Controling Location of Tapered holes ?

The traditional way to measure the location and dimensions of tapered holes is with gage balls.  I think it's still the best way for most purposes.

I.e., not a cylindrical pin or a tapered pin, but two perfect balls of specified, usually standard, sizes.


 

Mike Halloran
Pembroke Pines, FL, USA

I would use gage balls to determine axial the location of the taper and runout (like your figure 2) to control the radial location.

No matter circular runout or total runout  used on fig.2, it's a surface to an axis controls, while position is axis to axis control, it will depend on what you want to control. But Fig.4-3 in 2009 standard use surface profile to control it.

SeasonLee

Hi, SeasonLee,
You have mentioned Total runout can be used, is it possible to use total runout for tapered shafts/holes?
I think as you menstioned, Profile is best.  

Madhusudhan Veerappa
Mechanical Engineer

Total runout is OK on tapered surfaces as long as the angle of the taper wrt the datum axis is given as a basic angle.

(Yes, I know the standard doesn't give such an example, but recall that GD&T is a language and as long as intrinsic concepts are not being violated it is fine to apply the symbols in ways that might not be specifically shown.)

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

Hi John-Paul,

Thank you for the reply, Since I am new to GD&T ,Could you please help me to get the answer for the below questions.

1) When I mention the basic angle for the tapered hole wrt datum A and apply total runout to the part. Does it mean that the part inspector has to rotate the part to the basic angle and need to take the measurements. because when it is rotated wrt datum it becomes straight?

2) If I mention the taper hole angle in basic, from where it will gain the tolerance ? Is that the +/- tolerance for the end diameters of the tapered holes will indirectly give the tolerance for it (Similar to Fig 2-14 of ASME 1994 Std.)?

3) If I make the angle basic, Then I feel mentioning any one of the end diametrs with +/- tolerance would be enough. If I mention both the end diametrs, then it may leads to conflict. Please correct me If I am wrong.  

Madhusudhan Veerappa
Mechanical Engineer

1) For total runout: the part rotates around the datum axis in a regular manner (no angle_, but the measurement device would have to be rigged so that it can slide along the taper.  Think of a dial indicator sliding along a rail that is at the precise angle from the datum.  (I forgot that you are dealing with a hole, so it may be tricky to get an inspection device in there.)

2) The basic angle just sets up the inspection device. The actual tolerance on that tapered hole's angle comes from the total runout tolerance.

3) That's right -- one of the diameter callouts will have to go, since the angle would be basic.

I don't know if total runout is the best way here; I was just saying that it's possible.  Think of it as a regular total runout tolerance on a straight cylinder, but we're just saying that instead of the cylinder having zero degrees (basic) taper, it has another (basic) angle.  But I'd really have to calculate all the trig to see what happens for your example.

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

Total runout is an entire surface acts as an entity being controlled to a datum axis, total runout controls cylindricity and concentricity,it is a control of both form (roundness and taper) and location (centering), so it is good to assist in the form and balance of spinning parts. Circular runout is only a 2D control while total runout is a 3D control, if you want to choose runout, I will recommend to use total runout on this case.

When you inspect the part with total runout control, you don't need to rotate the part to the basic angle, the part is just mounted in a datum feature simulator to establish the datum axis, the part is then rotated and a dial indicator is used to obtain a total runout error reading (pls note the indicator travels along datum axis surface while the part is rotated).

The tolerance zone for a total runout control is two coaxial tapered cylinders whose centers are located on the datum axis, the radial distance between the cylinders is equal to the total runout tolerance zone. The +/_ size tolerance is the max and min limits of the size dimension, all actual local size must be within the limits. For any part inspection, you need to check the size tolerance, Rule #1 boundary and geometric control.

Indeed, most of tapered cone surface tolerance is controlled with surface profile, since it will control not only the shape of the conical surface but also its size.

SeasonLee

Good point, SeasonLee.  Total runout on a taper is real close to profile of a surface, but profile has the extra control of size. Total runout is like profile, but it "unlocks" the size control.

