what is best way to control location of coaxial hole

[bxbzq]

On drawing I need to drill a multi-stepped hole on a thick wall. There are say 6 coaxial diameters on the hole. What is the best callout to control the location of the diameters with positional tolerance control?

1. Use positional tolerance control for each diameter with same datum features reference. I think this would make the drawing kind of verbose. Is there a better way?

2. I see drawings drafted by my colleague show a single positional tolerance control applied to the axis of the hole. I guess the control of this callout is equal to the first one. But I'm not sure if it is an appropriate way because it just reminds me of the datum symbol placed on an axis.

3. Use a composite position tolerance control with a notation like 6 COAXIAL DIMATERS. This is a nice one but there are fewer people understand exactly what it means. Besides, the design intent, I guess, is not to control the coaxiality of the diameters. It just wants to control the location of each diameter individually.

Thank you for inputs.

 

[pmarc]

bxbzq,
If the intent is to control location of each bore individually relative to external datum features, I see the approach from your option #1 as the best one, with a modification though - if the position error allowable is the same for each bore, you can use method shown in fig. 7.24 of Y14.5-2009. However if those values are different, 7-25 is a way to go, so something similar to your proposal.

 

[pmarc]

bxbzq,
If the intent is to control location of each bore individually relative to external datum features, I see the approach from your option #1 as the best one, with a modification though - if the position error allowable is the same for each bore, you can use method shown in fig. 7-24 of Y14.5-2009. However if those values are different, 7-25 is a way to go, so something similar to your proposal.

 

[CheckerHater]

bxbzq
Stay away from "option 2". You are absolutely right, it IS similar to applying datum to axis. Just take a look at the drawing and ask yourself: is the axis derived from DIA2? DIA2? DIA3? Combination of DIA1 and DIA6?
One should always control feature. It could be surface of the feature or axis/center plane derived in unambiguous way.

 

[fsincox]

Is this ISO? Are you using ISO general tolerances?
Frank

 

[bxbzq]

pmarc,
In my case the hole is not exactly a counterbored hole. See attached. I think the approach you recommend still applies, right?

CheckerHater,
I guess the argument from my colleague would be: I understand the problem of applying datum to common axis because datum has to be established from a feature unambiguously. But in this case, since I want all the diameters to be located in a common tolerance zone centered around the common axis. Why bother to specify them individually? A single positional callout serves the purpose fairly well.
I'm not comfortable with the single positional callout, I just don't have a strong logic to argue back.

Frank,
Yes, the print invokes ISO. But the department who drafted the drawing is in process switching from asme to iso. I assume the drafter is very asme guy. Any difference between asme and iso here?

 

[fsincox]

You really set this up when you say "the best way", the best way is to specify all the tolerances (your choice 1) per each functional requirement ISO or ASME.
Does everyone do it? No! Just like the other people you see!

Yes, not only are there are differences but ISO standard tolerancing, in particular, gives you another option of using as system of general tolerances to cover coaxiality on the less critical features and state only the ones that are not acceptable under the general tolerance values. (ISO 2768-1 & -2)
You can use a general note to do it under ASME but the ISO system is much more sophisticated.
Frank

 

[dgallup]

It still makes a difference which bore(s) you use to establish the datum. It is entirely possible for the same part to pass based on one datum definition and fail based on another. You as the designer know the function of the part and need to communicate that to the people making and inspecting the part.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

 

[pmarc]

bxbzq,
You are not showing which features are datum features. Like I said, if the intent is to control location of all the holes independently relative to some "external" datum features (and not relative to one of the holes in the group), I sustain my initial recommendation - use Position callout for each of the holes. The only thing which I would think about a little bit is the longest, interrupted hole that could be somehow treated as a continuous feature (even in ISO GD&T).

Frank,
Please do not make this more confusing. There is no option in ISO 2768-2:1989 to assign general geometrical tolerances for Coaxiality or Position. The standard does not include those two characteristics.

However I confirm that there are differences in interpretation of Position between ASME and ISO. If the print ivokes ISO, one can/should even use Concentricity to control axes offset. ISO's Concentricity is a special case of ISO's Position intended to be used for cylindrical features shown nominally coaxial. ASME's Concentricity is something completely different to ASME's Position though.

 

[fsincox]

Pmarc,
Circular runout controls coaxiality! I am not sure who is confused?
ISO 2768-2 5.2.5 Coaxiality (NOTE.....)
People use runout to control coaxiality under ASME too. I am not a big runout fan myself but..
Frank

 

[CheckerHater]

bxbzq,

I was under impression you are looking not just for the best callout to control the location of the diameters, but also for standard way to do so.
The standard way to do things is not always the obvious or easy-looking one.
For example, the drawing you supplied shows 7 coaxial features, not 6.
But if "why bother" is valid argument, then... why bother?

Frank,

I am bigger fan of runout than you, but even I would limit it to shafts, not holes.

 

[fsincox]

I think we will all agree on the "best way", safe?
Frank

 

[KENAT]

So long as it is justified by function I don't see the problem with approach 2 - it is what is done with counterbores & countersinks most of the time. (Section 5.7 a of ASME Y14.5M-1994 & figure 5-37).

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[fsincox]

CH,
How process oriented of you. Do you have any ISO standard based reference for that, or, is it just a personal preference?
Frank

 

[CheckerHater]

Frank,

I stand corrected: not necessarily a shaft, but at least something you can stick into chuck and turn around.
Yes it is personal preference, and yes it is process-oriented. There was a discussion on this forum if runout could be measured on CMM. Everyone decided to stay away from that, so let's just keep it this way for now.
And if you think of it, isn't the entire concept of GD&T process-oriented? Otherwise we wouldn't have Y14.43, would we?

 

[Belanger]

Real-world example: circular runout is used all the time to control the wobble effect of the ID in a washing machine tub. Does that count as a "hole"?

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

http://www.gdtseminars.com

 

[fsincox]

CH,
I would say no. That is one of the battles in the ASME standard it self, its Foreword and introduction try to divorce itself from process however processes like runout seem to invalidate that. I have always felt you just need to believe it would pass if you could rotate it and a particular process was not required. Naturally, I would say that but it is the only way I can make it consistant with its own stated goal.
Frank

 

[fsincox]

I look at this the same way as I look at any suface callout requirement, do you really have to check every point on a surface? I do not feel you must, you just have to check enough points to establish a reasonable belief that if you could check every point it would pass.
Frank

 

[bxbzq]

Thank you all for the inputs. Sorry the question was not described clearly.
I was lazy and just copied part of the view from the drawing and datums are not shown in that view. The hole is drilled on the wall of a cylinder-like part. Datums are axis of cylinder and surface of flange at one end. CH is right, there are 7 diameters. I missed a very short one.
I like the way shown in fig. 7-24 in 09' and fig. 5-37 in 94' for counterbored hole. But in this case, the 2 bores sitting at both sides of the interrupt have different diameters. So probably I have to specify positioanl tolerance for each bore in this cross section view.

 

[bxbzq]

KENAT,
Do you think the approach 2 (see attached sketch) is same as what shows in the fig. 5-37 of 94' Standard?