.

The approach to applying GD&T in this example depends upon your company's philosophy and culture.

1 Reflecting GD&T only where needed company - I would suggest that there is a positional tolerance of diametrical tolerance zone of.009 at MMC Projected 1 inch relative to datum A. The location of the pattern would be reflected in linear tolerances from the side (.375) and from one end. This would definitely show that there is a strong relationship between the two (2) holes in the pattern while the location of the pattern is not important and is marginally in compliance to ASME Y14.5 - 2009.

Shop floor would probably just check the pattern from the sides and one (1) end with a vernier caliper while there would be a checking fixture for the features inside the pattern. Long term control will concentrate on the checking fixture rather than the location of the pattern.

2 Reflecting GD&T on all dimensions company - I would suggest that there is a positional tolerance of, maybe, around a diametrical tolerance zone of .025 relative to datums A, B (create the side as datum B) and C (create one end as datum C) in a RFS mode. Place MINOR DIA under the feature control frame. This positional tolerance would have to be checked using variable gauges (not conducive to long term checking) and on the minor diameter. Some on the shop floor might even convert this to a linear tolerance which isn't quite correct but not harmful. Note that there is no projection in this feature control frame since it is controlled by the lower segment feature control frame.

Below the first feature control frame, I would suggest another feature control frame where there is a positional tolerance of a diametrical tolerance zone of.009 at MMC Projected 1 inch relative to datum A. This is not a composite feature control frame since the bottom segment has different requirements from the top segment. This would be a single segment feature control frame.

Shop floor would probably use a checking fixture for the bottom segment feature control frame and it is conducive to long term control. Long term control is utilized when the requirement is important to its function and mating relationship and having a positional tolerance at MMC lends itself to long term control.

Dave D.

http://www.qmsi.ca

 

[pmarc]

Dave,

Just 2 comments to what you said:

1.

Does your company apply GD&T on all features whether applicable or not to the feature's function? In other words, no linear/polar tolerances at all

GD&T on all features does not mean no linear/polar tolerances - coordinate dimensioning is still useful for defining such geometrical characteristics like size of features, chamfers or radii.

2.

Reflecting GD&T only where needed company - I would suggest that there is a positional tolerance of diametrical tolerance zone of.009 at MMC Projected 1 inch relative to datum A. The location of the pattern would be reflected in linear tolerances from the side (.375) and from one end. This would definitely show that there is a strong relationship between the two (2) holes in the pattern while the location of the pattern is not important and is marginally in compliance to ASME Y14.5 - 2009.

Why do you think it would be obvious for somebody to consider location of the pattern specified by linear tolerances less important than positional tolerance with projected tolerance zone? Based on the tolerance values given? Or based on the fact that coordinate dimensioning is easier (?) to understand and more common on drawings?

 

[dingy2]

pmarc:

1. Agreed - I should have stated coordinate tolerances rather than linear since features of size require a +/- tolerance. Neither a radius (under 180 degrees) or a chamfer are not features of size. If one uses full GD&T, then chamfers and radii would be basic for profile of a surface application.

2. When one reviews a drawing that has limited application of GD&T, then the features with GD&T become more outstanding or more important than the coordinate tolerances. As an example, if one had a profile of a surface on one particular surface while all the other surfaces are shown in coordinate tolerances reflect the importance of that one surface.

I don't think the coordinate is any less nor more difficult than positional tolerances to understand but I have been at this for a while. Projected tolerance zone sometimes can be confusing though.

Dave D.

http://www.qmsi.ca

 

[dtmbiz]

lecuyero,
The original drawing is perfectly correct. Everyone seems to be reading this as the hole being positioned from the edges which are not indicated as datums. I agree the FCF controls perpendicularity for the holes to datum A and because there are 2 holes, the positional symbol is correct with a basic dim locating the holes to each other. If there were just one hole then the perpendicularity symbol would be used IMO. This drawing shows the holes as most important and the edges are built around them. Think of this as a large piece of material which 2 holes are drilled and tapped. Then the outline of the block is cut relative to them. I know this isn’t the likely way for the part to be manufactured but it illustrates the feature’s importance as called out. This would be why the edges have general toleranced dimensions to position the edges relative to the holes. It is not that these dimensions serve as pattern locating. It would not be wise to use a plus-minus tolerance zone in conjunction with a diametrical tolerance zone. In basic GDT classes this rectangular tolerance zone has a “corner” on the hypotenuse that is a larger distance than the “plus-minus” values. It is a classic reason as to the advantage of a cylindrical tolerance zone. To use a rectangular tolerance zone in conjunction with a cylindrical tolerance zone will only lead to problems. The idea that using the surfaces defined as B and C in the second drawing “costs” more; IMO is not true. It is a “different” callout and suggests an importance for datums B and C; (e.g. that they contact a mating part). Although the original “before” being marked-up and the second drawing with a composite callout are both correct, they both indicate “different” feature importance.
You originally state that the mating part is 1” thick which would make the projection distance in the 1st drawing correct. IMO use the MMC of the mating part thickness for the projected value.
I would add that the use of datums does not “cause bad things to happen”. Datums are a fundamental of the standard and are “building blocks” as to defining a parts features relative to function and interface.