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

SeasonLee,

Quote:

The tolerance zone for a total runout control is two coaxial tapered cylinders whose centers are located on the datum axis, the radial distance between the cylinders is equal to the total runout tolerance zone.

If I got your statement correct, you are saying that the total runout value is equal to the distance between tapered cylinders in a direction perpendicular to a datum axis, right?

I am asking, because I would say it is equal to a distance between the cylinders in a direction normal to nominal contour of a conical feature (see fig. 9-2 in Y14.5-2009).

Forgive me, if I interpreted your post wrong.

pmarc

Yes, you are right, I should say "in a direction normal to nominal contour of a conical feature " instead of the "radial" distance between the cylinders. I couldn't find out a total runout example in 2009 standard for a tapered cone, Fig.9-2 is a circular runout.

SeasonLee
 

Please look to attached picture. This is the presentation of a method of locating conical (tapered) feature that I was trying to describe some time ago in one of the threads about similar issue.

http://files.engineering.com/getfile.aspx?folder=0fd8eba3-7512-4cf7-b383-8cb4b500f071&file=location_conical_feat.JPG

Basically saying it is a combination of profile of a surface (that is controlling orientation and form of the conical feature as well as length of the cone) and tolerance of position (location of the feature relative to datums A, B, C) applied to a single circular element (diameter of the base of the cone).

Of course - as usually - this method has some pros and cons. IMO the biggest advantage is that (M) or (L) modifier can be applied to the positional tolerance for bringing bonus tolerance concept into play. The weakest point I see is a fact that the concept of positional tolerance of a single circular element of a feature has not been described and legalized anywhere in Y14.5, so it does not have to be clear for a reader how to interpret the requirement specified.

Any comments are really welcomed as I am very interested in clarifying the issue of allowable method of locating conical features?

Madhu454

pmarc's post remind me that we haven't replied your question in fig.3, it seems we all concentrate on total runout and profile control, we forgot the OP is "Controlling location of tapered holes".

I will say yes, you can use position to control location of the tapered hole, as I mentioned earlier that position is axis to datum axis control, the tolerance zone is on the axis, so you don't need to call out position on both ends of the tapered hole. As pmarc stated that the biggest advantages is material modifier can be applied, bonus will be generated and more parts can be accepted, but this could be a disadvantage for a spinning part since the bonus tolerance could endanger balance of the mass. I am not quite sure the purpose and its function on your part, for a precise spinning part, I will not choose position control.


SeasonLee

pmarc, since you asked for any comments ...  I think your posted picture is OK except that the diameter of 12.0-12.4 should be basic.  (A profile tolerance must be applied to a "true profile").  But the premise works for me; it seems similar to the philosophy shown in Fig. 8-24 of 2009 (or Fig. 6-19 of 1994).
 

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

Belanger: It looks to me like Fig 8-17 in ASME 14.5-2009 would contradict your statement that the 12.0-12.4 diameter should be basic and would agree that what pmarc has proposed looks similar to the BOUNDARY principal in ASME Y14.5-1994 (p. 171) and combined control in 14.5-2009 (p. 176). However it would seem to me that a two segment FCF pointing to a surface would be required to invoke this principal.

All: What I'm curious about now is how the bonus tolerance is determined on a conical feature. Would the two cases in the attached file have a bonus tolerance? Would specifying multiple gage lines to define locations where the local diameter is to be measured be worthwhile and then take diameter with the largest departure toward the MMC to calculate the bonus?

If pmarc's drawing was used with the diameter in question specified as a size, and leveraging Fig 8-17, it would seem to me that the diameter at the top would alone determine the bonus tolerance.

I guess I'm looking at this from employing a quick inspection method without have to make an attribute gage so maybe I'm be too narrow minded.

• http://files.engineering.com/getfile.aspx?folder=db625a34-2910-4a27-85e1-b0

J-P,
I put diameter 12.0-12.4 as a size dimension intentionally, because this allows me to have bonus tolerance when needed. Basic dimension would not let me to have it. I was rather trying to utilize (with some modifications) dimensioning schemes shown in Figs. 8-17 & 8-18 of 2009 edition. But for sure I would not consider my proposal similar to BOUNDARY (or combined) concept.

