×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Hole Position Usage
2

Hole Position Usage

Hole Position Usage

(OP)
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/getfile.aspx?folder=01b142c6-6eb0-4f54-8c83-4411e80c95c6&file=gdt_usage.JPG
 
 

RE: Hole Position Usage

2
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.
www.qmsi.ca

RE: Hole Position Usage

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

RE: Hole Position Usage

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
www.infotechpr.net

RE: Hole Position Usage

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.
www.qmsi.ca

RE: Hole Position Usage

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.
www.qmsi.ca

RE: Hole Position Usage

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

RE: Hole Position Usage

(OP)
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?

RE: Hole Position Usage

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: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: Hole Position Usage

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

RE: Hole Position Usage

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: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: Hole Position Usage

Quote:

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.  

RE: Hole Position Usage

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.
www.qmsi.ca

RE: Hole Position Usage

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

RE: Hole Position Usage

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.

RE: Hole Position Usage

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.

RE: Hole Position Usage

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.   

RE: Hole Position Usage

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.
www.qmsi.ca

RE: Hole Position Usage

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".

 

RE: Hole Position Usage

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:

Quote (powerhound):

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.


 

RE: Hole Position Usage

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.
www.qmsi.ca

RE: Hole Position Usage

Dave,

Just 2 comments to what you said:

1.

Quote:

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.

Quote:

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?   

RE: Hole Position Usage

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.
www.qmsi.ca

RE: Hole Position Usage

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.
 

RE: Hole Position Usage

dtmbiz,

You said:

Quote:

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.   

RE: Hole Position Usage

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.

 





 

RE: Hole Position Usage

dtmbiz,

Quote:

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.

Quote:

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.

Quote:

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.

RE: Hole Position Usage

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
www.infotechpr.net

RE: Hole Position Usage

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.





 

RE: Hole Position Usage

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.


 

RE: Hole Position Usage


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
 

RE: Hole Position Usage

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.
www.qmsi.ca

RE: Hole Position Usage

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?


 

RE: Hole Position Usage

(OP)
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

RE: Hole Position Usage


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
 

RE: Hole Position Usage

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

RE: Hole Position Usage

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 !


 

RE: Hole Position Usage

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

RE: Hole Position Usage

(OP)
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/getfile.aspx?folder=0aed7931-ed0f-46f9-a9f5-c6d2fe70ed0b&file=gdt_usage_incorrect.JPG

http://files.engineering.com/getfile.aspx?folder=db3dee95-8025-4789-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.
 

RE: Hole Position Usage

If the hole pattern MUST be a datum then attach the B datum identifier to the FCF and position the holes relative to A only. The only problem is that if you are identifying a B datum then you should probably locate something relative to it. The only thing I see is the outside profile, in which case you will need to use "Profile".

Is there a problem with making the long edge B and the short edge C, then positioning the holes (using basic dimensions) to A, B, and C? I You can use a composite tolerance with .020 in the top section located WRT A, B, and C and then in the lower frame put .008 WRT to A only. That will more tightly control the perp AND the distance between the holes but leave the pattern itself to be free to wander within the .020 tolerance zone.

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

RE: Hole Position Usage


Happy New Year to all who loves GD&T.

Lecuyero

On your latest post, the 1st drawing is incorrect. If you are using pattern as a datum feature, be sure attach the base of the datum feature symbol to the FCF (hanging from the FCF) as shown on your 2nd drawing, you can't just directly adhere to a hole feature. Besides, secondary datum B should be removed from FCF.

The 2nd drawing is correct except the secondary datum B should be removed from FCF, the 2 threaded hole is a pattern and used as secondary datum, so can't use itself as a reference datum. However, you need this datum if there are other features relative to the secondary datum (pattern). Fig. B on my attachment is a good example for your reference---when to use a pattern as a datum.

Fig. A is the recommended callout for your case, of course you may choose composite tolerance as an alternative method, but I prefer to the projected tolerance zone since it is an easy way to meet your design intend, a simple case. Do not complicate a simple issue.

SeasonLee
 

RE: Hole Position Usage

PowerHound,
What you have posted in reference to requirements regarding positional tolerancing is in complete agreement with what I had posted. I believe because there are no basic dimensions or datum references relating the edge surfaces to the holes, then this cannot be a correct positional tolerance accoding to the standard. I believe yourself and others then go further to say the original drawing is incorrect.
There's where we part paths.

