Controling Location of Tapered holes ?

[Madhu454]

Hello All,

Please see the attached drawing.
I need to control the location of tapered hole with respect the outer shaft diameter,

Question
1) Can I use circular runout to control this? Circular runout controls both form as well as location of each sections wrt datum A. ?
2) Can I use Position control for this?? Is it possible to use position control to locate the taper hole? Please refer to figure-3, I got confused for which dia I need to apply position control. Assume that I have used Position control for dia 20.0-20.1, how do they establish the axis? Is the AME will be a cylindrical pin or taper pin? If they use cylindrical pins will touch the part at only one point and will not get into the taper hole. The same way if I use position tolerance for smaller hole dia.

Please let me know the best method to control the location of taper hole. also please let me know whether Position control can be used for this?

Thanks for your time.

Madhusudhan Veerappa
Mechanical Engineer

 

[MikeHalloran]

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

 

[dans95]

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

 

[SeasonLee]

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

 

[Madhu454]

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

 

[Belanger]

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

 

[Madhu454]

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

 

[Belanger]

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

 

[SeasonLee]

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

 

[Belanger]

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

 

[pmarc]

SeasonLee,

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.

 

[SeasonLee]

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

 

[pmarc]

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/getfil...3-8cb4b500f071&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?

 

[SeasonLee]

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

 

[Belanger]

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

 

[prdave00]

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.

 

[pmarc]

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.

 

[Madhu454]

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 (exrofile) 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

 

[pmarc]

Madhu454,

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.

 

[Belanger]

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