PRDAVE00,
In my opinion bonus tolerance concept for whole conical feature can't work, because a cone does not have unique size dimension which would determine how much bonus tolerance is avaliable. Therefore - as you correctly noticed - I wanted to use the diameter at the top (base) of the cone alone to determine the bonus. And, as I already mentioned, this seems to be the biggest roadblock since such approach is not mentioned anywhere in Y14.5.

I somehow wanted to see if my proposal was clear for readers.

Hi John-Paul,

I am curious to know below things, Please help me to inderstand GD&T better

1) if we make the dimension as basic, then the M modifier in the positional tolerance is still valid? Don't we need to remove that?
since there is no MMC limit. Then the axis interpretation has to be made, how do they determine the axis? (what is the AME for tapered holes? - is it the gage balls they use as Mike Halloran said in the above post.)

2)  In your above post you have said (A profile tolerance must be applied to a "true profile") . I have few doubts on profile. In one of your earlier post you have said, profile can be used like a flatness control. Please refer to the attached file.
Figure-1 and figure-2 gives the same meaning and Figure-3 and Figure-4 gives the same meaning. Here there is no basic dimension is used in the figure-1 and figure-3, but still we can use profile control. My question is, we have not defined any thing in basic here -what is the true profile here.?  

(By going through the other posts on the forum i understood that, using higher level specifications (ex:profile) must be avoided when there is a option to use lower level specifications ex-flatness. I agree completely on this. My question is regarding -making the dimesion 12.0-12.4 as basic in the lost post you mentioned)

I may be wrong, but I interpreted the drawing in this way, The dimesion 12.4-12.0 controls the size. The profile tolerance 0.4 wrt datum A locates and orients the top surface of the conical tab. the profile tolerance with 0.2 tol wrt datum A controls the orientation and form of the surafce (within the size limts of 12.0-12.4). and finaly with the position tolerance with M modifier (a boundary of 12.9 base dia and 10 basic angle to itfor a height of 14 min )will control the location of Tab.

Madhusudhan Veerappa
Mechanical Engineer

• http://files.engineering.com/getfile.aspx?folder=57dd8ee3-87e4-4e8d-a8ae-0e

Madhu454,

Quote:

I may be wrong, but I interpreted the drawing in this way, The dimesion 12.4-12.0 controls the size. The profile tolerance 0.4 wrt datum A locates and orients the top surface of the conical tab. the profile tolerance with 0.2 tol wrt datum A controls the orientation and form of the surafce (within the size limts of 12.0-12.4). and finaly with the position tolerance with M modifier (a boundary of 12.9 base dia and 10 basic angle to itfor a height of 14 min )will control the location of Tab.

Basicaly, this is exactly what my intetion was with one exception however - position tolerance is controlling location of single circular element at the base of the cone, so the boundary you described would not apply.

I am visualizing a 'functional' gage for the position callout as an untapered hole of 12.9 diameter, perfectly oriented to datum plane A and perfectly located at basic 20 and 50 wrt datum planes B & C. The thing is with the depth of the gage's hole: from theoretical point of view it should be infinitely thin, but in reality I believe that any thickness will work.

It has to be kept in mind that profile of a surface verification must be done with a separate check since it is impossible to build a hard gage that would verify profile & position simultaneously. It is even impossible to build a hard gage that would verify profile of a surface alone.  

Evan, I still say that the diameter must be basic. Otherwise, it conflicts with the notion of profile tolerance on the cone. Why is a toleranced diameter necessary for bonus tolerance to occur?  The profile tolerance allows the diameter to vary, so it provides the bonus effect.

I think we need Dean in here because in the past he's had some thoughts about profile's relationship to bonus tolerance.

Madhu, profile can be used on a flat surface; and that is still being applied to a true profile.  The basic dimension of a flat surface is implied as zero. Now the location of that flat surface can vary within a toleranced dimension, but the true profile of the surface is perfectly (basic) flat.   I'll look more closely at your sketch and post later.

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

John-Paul
Just commenting on your last response... I have not read the rest of the thread.