 

[pmarc]

dtmbiz,

You said:

This would be why the edges have general toleranced dimensions to position the edges relative to the holes.

Original drawing is not saying this. Since pattern of two holes is not assigned as datum feature B and the edges have no geometrical tolerance referencing datum B, there is no information which of these features are more important.

 

[dtmbiz]

pmarc,

The drawing is delineated in such a way that can absolutely be interpreted as valid and compliant with the standard. This interpretation is in agreement with what the OP stated was the design intent; holes important, edges not so much.

I have presented a logical interpretation of the drawing per the standard. The FCF and basic dim between the holes are the requirements to locate and orient two tapped holes to a single datum. Logic concludes that the outside edges come from the hole position, not the holes from the edges, according to the delineation of this drawing from what is presented.

IMO an interpretation based on an "assumption" that there is an error or something lacking with this callout, while the callout is obviously compliant with standard and the OP stated the objective to control the holes, while the edges (surfaces) were not that important; then IMO that interpertation is asserting what the interpreter wants instead of what the drawing calls for.

The second drawing does show the holes from the edges.

The callouts, datums (or lack there of in this case) and the delineation paint the picture. It is not uncommon to locate features such as the tapped holes via FCF and datums; and then to locate a surface from those features. It is not part of the standard to require a feature to be dimensioned from a datum.

This is a clear example for a drawing to be mis-interperted or "reading into it" what is not called for when looking at the entire dimensioning scheme along with the stated design intent.

 

[pmarc]

dtmbiz,

The drawing is delineated in such a way that can absolutely be interpreted as valid and compliant with the standard. This interpretation is in agreement with what the OP stated was the design intent; holes important, edges not so much.

- Can you indicate a paragraph or a figure in Y14.5 that would show a situation when part outline is dimensioned from a pattern of holes with the use of coordinate (plus/minus) dimensioning?
- We know which features are more important because OP described this in simple words. However I will keep saying that the drawing is not precise in reflecting design intent and other persons who would not know OP's description can interpret it in a different way. Why do you think all inspectors of this part would measure outline from the pattern and not pattern from the outline? The print is leaving an area for different interpretations.

IMO an interpretation based on an "assumption" that there is an error or something lacking with this callout, while the callout is obviously compliant with standard and the OP stated the objective to control the holes, while the edges (surfaces) were not that important; then IMO that interpertation is asserting what the interpreter wants instead of what the drawing calls for.

I do not arbitrarily assume there is an error on any print. I just believe that full and unambiguous description of part's geometry should be the major goal of GD&T usage. If existing callouts do not do this, then I am putting my remarks.

This is a clear example for a drawing to be mis-interperted or "reading into it" what is not called for when looking at the entire dimensioning scheme along with the stated design intent.

The fact that your interpretation is different than mine somehow proves that this print is not clear. Why do you think it is me who mis-interprets the drawing? Maybe we are both right or both mistaken. Again, please show me a figure in the standard that would show pattern as an implied datum and the part's outline dimensioned from it.

 

[PeterStock]

What is not clear about the op initial drawing comes from the use of coordinate dimensions to locate the outer shape features of size with the resulting lack of control as to how that measurement is to be made. I would suggest using basic dimensions and a profile tolerance to allow for the maximum possible tolerance. Note the initial is compliant with the standard but that does not mean it is not ambiguous in some way. If the part is made of bar stock (likely from the initial drawing), I would show the overall dimensions as basic with a profile tolerance that would allow both the size variations and warpage of the stock material.

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services

http://www.infotechpr.net

 

[dtmbiz]

pmarc,

After a quick scan of the thread I see were you join with others in the case for the holes being located as a pattern. Either these folks consider the 1st dwg to be lacking in datums or that a plus-minus dim locates the holes. This would be a rectangular tolerance zone. Know responds to this point as to how a rectangular tolerance zone works in conjunction with a cylindrical tolerance zone. It doesnt make sense as to why this would be done.
Thus it is obvious to me that assumptions are being made to make a "correct" DRF and corresponding FCF.

The original drawing can only be interpreted as I described and still comply with the standard without altering the original dimension scheme and adding accomodating datums.

