Define mismatch allowance on a cylindrical ID

[cbrf23]

Hi,
I'm looking for someone to take a look at the tolerance I've proposed and tell me if this is the best way to achieve the control I need, described below.

This part is made in a lathe as a side A/B process, and as such there is a mismatch that can occur where the tool path exit and entrance blend from each side.
This needs to occur in the thick wall area, and there cannot be a step larger than .002 (see illustration included in attached screenshot).

I'm thinking profile of a line best controls what I want, and could be inspected at the machine using a v-block and indicator checking at a few places around the cylinder (part of control plan).
Physical inspection at the machine is important, which is why I was considering profile of a line vs surface, as profile of a surface I believe would require a CMM or other time consuming check.

Does this seem like a good way to control what I've described?
Is there something I should put on the drawing to indicate what I want, such as a note "check profile 3 places approximately 120° apart on inner diameter" or would profile of a surface be a better callout here?
Or, is there a different geometric tolerance that would be more appropriate for this scenario?
Cylindricity was originally proposed, but I believe would be very difficult to inspect appropriately at the machine.

Thank you!

 

[cbrf23]

Just realized in the first shot the ID bore I'm trying to control was not dimensioned.
Here it is with that dimension, not that it really makes a difference to the question.

 

[TheTick]

error

 

[CheckerHater]

Sorry, cannot see the difference between two pictures.

 

[cbrf23]

Just checked and I uploaded the WRONG pictures. Terribly sorry.

@TheTick - what browser are you using? I'm getting an error using chrome (double headers received from server) however the download links work fine with firefox.

CORRECT IMAGE ATTACHED!
Again, very sorry for the confusion.

 

[powerhound]

You need to remove the comma from the file name. You also might need to remove the spaces.

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

 

[ewh]

Corrected image opens fine for me

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[CheckerHater]

Straightness of a line will cover your situation.
Just replace profile symbol with straightness symbol.

 

[pmarc]

1. While profile of a line callouts seem to solve the mismatch issue in areas A<->B and C<->D, nothing on this drawing prevents from mismatch happening in the remaining portions of dia. 2.000 cylinder. As far as I understand, no mismatch in thin wall areas is one of your concerns too.

2. Your profile of a line callouts (with no datum feature references, and for dia. 2.000 being directly toleranced, and not basic) result in exactly the same requirements as straightness of linear elements. Both choices would be correct, but some may find straightness more intuitive, especially when dia. 2.000 is not basic.

3. Why don't you want to leave this explanatory picture on the drawing? I am great fan of using GD&T language wherever possible, but in this case I have a feeling that this additional graphic would make the message much clearer. Put extra note that no mismatch in remaining areas of dia. 2.000 is allowed, and your job is done.

 

[cbrf23]

@Pmarc, to answer your questions:
1. The decided format was to leave a note on the drawing, something along the lines of "No mismatch permissible on ID surfaces outside of A<->B and C<->D".

2. I believe you are correct, they would be effectively the same. We had discussed straightness at one point, but the general feeling was that the profile callout would be less likely to be mis-interpreted on the floor, as opposed to straightness of surface possibly being inspected as straightness of axis or something else.

3. I like the idea of leaving it on there - I had created it for this question only, but I will see if it can be added to the print. Given the required drawing format there may not be enough room, but we will see.

Thanks for taking the time to answer!

@checkerhater, thank you as well! See note 2 above regarding straightness.

 

[CheckerHater]

Whatever works for you.
There is also a strong opinion about profile being only applied to features defined with basic dimensions (see note 2 in pmarc's post)
I guess you will never make everybody happy, so good luck!

 

[cbrf23]

@CheckerHater, I was unaware of any profile biasing - is this specific to certain industries or do you have any idea where this comes from?
Most of our work is done in house, so I dont think there is much to worry about with preconceived biases, however if we do need to farm something out in the future (which on occasion we do) I want to make sure it is easily understood.
Thanks!

 

[CheckerHater]

You can use search feature to find threads like this one:
thread1103-349427
Take a look when you have time. It starts as a discussion of runout, but turns into argument about what profile can and cannot do.
You will see that there are some very strong opinions pro- and contra- using profile without basic dimension.
That was the reason I suggested straightness in the first place - didn't want to start another lengthy discussion.
As you mostly do your work "in house" you should have a chance to polish out misunderstandings anyway.

 

[Belanger]

There is also a strong opinion about profile being only applied to features defined with basic dimensions

I'm not trying to pick a fight, but just to clarify...
I wouldn't say this is an opinion; paragraph 8.2 actually says so. (A straight line is by assumption a basic dim.)

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

 

[CheckerHater]

Para 8.2 is vague enough to support both opinions. It depends on which sentences you pick to put the emphasis on:
First way to support “basic” point of view:
“Profile tolerances are used to define a tolerance zone to control form or combinations of size, form, orientation, and location of a feature(s) relative to a true profile … A true profile is a profile defined by basic radii, basic angular dimensions, basic coordinate dimensions, basic size dimensions, … including design models.”
See? Profile can only be used with basic dimensions. Now, let’s pick the other combination of sentences:
“A true profile is a profile defined by … basic size dimensions … When used as a refinement of size tolerance created by toleranced dimensions, the profile tolerance must be contained within the size limits.”
Suddenly the profile can be used with directly toleranced size dimensions to “refine” them the way straightness or flatness does.
For anybody interested I included the entire Para 8.2. Make your own interpretations!

 

[Belanger]

For the most part, I still have to disagree. Your selective ellipses make it sound like there's an internal conflict within that paragraph when there isn't.

The true profile is what defines the shape, and should always be basic. This is sometimes the same dimension as what defines the size, but not always. So their statement about profile being a refinement of size dimensions only kicks in when the size dimension is not integral to the true profile itself.

For instance, notice in Fig. 8-27 that the true profile is indeed basic (a flat plane where the shape is zero mm). Therefore, the first requirement of para. 8.2 has been satisfied.
Yet the size of 80 mm is not basic. The profile spec is less than the size tol -- which satisfies the other part of 8.2 that you highlighted. IOW, true profile and size are different things being discussed.

The example where I might have to concede is on page 167 of Y14.5. However, that use of a toleranced diameter has been debated here in the past. So the answer to the debate about page 167 may sort of deflate my absolutist statements here.

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

 

[CheckerHater]

cbrf23, do you see what you started?