When profile controls size as well as and form, orientation, and/or location it can be thought of as a control that the tolerance is both "zero at MMC" and "zero at LMC"... giving the feature its greatest freedom to rotate and translate at the profile's median contour.

Paul
 

I agree, Paul.  But for Evan's point, I think we can still say that the size variation provided by the profile control factors into the position tolerance, and provides bonus.

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

Whoops, check that -- I see what you mean, Paul. If a cylinder/cone is at its biggest, it can't move; but if it's at its smallest, it also can't move.

I'll have to noodle this idea, but I still refer Evan to Fig. 8-24 where ASME shows a similar concept.

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

PrDave ... good point about Fig. 8-17.  That's been the subject of several forum discussions, and I'm not the only one who thinks that example is a little strange.

I only say this because paragraph 8.2 says that a profile tolerance defines a tolerance zone "relative to a true profile."  The same paragraph defines a true profile as "a profile defined by basic radii, basic angular dimensions, basic coordinate dimensions, basic size dimensions, undimensioned drawings, formulas, or mathematical data, including design models."

Figure 8-17 has a basic angular dimension, so I get how the profile tolerance controls the angle of taper.  But don't they need a basic dimension for the diameter? Otherwise, it's not really controlling profile in the round aspect of the cone, and profile of a line might be more appropriate.
 

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

madhu454

The geometric tolerance should be less than the size tolerance on your latest post fig.1 and fig.2, take fig.1 for example: the surface profile tolerance 0.5 is greater than the size tolerance 0.2 (10.2 – 10.0), it's a conflict.


SeasonLee

madhu454

Quote from Al Neumann GD&T workbook page 12.3 :
"Profile tolerance is also very versatile. The classic profile specification is usually applied with datums and basic dimensions. But profile can also be applied with plus/minus tolerances. If it s applied with plus/minus tolerances, depending on the situation, it will react like a form or orientation tolerance and must be within the confines of the plus/minus tolerance."

On a flat feature, surface profile tolerance zone is two parallel planes equally displaced about the true profile, the surface must lie within these two parallel planes, in other words, the surface variation is controlled by these two parallel planes, so surface profile will also control the flatness, this is same as surface parallelism will also control surface flatness.

SeasonLee
 

Sorry to keep pushing the point, but now that I'm at home I am able to draw some sketches of why I think Fig 8-17 is questionable.  Earlier I wrote that profile of a surface must always have a basic dimension to describe the shape.  (Of course profile's relationship to the datums doesn't have to be basic, but any dimension defining the shape itself should be basic, in my understanding of para. 8.2.)

See the attached figure.  The first example applies profile to a flat surface.  We have established that this is OK -- the basic dimension is zero (no curvature; a mathematician could even say a radius of infinity) so it is identical to a flatness callout.

I presume everyone is also OK with the second picture -- the surface is slightly curved, so a basic dimension is required to define the "true profile."

The third and fourth pictures are the same, but they have a more dramatic curve.  Isn't it true that I must give the radius as a basic dim, not a ± ?

The last picture just takes it to the full curve, which we call a circle.  I'm proposing that the diameter of the circle must be basic, just as the other radii were basic.   But I am hearing from some folks that suddenly it's OK if this diameter is directly toleranced.

I don't mean to be stubborn (I know I've even insinuated that the standard goofed on this), but help me see what I'm missing that makes it OK to apply profile of a surface to a hole that has a  ± tolerance on its diameter.

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

• http://files.engineering.com/getfile.aspx?folder=eb4e200c-ea90-4509-ad3b-b5

John-Paul,
I agree completely that if a size or shape characteristic of a profile tolerance zone can be expressed by a basic dimension, then it must be...  Leaving that basic dimension off would mean that the drawing is incomplete.  There are some who have taught otherwise, but I contend that the standard does not back this up...  The problem is partly due to those figures that combine profile and plus/minus.  They are confusing for sure.