The standard does not have all encompassing example figures. Many senarios are not in the standard. The ones that are there are not necessarily complete. Page 1 para 1.1.4.

If you can envision that the non-basic dimesions are relating a pattern tolerance zone, then maybe you can envision....

5.2 (b) 2nd pars...

"Basic dimensions establish the true position from
specified datum features and between interrelated
features."

5.2.1.1
"The location of each feature (hole, slot,
stud, etc.) is given by basic dimensions. Many drawings
are based on a schedule of general tolerances,
usually provided near the drawing title block. Dimensions
locating true position must be excluded
from the general tolerance in one of the following
ways:
(a) applying the basic dimension symbol to each
of the basic dimensions [see Figs. 5-l(a) and (b)];
(b) specifying on the drawing (or in a document
referenced on the drawing) the general note: UNTOLERANCED
DIMENSIONS LOCATING TRUE
POSITION ARE BASIC."

Logic:
If the postional FCF does not reflect "Basic dims" for locating the holes;
A. The holes are locating the edges.
B. The callout is incomplete
C. Ignore the standard references above and locate the holes with non-basic dims.

For me its easy to see the holes are the start point and the edges are defined from them.

quote:
"Why do you think all inspectors of this part would measure outline from the pattern and not pattern from the outline?"

I really try not to use the word "all" and I certainly do not know what inspectors think. I do however know the standard fairly well and its application.

IMO, We are arriving at different interpretations because some are making assumptions and not interpreting the callout litterally. BTW, once again the original drawing is legal and logical, however not my preferred callout.

 

[dtmbiz]

pmarc

I did want to let you know that I do agree with you that IMO it might be better to ID the holes as a pattern datum and possibly use a profile tolerance for the bounding surfaces as PeterStock has mentioned. However if for instance this were bar stock then the stock tolerances could apply.

My intent here is to point out that the original callout is correct and compliant per the standard. I agree it may not be the optimum callout.

 

[SeasonLee]

Here is my 2 cents on this topic:

1. “When a hole pattern is used as a datum feature, it does not have to be located from the outside edges of the part. The outside edges of the part can be defined from the hole pattern and tolerance with a profile control.” Quoted from the last paragraph on page 350 of the book “GD&T Self-Study Workbook” by Alex Krulikowski. You may find the details from the attached.
The threaded holes is a pattern indeed, but they are not used as a datum feature. Therefore , the statement above is not applicable to this case.

2. When to use a projected tolerance zone modifier ?
A rule of thumb : Whenever the height of the clearance hole (mating part) is greater than the depth of the threaded hole, the projected tolerance zone modifier should be specified.
For this case, the projected tolerance zone modifier should be used, since the mating part height 1” is greater than the threaded hole depth .75. But this projected tolerance zone modifier can’t be used on the lower segment feature control frame (FRTZF) as mentioned by Dave, since a single datum reference used on the TOP (Tolerance of Position) control means to control the spacing and orientation of the holes in a pattern.

SeasonLee

 

[dingy2]

SeasonLee:

One cannot confirm positional tolerances at the depth of a blind threaded hole but can confirm its position at the surface. I should also add, unless the threaded hole is really quite large but the holes in question are only 1/4 inch. A CMM stylus (finger) cannot reach down to .750 depth contact around the ID of the minor diameter. I would still suggest a projected tolerance zone whether the mating part or threaded stud (if used) is not higher than .750.

Dave D.

http://www.qmsi.ca

 

[dtmbiz]

SeasonLee,

I am not quite sure what you are saying about this (original) drawing.

Are you saying that because the holes are not identified as datum feature
that you cannot measure to the edges from them?

It is possible to measure the holes per their related FCF. And then the edges could
be measured from the holes at RFS. Would you say that is “illegal”?

Or am I not understanding your point?

 

[lecuyero]

When I think about it more...if the hole pattern was defined as the secondary datum then my original drawing would show original design intent. I could declare the edges with general tolerances and the only basic dimension would be the 1.500 between the holes. The perpendicularity of the hole pattern to the edges would be controlled by general tolerances and there should be no way the holes could end up "outside" the material.

Dingy, to answer your question: Our company only uses GD&T when regular tolerancing does not suffice. I generally only use it for hole locations and carefully controlled surfaces

 

[SeasonLee]

Dave

What I said is a general rule of thumb to use a projected tolerance zone modifier, if you think the perpendicularity of the threaded holes are really critical on the application, of course you may specify it on the print no matter the mating part is higher or lower than the threaded hole depth.
BTW, I will use Tru-Pos Locators to measure position and orientation tolerances of tapped holes, since the CMM ball arm may touch the deep threaded hole edge especially for a tilted tapping hole.

dtmbiz

I would say the original drawing (2nd post) is correct except the datum reference, I will measure it based on the DRF and FCF (datum precedence A-B-C).

