Tolerancing of cones

[pmarc]

Short question:
Take fig. 8-17 from Y14.5-2009. Delete profile FCF and add length of the cone (let's say 50+/-0.2).
Would that be enough to treat the cone as fully defined?

 

[powerhound]

No, because the angle is basic. If you also give the angle a +/- tolerance, I think that would suffice.

John Acosta, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[CheckerHater]

The way I see it the cone is not fully defined even WITH profile requirement.
Profile tells you where conical surface is located in radial direction but it doesn’t tell you where it ends lengthwise (unless you specify the length basic or not).
So both pictures look “intentionally incomplete” to me.
And please clarify the idea of ”fully defined”:
Fully defined from middle school point of view? Fully defined as a feature to be checked? Fully defined to be used as a datum?
You know better than me that GD&T is full of subtleties

 

[pmarc]

CH,
As I said, assume the length of the cone is 50+/-0.2.

By fully defined I mean that its size and form is unambiguosly defined.

 

[CheckerHater]

In this case I will side with ph.
In absence of FCF basic 15 deg angle makes no sense.
So all three dimensions (diameter, angle, length) being +/- dimensions should be good enough.

 

[pmarc]

Okay, so another question:
Figures 2-20 and 2-21. The angle is expressed by basic flat taper or basic conical taper, but no profile FCF present. Would profile of surface callout be really needed in case of these two figures to fully define size and form of the features?

 

[CheckerHater]

You have to specify the size of your tolerance zone somehow. It is pure geometry:
On Fig.2-21 it is done by combining “perfect” basic DIA 23 AND TOLERANCED 10.1/9.9 length.
If 10.1/9.9 dimension on Fig.2-21 was basic 10 instead, you would need to add profile to specify the width of the tolerance zone.
I still don’t understand what are you trying to prove – that there is more than one way to dimension a cone?

 

[pmarc]

I am wondering whether basic angular dimension can or cannot exist without profile tolerance.

Look what is happening on fig. 2-20. Assuming that this is a cone and not a wedge, basic ratio 0.15:1 indirectly defines basic angle of the slope. Now, if we take my modified version of fig. 8-17, it would be different to fig. 2-20 only in a way how basic angle was expressed, am I correct?

So what if I did not want to express the angle of the cone by +/- angular dimension (as you and Powerhound suggested), because I was not interested in a tolerance zone being two non-parallel lines? What if in the same time I was absolutely OK with the surface lying within boundaries defined by dia. 30+/-0.2 dimension?

Do you see my point?

 

[CheckerHater]

OK, now I think I am getting it.
Say, you have basic angle, basic length and toleranced diameter.
Or basic angle, basic diameter and toleranced length.
Yes, it will be enough to define tolerance zone. It just will be less convenient. Your basic taper gives you simple ratio between length tolerance and radial tolerance. Basic angle will require use of trigonometry on the shop floor.
So using profile with basic angle is more like “best practice” (but it really IS best).
By the way, when you check NPT thread with ring gage your gage is your basic diameter and basic angle and you actually put tolerance on the length of engagement as specified by the standard (+/- one thread or whatever).
Is that what you were asking?

 

[fsincox]

It has alwas been my understanding that it can, in the past. So I say yes.

 

[CheckerHater]

Yes, basic angle without profile symbology may be enough to theoretically (mathematically) define location and shape of tolerance zone. Will it bring any practical advantage? I am not sure. I can imagine the tooling and technique used for checking the part won’t be much different from what you may normally use for profile.
But I can think of another application. Basic dimensions are sometimes serving another purpose, the one some are ashamed to admit: they are used to dimension fixturing you use to inspect the part.
Look at Fig. 4-49 14.5-2009. Every time you use sphere in the way shown, or round pin to measure thread or gear, these are the objects dimensioned in basic, meaning they are to be produced to “gage maker tolerances”.
If you can imagine the part that for some reason must be inspected the way shown on enclosed picture, this could be good legitimate use for basic angle without profile requirement.

 

[pmarc]

CH,
I do not know why, but you somehow assumed in your considerations that at least 2 dimensions defining the cone are basic. What I meant is to have only the angle basic. Do you still think it would be enough to fully define size and form of a cone?

As for basic dimensions used to dimension a gage/fixture, I have no problem with that. Standard is quite clear about it (para. 4.24.7). I wish it was that clear when talking about different methods of cone tolerancing. In my opinion it is a bit of a mess.

 

[CheckerHater]

Pmarc,
You know, it’s like National Treasure movie where FBI agent played by Harvey Keitel keeps repeating “Somebody has to go to jail”. Something has to be basic.
Think of it this way: you need 2 basic coordinates and tolerance to create unambiguous position control.
Same thing here: 2 basic dimensions (one of them angle) designate theoretically exact place in space and toleranced dimension is responsible for specifying (thru some trig) the width of tolerance zone.
Otherwise tolerance zone will be dependent on both diameter tolerance and length tolerance creating ambiguity/tolerance stack-up I don’t even want to think about

 

[pmarc]

Okay, I buy this. Thanks.

 

[fsincox]

Yes, I do think I understand what is conveyed if a part is dimensioned that way. No, I do not know how popular it will be here!

 

[MechNorth]

Let's look at a situation here; a conical taper with toleranced diameters at both ends and a tolerance length;. Even without an angle called out (basic or toleranced), that used to be enough information to manufacture the cone, right? What happens on the conical surface between the two toleranced diameters? Don't know ... pretty much anything because there's no control on that zone. If the angle is basic, there's no indication of the inflection point (small end, large end, half-way, 2/3 way ... ?), so you don't know what the tolerance zone looks like and therefore you don't know what the surface can look like. +/- limit on the angle helps to establish the angular limits on the surface, which can control the entire surface ... but you still don't know where the inflection point for the angle is. +/- would need an origin of measurement indicator.

Now the above is relevant only if it's the only feature, or if it's establishing the primary datum feature. If the cone has to be controlled wrt anything else, profile is your only real choice. I spent a lot of time working with precise conical tapers. Originally we used +0.005mm on diameters (both ends) and toleranced length, and hoped that the tapers were well centered on the axis of the part; once we went GD&T, we controlled conical tapers within a unilateral profile of 0.0025mm, then used the tapers to establish datums.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[fsincox]

I am not sure if the point of inflection is as unclear the way the OP was laid out.

 

[pmarc]

Jim,
I fully agree that all these considerations are relevant only if feature is treated as a single feature, without any relation to other datums, and that otherwise profile of surface is the best option.