The reason I say that what profile controls cannot be affected by the presence or absence of a basic dimension is that there will then be cases for which there will be ambiguity...  Those cases are when a basic distance of zero, or a basic angle of zero, or any increment of 90 degrees, is present, so the basic need not be shown...  We cannot then know whether a basic is present or not.  Also for an annotated 3D CAD body (per Y14.41) the model is queried to get basic dimensions, so how could the presence or absence of a basic affect what profile controls for those cases..?

The 2D size tolerance and position that pmarc shows is a different animal though, in my opinion (clarification is needed in future standards on this)...  The 2D size and position tolerances (on a circular cross section and its center point) may be a refinement on the control provided by the profile tolerance, couldn't they?

Dean
www.d3w-engineering.com
 

Hi,
I dont have the copy of 2009 std, the Figure 8-17 is it Fig 6-23 of 1994 standard.  

Madhusudhan Veerappa
Mechanical Engineer

Madhu454

Yes, Fig.8-17 of 2009 is same as Fig.6-23 in 1994 standard.

SeasonLee

Dean,
I agree about basic dimensions sometimes (often?) being implied, such as a zero basic dimension of coincident lines.  Same thing for CAD data; the "dimensions" in the CAD model are basic.  So whether the basic dims are displayed directly or implied, a profile tolerance must be applied to a feature whose form is defined by basic dimensions.  I didn't mean to imply that a literal basic dimension has to be shown on the drawing. But to place a toleranced diameter on a cylinder which will get profile of a surface tolerance is contradictory.

When dealing with a cylinder or cone, the issue is that the dimension defining the form (which must be basic) is inherently tied to size.  See the attachment provided in my previous post.

I disagree with your last paragraph.  I certainly understand the desire to separate size and form, but I think that the way profile operates on a cylinder/cone, there's no way to do so. Again, see the attachment; I can't really do it justice here with text.

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

Pmarc,   In your post of 14 July at 2:45, you said that there is no similarity to your proposal and boundary concept given in Fig. 8-24.    Why?  (I would say that that is a more proper way to use profile and position together on the same feature.)   Is it because those feature control frames are stacked together?

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

J-P, I said this not because position and profile FCF's are not stacked together in my proposal. I think there is a difference in geometrical interpretation of both methods, which does not mean 'my method' is the correct one. Actually the more I think about it, the more shortcomings I see. Figs. 8-17 & 8-18 indeed seem not to be the best thing that happened to Y14.5-2009 standard. I just wanted to somehow utilize them by combining with other tolerancing techiniques (positional tolerance in this case).

By appling positional tolerance separately from the profile I was additionally aiming for giving an option of picking RFS, MMC or LMC concept depending on the feature's function. Fig. 8-24 does not give it. The 'boundary' concept works fine only when (M) or (L) modifier is placed in the tolerance portion of position FCF. RFS concept would rather require usage of typical profile of surface approach. In my proposal (assuming everything else worked fine) simple addition or removal of material modifier symbol would do the thing.  

John-Paul,
There is a way to apply a size tolerance to a feature which also has a profile tolerance applied...  If the size tolerance is tighter than the size control provided by the profile,then it's a refinement of at least the size, and possibly also the form of the feature (depending upon how much tighter it is than the profile value).  I'm not saying that this would be a likely or good practice, but nothing in the standard precludes it.

For a cone, a size tolerance, if applied, can only be applied to a 2D cross section of the feature...  What the size tolerance then means could be an issue, since a cone is not a feature of size.  Let's just say for now that a 2D size tolerance is OK here...  As long as the size tolerance range is tighter than the profile tolerance value that may also be included, then the size tolerance would have an effect and it would undeniably be valid.  Again, not necessarily a likely or good practice, but we must have a clear and sensible requirement from a standard to say it's not valid.

I am firmly in the camp that says that profile and +/- should not be combined, but if pmarc's figure had a size tolerance range tighter than 0.2/cos(cone's included half angle) (tighter than +/- 0.1004 since the angle is 5 degrees on pmarc's cone)(assuming that the 2D size tolerance zone is radial and not normal to the surface of the cone), then this is a combination of size and profile that I think is just two separate and independent tolerances...  The profile does its job and the size tolerance independently plays its own role.  One thing about pmarc's figure though...  That Position tolerance should only apply to the center point of the single cross-section...  If only a standard provided clarification of that point, we would be better off.