Lecuyero

You are right and I agree and recommend to use the hole pattern as a datum feature, as you mentioned that the holes to the edges of the surface is not important, this change will simplify any confusion that may caused.

SeasonLee

 

[powerhound]

dtmbiz,

I read your post with the paragraphs from the standard and they indicate that location of features is given by basic dimensions. The original drawing is incorrect but the markups to show basic dimensions is a good redline. I don't agree with either of the comments by the FCF though.
The whole purpose of the standard is to eliminate the use use of logic or common sense from drawings because not everyone has one or the other. One of the fundamental rules states that there can only be one interpretation of a drawing. If there is more than one interpretation, and the others cannot be invalidated by the use of the standard, then the drawing is illegal.

Nothing says that the holes are built relative to the edges or that the edges are built relative to the holes, this is ambiguous and violates the fundamental rule. Holes located with true position MUST be located using basic dimensions. This is per the standard and paragraphs that you provided. It even specifically says that block tolerances are to be excluded and the methods to be used both make the dimensions basic. Nothing in the standard says that logic must apply in order to override ambiguity.

In your last post you asked about whether you could measure the holes and then measure the edges of the part from the holes; you could do that but with a lack of a datum reference frame, it is only a 2 point measurement from each hole, it doesn't take the planar features into consideration. That may be just fine, or it could make a bunch of scrap parts.

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

 

[dtmbiz]

Powerhound,

Your opinion is noted. I obviosly disagree that the standard supports your opinion. I do agree the part outline is not controlled very well as delineated in the original drawing. I stated before that I would have done it diffently. As PeterStock mentioned before, if the holes are in bar "stock" then those industry tolerances apply and a profile tolerance would not be appropriate.

If you can point me to the paragraph and or fig(s) in the standared that supports your opinion then I will review it.

I agree, common sense isnt too common anymore.

Logic from Webster:
"a (1) : a science that deals with the principles and criteria of validity of inference and demonstration : the science of the formal principles of reasoning.

The standard principles and fundamentals depend on logic. If logic cant be used then we shouldnt be in "the business".

I do hope you have a great New Year !

 

[powerhound]

dtmbiz,

I'll just reference your post:

This paragraph says that basic dimensions establish true position from specified datum features and between interrelated features.
==>5.2 (b) 2nd pars..."Basic dimensions establish the true position from specified datum features and between interrelated features."

The first part of this paragraph reaffirms the above paragraph.==>5.2.1.1"The location of each feature (hole, slot,stud, etc.) is given by basic dimensions.

This part of the paragraph says that dimensions locating true position nust be excluded from the general tolerance block==>...many drawings are based on a schedule of general tolerances, usually provided near the drawing title block. Dimensions locating true position must be excluded from the general tolerance in one of the following ways:

This of the paragraph gives the methods by which the dimensions can be excluded from the general tolerance block. Note that both methods result in a basic dimension==>(a) applying the basic dimension symbol to each of the basic dimensions [see Figs. 5-l(a) and (b)];(b) specifying on the drawing (or in a document referenced on the drawing) the general note: UNTOLERANCED DIMENSIONS LOCATING TRUE POSITION ARE BASIC."

I understand your case for logic but it's not in the standard. These paragraphs that YOU provided are where the standard says that positional tolerancing requires basic dimensions. If these words aren't enough to convince you then there's really nothing left...maybe you can show me a place in the standard where it says features can be positioned using non-basic dimensions, and maybe I'll become a believer. As far as showing you any figures, look at any figure in chapter 5 and notice that every single one uses basic dimensions to positionally locate features. Can you point me to the paragraph or figure that supports your opinion?

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

 

[lecuyero]

I tried to use the hole pattern as a datum but kept running into the issue of requiring the datum B to be defined by datum B. The first drawing I'm pretty sure is illegal. The second drawing still gets my design intent across but I'm not sure if it is ambiguous. I still want to refrain from defining any of the edges with basic dimensions.

http://files.engineering.com/getfil...9f5-c6d2fe70ed0b&file=gdt_usage_incorrect.JPG

http://files.engineering.com/getfil...5-4789-a9ab-3ce70361161a&file=gdt_usage_2.JPG

My logic goes: If the pattern was defined with the standard A-B-C datum system then the hole locations would be more precise and costly than I need/want. Using a composite feature like was suggested doubles the amount of inspections for each hole. If done on a large part with hundreds of holes I can imagine this cost difference being significant.