Member Login

Remember Me
Forgot Password?
Join Us!

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!

Join Eng-Tips
*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.
Jobs from Indeed

Link To This Forum!

Partner Button
Add Stickiness To Your Site By Linking To This Professionally Managed Technical Forum.
Just copy and paste the
code below into your site.

Tolerancing of cones

Tolerancing of cones

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?

RE: Tolerancing of cones

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

RE: Tolerancing of cones

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 smile

RE: Tolerancing of cones

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.

RE: Tolerancing of cones

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.

RE: Tolerancing of cones

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?

RE: Tolerancing of cones

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?

RE: Tolerancing of cones

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?

RE: Tolerancing of cones

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?

RE: Tolerancing of cones

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

RE: Tolerancing of cones

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.

RE: Tolerancing of cones

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.

RE: Tolerancing of cones

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 smile

RE: Tolerancing of cones

Okay, I buy this. Thanks.

RE: Tolerancing of cones

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!

RE: Tolerancing of cones

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
TecEase, Inc.

RE: Tolerancing of cones

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

RE: Tolerancing of cones

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.

Red Flag This Post

Please let us know here why the post below 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!


Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close