One more thing to mention is that a 2D size tolerance on a cone seems odd, but industry does it every day with modifiers like "+DFT" or "-DFT" or the alternative practice of "Draft reduces material" or "Draft adds material".  This practice is an imprecise one, but for small angles (draft), and hopefully relatively large tolerances, everyone seems comfortable enough with it.

Dean
www.d3w-engineering.com

Dean, I think I understand your comments, and because of Fig. 8-17, I suppose I am obligated to accept such a practice.  But to make that really work, they need to clarify paragraph 8.2 to say that there are times when a profile tolerance doesn't have to be applied to a true profile (i.e., basic dims).

I would be more likely to agree with all this IF we were talking about profile of a line.  (This would be kind of the opposite of your scenario -- where the size tolerance is 3D but the profile tolerance is 2D.)

Here are some questions that arise in my mind if we say that a basic diameter is not always required for profile:

If profile of a surface is applied to a cylinder where the diameter has a ± tolerance, would profile of a surface be identical to cylindricity?

If profile of a surface is applied to a partial cylinder (think of an arc that sweeps only 30 or 40º), then is the radius of that arc required to be basic?

If the answer to the previous question is no, then couldn't each picture in Chap. 8 of the 2009 standard be modified to eliminate basic dims, if so desired?

If the answer to that second question is yes, then how far must an arc sweep before we say that it is no longer required to be a basic dim?

Once again, I understand the desire to unlock profile from a basic size, but I can't help thinking that we'll get backed into a corner somewhere in all this.

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

John-Paul,
I must be stating my opinions in the wrong way...

Profile on a cylinder absolutely requires a basic diameter.  Profile on a cone requires complete definition by basic dimensions, but if no datum features are referenced that definition may be only the basic included angle of the cone (since the tolerance zone is free to translate in the axial direction it effectively become variable in size).  If translation in the axial direction is constrained by a referenced datum feature then a basic dimension to the cone's apex may complete the definition, or as an alternative, a basic diameter combined with a basic dimension to define the axial location of that diameter may be used.  Of course if the referenced datum features constrain all degrees of freedom then the cone's axis must be located by two more basic dimensions.

Even with a fully constrained, and fully "Basic dimension defined" profile tolerance zone, there is nothing that precludes the application of a sufficiently tight size tolerance to refine the size and possibly form of the feature.  Not that I would recommend this, but nothing in the standard says this could not, or should not, be done.

Dean
www.d3w-engineering.com


 

Dean,  I think I see the reasoning if some careful caveats are in place:  only on a cone, and only if no datum references are given.  The bit about axial translation makes sense; since there may be some movement in that direction, the exact diameter cannot always be nailed down.  (I hereby retract my questions re Fig 8-17!)

pmarc's picture has datum references on the cone, so for that example I think my comments have merit.  The issue that remains open is how to determine bonus tolerance in the case where profile is used on these cones. (See PrDave00's post.)

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

DEAN, JOHN-PAUL,

Thanks a lot for your really valuable comments about my proposal.

I have been thinking and thinking about figs. 8-17 & 8-18 in Y14.5 2009 edition and it is really interesting that these figures have not been changed comparing to 6-23 & 6-24 in Y14.5M-1994 - therefore I suspect there has to be a reason for keeping them in the standard and there has to be a logical explanation of how to understand them without assuming they are inappriopriate.

DEAN, if I got you correctly, you think that my concept could work if a size tolerance was a refinement of profile of a surface tolerance value divided by cosine of cone's half angle. But looking at 8-17 for instance it is rather not the case - size tolerance is much greater than profile tolerance value. And I believe it can be explained if size dimension and profile of a surface are treated as two completely independent requirements. With such approach I do not see any conflict between them. Profile controls form of a cone's surface of revolution only (without impacting its size) while the diameter dimension limits size of single circular element (base of the cone). IMO, these two requirements can be met independently. Please take a look to attached presentation (page 1) in which I tried to explain graphically my point of view using my proposal.