 You say logic cannot be used to eliminate the true position possibility and consider the edges being located from the hole(s) center. It is true that the hole FCF is legal to control the holes perpendicularity and distance to each other.  It is true that features of size can be dimensioned legally according to the standard without using positional tolerancing.  Dingy2 says that the holes are being positioned from the edge as a pattern. I disagree with that opinion because there would be a mix of a rectangular tolerance zone and a cylindrical tolerance zone. I see this as problematic.

I have never said that the original drawing was the best way to define the drawing as shown. I simply say that it is NOT illegal according to the standard and go on to give examples from the standard to support my position. SeasonLee's last post simply claims the drawing is incorrect with nothing that I see supports that opinion based on the standard. If it's there, then please show me.

The following examples from the 1994 standard illustrate dimensioning to holes without the use of  "positional  tolerancing".  Without the use of the "origin symbol"  whether or not the dimension starts from the edge or hole is a matter of interpretation. There is nowhere in the standard that states positional tolerancing with a cylindrical tolerance zone is mandatory. BTW I personally believe the positional  tolerancing "is" the best way to go.
pg 6 fig 1-4; pg 7 fig 1-6; pg 9 fig 1-14; pg 10 fig 1-18
Rectangular Coordinate, Baseline,   Polar Coordinate dimensioning
pg 19 fig 1-48, 1-49; pg 20 fig 1-50, fig 1-51

 

RE: Hole Position Usage

dtmbiz,

  Your examples are completely out of context of our discussion. We are discussing tolerances of postion and your examples are specifically about what dimensions and leader lines are supposed to look like and how they are placed. The standard provides examples to illustrate the point being made and some are incomplete by intent. I'm not even sure what point you were trying to make by providing them. I know how dimension lines are supposed to look and how they are placed.

  That being said, I think I had the wrong impression of what your position was on our topic. I've been under the impression that you thought it was okay to use +/- dimensions to position a feature using a true position callout and FCF. From reading your last post I don't think that's what you were trying to say. Were you?

  I do see what you're saying regarding the edge being located from the holes instead of vice-versa and this is why this print is technically illegal because it violates 1.4(d) of the standard. It can be interpreted in more than one way.

  Regarding the logic, nothing can be left open in GD&T. I know of a legal case where logic was pitted against what the standard said and the standard won in court. It was the reason that "Spotface" got its own symbol in the 2009 standard.
 

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

RE: Hole Position Usage

PowerHound, Seriously? Figs are out of context?

Quote;
"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"

These are references to dimensioning "without using basic dimensions". Or maybe this is one of those "logical" times to ask for your definition / context as to what you mean by "positioned"? Maybe I'm not understanding you?

 Rectangular and Polar Coordinate, Baseline dims. If you read the corresponding paragraphs it clearly states that these types of dimensions can be basic or non-basic. Is your opinion that if a standard uses a fig to focus on let's say broken extension lines; that the rest of the fig is erroneous; not to standard, even though it may not be complete? If you place the ASME Y14.5 reference on a drawing format, you can dimension the entire drawing without basic dimensions nor FCF's of any kind and still comply with the standard.

Quote:
"That being said, I think I had the wrong impression of what your position was on our topic. I've been under the impression that you thought it was okay to use +/- dimensions to position a feature using a true position callout and FCF. From reading your last post I don't think that's what you were trying to say. Were you?

I was not suggesting in any way to use +/- dimensions for a proper "positional tolerance" call out. You are correct that we are in agreement to use basic dimensions.

As far as 1.4(d)..... good luck.... just re-read this thread and how many others with all the various interpretations. I am not saying this is wrong, however for those that oppose using the standard, this is one of the standard's fundamentals that is used to advocate not using the standard. In light of this I have been thinking about what the intent of this paragraph is. It is obvious that in many cases using coordinate dimensioning and not using the origin symbol, many dimensioning schemes would be subject to more than one interpretation. I wonder if this paragraph is aimed more at the interpretation of what feature is being dimensioned. For instance that a feature be clearly dimensioned to an intersection, tangency, or center point (axis). Or maybe "one interpretation" as to what datums are being defined. I'm not really convinced myself on this one, however if 1.4(d)were applicable to all callouts "in the real world", then I don't think this forum would exist.