JOHN-PAUL, in your last post you said that 8-17 could work only if no datum reference in profile of surface FCF was given. I would say that addition of at least A datum to profile callout (like I did in my proposal) is not making the figure vague and is not conflicting with anything in the standard. Referencing A in the FCF orients profile tolerance zone relative to datum plane A. Please refer to page 2 of attached document to see how I understand presence or absence of datum reference A in profile FCF.

http://files.engineering.com/getfile.aspx?folder=73af64c4-23d5-40c7-b557-44b1f2a32109&file=profile_cone.pdf    

pmarc,
I'm not entirely in agreement that figure 8-17 provides a helpful example.

In the figure you attached I think all that you assert would be true if you used a customized datum reference frame and specified "A" as instead "A(v,w)"...  This way A provides orientation constraint to the profile tolerance zone, but it does not constrain translation in the x direction as it normally would.  Normally, the reference to A would constrain the cone's apex in the axial ("x") direction and therefore make the profile effectively control "size" of the cone (which can be viewed as "at each cross-section" if that's more comfortable, since a cone is not a feature of size).

Dean
www.d3w-engineering.com
 

Hi All,

I've been busy this week so I haven't had time to follow or contribute to this thread until now.  Very interesting discussion.

I would agree with J-P and Dean that allowing +/- to be mixed in with profile and alter its meaning is not one of Y14.5's brightest moments.  One of the main objections I have to this mixing is that it is presented in a non-rigorous "definition by example" way.  All we are given are figures 8-17 and 8-18, in which a +/- tolerance can somehow take away a profile tolerance's ability to control the "size" of a feature.  A cone is an unfortunate feature to demonstrate this on, because translating a cone along its axis has a similar effect to changing its "size".  IMHO, Figure 8-18 is a conceptual train wreck.  We also have Figure 8-27, in which a +/- tolerance somehow un-refines (coarsens?) the location control usually provided by profile.  Are there other cases in which we can replace a basic dimension with a +/- tolerance and change the meaning of profile?  Like the cylindrical surface J-P mentioned, with both a profile tolerance and a +/- size?  If we replace a basic angle with a toleranced angle, will this take away a profile tolerance's ability to control orientation?  Where does it end?

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

Why not use a composite profile tolerance and all basic dimensions?

Peter Truitt
Minnesota

Evan, I agree that profile with plus/minus can lead to a trouble, but only in the case of Fig. 8-17.  That's because profile intrinsically controls form, and when dealing with a cylinder or cone, the very number that defines form (diameter) is also the one that controls size.  With Dean's comments, I feel a tad better about it now, but I think we all agree that some clarification in the standard would be helpful on this specific point.

However, I wouldn't take issue with Fig. 8-27 because that plus/minus dimension has nothing to do with the form of the surface being toleranced.  That is merely a location dimension, and the profile tolerances are not intrinsically required to control location: it's an optional add-on.

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

John-Paul,
I think Figure 8-27 (Y14.5-2009) should be deleted from the standard...  With "A" referenced, the profile tolerance zone would be constrained in location and a basic dimension of 80 mm must then be provided.

Figure 8-18 must have the reference to datum feature B deleted.

Dean
www.d3w-engineering.com
 

Dean... here's the best way to think about profile:  It always controls form (that is its intrinsic purpose).  It can also control orientation (if a datum reference is given).  And it can also control location (if a datum reference is given and a basic dimension back to the datum is given), and location obviously includes orientation as a sub-control.

Fig. 8-27 is the middle of the three scenarios I describe; datum A is meant for orientation purposes only.

Also look at paragraph 8.2, which says it this way: "Profile tolerances are used to define a tolerance zone to control form or combinations of size, form, orientation, and location of a feature..."

Fig. 8-27 controls a combination of form and orientation.  In this case think of it as parallelism of "each element," where datum B helps define the orientation of the elements to be sampled.   So a basic dimension is not required.

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

John-Paul,
The way to think about profile cannot include misconceptions that are not explicitly supported by the standard.  The figures that have been pointed out here cause confusion and what your saying here will do the same.

The presence or absence of a basic dimension cannot be used to determine what profile controls.  This is a common misconception that others have written into their books and included in their training.  It is a misconception that finds support only by the implication provided by a couple of figures in the standard that must be revised.

I think this is the highest priority issue to get clarified in the next version of the standard.  Only after this will the improper training, and confusion it generates, stop.

The presence or absence of a basic dimension cannot have any effect regarding what profile controls since there are times when basic dimensions are not shown, such as distances of zero or angles that are zero or any increment of 90 degrees.  We also don't show basics if annotating a 3D CAD model per Y14.41 instead of using a 2D drawing...  Since one has no way of knowing whether a basic is present or not for those cases where they're just not shown for other reasons, then it is completely illogical to depend upon their presence or absence to determine what profile controls.

Only the capability of the referenced datum features to constrain the profile tolerance zone determine what is controlled.  If there is a desire to release one or more of those degrees of freedom then now with Y14.5-2009, a customized datum reference frame can be used.

Sorry to be so blunt, but this issue is one that needs to get clarified and resolved asap.  It's a big cause of confusion within a subject that has, as part of its purpose, the resolution of confusion.

Dean
www.d3w-engineering.com

It's OK to be blunt, but I really think you're stirring up a non-issue.  Why is it a misconception to state that profile tolerances can control orientation but not location?   There's an example of such in Fig. 8-27.  It's true that more pictures of this usage might be helpful, but I'm at a loss for how we can claim that such usage is not even allowed.  See the attached graphic for a quick comparison that I've used in the past; you will agree with the second example but probably dislike the first example.

You say that "the presence or absence of a basic dimension cannot be used to determine what profile controls."    I would say that it can.   The only reason that I hear for why it can't is in regards to the case of dimensions not being displayed.

But there are already rules in place for that.  See paragraphs 1.4(a) and 2.1.1.2 (and also Y14.41).  If the distance back to a datum is not shown and it's understood to be basic, then that profile tolerance controls location.  If the drawing leaves off dimensions as a general practice, but shows the distance back to the datum with a direct tolerance, then the designer is really trying to say something:  that particular profile tolerance controls orientation only (and form, of course).

 

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

• http://files.engineering.com/getfile.aspx?folder=c2e350fa-2604-48a1-954f-52

John-Paul,
It is a misconception to say that the presence or absence of a basic dimension will affect what profile controls.  My statement in the post above is very clear on this, so I am completely confused about how you could have misunderstood what I was describing as the misconception.  Of course profile tolerances can be used to control orientation and not location...  They do this when the datum features referenced constrain only the orientation of the tolerance zone or if a customized datum reference frame is used to release the translational degrees of freedom that would otherwise locate the tolerance zone.

The sections you cite say nothing to support the assertion that some people make that what a profile call-out controls is affected by the presence or absence of basic dimensions.  Nothing in the standard says this.  To take that position is illogical, when all things are considered.  Yes, some confusing figures that need to be deleted or revised imply this, but no words at all explicitly say this.

If you think this is a non-issue, then you haven't seen the drawings that I have that were produced by a group that had received training that taught them the profile misconception which they then tried to run with.  The drawings were nothing but utter confusion and the reason for this was directly due to  this very real issue.

Dean
www.d3w-engineering.com

Dean, I hope we're not boring the others.  (Perhaps this topic of Fig. 8-27 deserves a separate thread?)
  
I encourage you to offer more explanation of the problem, because I indeed see no issue with relying on basic dimensions (or lack thereof) to dictate whether the profile tolerance controls orientation or location. If the drawings you mentioned really did run with this concept but to a wrong conclusion, I'd be interested in where they really made a wrong turn, because the concept of Fig. 8-27 is sound in itself.

You keep saying that it's a misconception to say that the presence or absence of a basic dimension will affect what profile controls.  Yet you agree that profile can control orientation (not location) "when the datum features referenced constrain only the orientation of the tolerance zone..."

The natural question then becomes:  How are we to know when the datum features referenced constrain only orientation?  Can't that easily be determined (a la Fig. 8-27) by seeing that the distance to the datum is directly toleranced, not basic?

 

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