I would be getting off topic to write more about my point of view on logic. Where is the standard for subtraction and addition to calculate virtual conditions for example? Or any other math calculation for that matter. Where is it in the standard that we use for instance the word "parallel" in the context of geometry and not "a parallel conversation"? Where in the standard does it mandate the formula to choose a profile callout let's say, other than a positional callout? Where in the standard does it state exactly what order of precedent the DRF datums should be in?  I'm fairly certain that you won't see that these are relevant examples either. That's Ok with me, hopefully, we'll just agree to disagree.

As for the case you sight, where can I read about this spot face controversy? [b]I do not think the standard(s) are flawless.[\b] Humanoids are involved.

Back to the OP and my assertion that the original drawing is legal. Since you bring up a  court  of  law in the US, then I shouldn't have to remind you that unless one is proved to be found guilty according to a particular law; then I will continue to assert that this callout is legal until I see a convincing argument that sites the standard proving it is not legal.

That's my story and I am sticking to it...





 

RE: Hole Position Usage

Very interesting discussion.  I haven't had time to jump into this but I will now.  Here are some thoughts:

I would say that the original drawing is compliant with Y14.5.  The Position FCF obeys the rules - the relationships between the considered features and the datum features are all basic.  There are explicit basic dimensions for the hole spacings, and implied basic 90 degree angles for their orientation relative to datum A.

Fundamental Rule 1.4(d) is a very big can of worms, and worded in such a way that it cannot be meaningfully applied.  It's difficult to say what the original intent of this rule was - I think that dtmbiz is right that it was probably something to do with clearly defining which feature(s) a dimension applies to.  If one goes beyond that and looks at how dimensions can be defined on a real (i.e. imperfect) part, then 99.9% of drawings violate Rule 1.4(d).  Other than size tolerances on regular features of size (cylinders, spheres, slots), directly toleranced dimensions (a.k.a. plus/minus tolerances or coordinate tolerances) are ambiguous on real part geometry.  There are no rules on how to define directly toleranced dimensions on a real part, so they are fundamentally subject to more than one interpretation.  Yet Y14.5 allows them, describes them, and provides many examples of their use.

So the directly toleranced dimensions on the original drawing are legal, but not without problems.  Their meaning is clear on a drawing or model, but ambiguous on a real part in which the holes are not perfectly round and the edges are not perfectly flat and square.  Which is every real part, so there is always some ambiguity.  This used to drive me crazy, and I was an advocate of limiting the legal use of directly toleranced dimensions to simple sizes only.

But I eventually realized that directly toleranced dimensions have their place, because there are many applications in which they are used successfully.  Directly toleranced dimensions go along with a simplified approximation of the part geometry, in which the features are assumed to have perfect form and perfect orientation.  In situations where the form and orientation error of the features is small in comparison to the size and location tolerances, directly toleranced dimensions can be the lowest cost option.  The overall savings gained from simple dimensioning and simple inspection can outweigh the costs of multiple interpretations.  Geometric tolerancing is the tool of choice if you need things to be fully defined, but sometimes the quick-and-dirty approach ends up being cheaper.  

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

RE: Hole Position Usage

Evan:

You certainly have changed your original thinking.

I absolutely agree with you that one could apply directly toleranced dimensions on a drawing where there is no function and mating relation while the geometrical applications could be applied to fully describe the design intent where there is a need.

I realize that you, MechNorh and I have had some "intense" discussions in this area in the past but the standard reflects origins without the application of GD&T.  

Dave D.
www.qmsi.ca

RE: Hole Position Usage

Dave,

I may have softened my stance on directly toleranced dimensions, but I'm not ready to admit that I agree with you yet ;^).

I still don't agree with the rule of thumb that directly toleranced dimensions should be used when there is no functional or mating relationship between the features, and geometric tolerancing when there is.  All features on the part have a function and dimensional requirements that go along with it, otherwise the feature wouldn't have to exist.  The requirements may be very loose but they are there, and geometric tolerancing would always be capable of giving the largest tolerance for manufacturing while meeting the functional requirements.  But in many manufacturing situations the extra tolerance cannot be taken advantage of, and does not result in a significant cost saving.  In these situations, the complexity of GD&T ends up not being worth it.  The simplicity of directly toleranced dimensions wins out, even though it gives away some tolerance and makes borderline parts very difficult to evaluate.  Many companies are willing to live with these headaches, or avoid them by not making parts that approach the limits.  Simple inspection can definitely be bought by making parts with very good form.

I do agree with you that the standard has its roots in directly toleranced dimensions and gradually added geometric controls to the tool set.  Users have found that there are many applications where directly toleranced dimensions are "good enough" and other applications where they are not.

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources