Hole position w/ concentric radius

[twkinfected]

Looking for a little help on this one. We are making a part that is an oval and has three holes lined horizontal, the two outer holes are the same Ø and the middle hole is slightly larger. The two outer holes are toleranced 21±.4 center to center from the larger middle hole to the smaller outer holes. The two outside holes have concentric corner fillets that make up the profile of the part. The only other dimensions on the print are the hole sizes and the radius of the oval to constrain the profile. There is no profile tolerance listed on the print. We laser cut the outside oval profile and the larger middle hole, and then CNC milled the two outside smaller holes. The center to center distance of the smaller holes to the larger hole is within tolerance, but the distance from the larger middle hole to the outside tangent point of the what should be concentric radii is not, the part was not located properly during setup. My question is, since the outside radii should be concentric with the two outside holes, do the center of the radii share the same ±.4 tolerance as the holes? There is no profile tolerance as previously stated. Does the tolerance of the radii (±.4 also) have any affect on this?

Travis K.
Mechanical Eng.

 

[twkinfected]

EDIT: added a screen shot to clarify question.

 

[axym]

One could argue that the 21 +/- 0.4 tolerance applies to the center of the radii just as much as it applies to the center of the small hole. The tolerance of the radii does affect the tolerance on the 36 dimension, I would say. So the 36 dimension would have a tolerance of +/- 0.8.

Directly toleranced dimensions can get very ambiguous when applied to parts with nominally symmetric or coaxial features. It is not clear as to exactly which features the 21 dimension even applies to. It is also not clear exactly how coaxial and symmetric the features need to be. Parts like this are the reason we have GD&T. The directly toleranced dimensions are a guessing game when applied to a real part - there will be multiple interpretations.

Sorry to not be more helpful.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[dgallup]

I agree the stackup on the (36) is +/-.8. However, it is not a controlling dimension on the drawing so I would not measure it.

 

[dingy2]

The dimension question is really a reference dimension (21) and should not be confirmed. The Designer could have controlled the overall distance from the centre if that was required.

Evan stated "Parts like this are the reason we have GD&T." I might not totally agree with that statement since I believe that GD&T is applied to reflect the "function and mating relationship" of the part. One would need to understand the mating relationship of this part before applying any GD&T.

Dave D.

http://www.qmsi.ca

 

[KENAT]

Yep, that's a fairly lousy/incomplete dimensioning scheme, at least from my understanding of ASME Y14.5M-1994.

"since the outside radii should be concentric with the two outside holes"

Actually, nothing I see in your sketch explicitly states this. The nominal centers appear to be at the same location but beyond the +-.4 tolerance horizontally there is no other tolerance tying them to each other.

A principle of ASME Y14.5M-1994 (ASME Y14.5M-1994 2.7.3 I think) is that just showing things nominally aligned does not imply any tolerance on just how aligned they are. You need to explicitly give a requirement.

Posting guidelines faq731-376

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

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

 

[PeterStock]

I am thinking that an implied 0.000 dimension could apply to the distance between the outer holes and the center of the radius, adding the default tolerance on a linear dimension to the sum of the other two dimensions. As there is some confusion in interpetation, if I was doing the drawing, I would to a profile tolerance on the outside of the part.

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services

http://www.infotechpr.net

 

[drawoh]

twkinfected,

Your drawing shows a major advantage of positional and profile tolerances. You want apply the tolerance to the feature, not to an ambiguous dimension.

My official interpretation of the drawing would be that both the hole and the radius are controlled by the ±0.4 tolerance. The effective tolerance of your 36mm dimension would be ±0.4 + ±0.4 = ±0.8mm.

You have no dimensions or feature control frames controlling concentricity. This is another advantage of GD&T. You could make a very strict legal argument to the effect that this was not specified, as long as you do not mind not getting any more business from your customer.

This really is not a drafting problem. The problem is understanding what you can ship to your customer, with some expectation of repeat business. Are you willing to put your name on this stuff? Can you call your customer and ask them if it is okay?

JHG

 

[ewh]

I would include centerlines for the radii and a radial dimension which would originate at the center point. The intent should be quite clear.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[twkinfected]

Thank you everyone so far for your input.

Drawoh,

As much as I would love to call up this customer and have them change their prints, they make up 90% of our business so the risk I run when pointing out problems like this is very high. This is also a global company, this particular part originating in Japan, which makes the barriers between American manufacturing and Japanese manufacturing incredibly difficult to work around. This part also requires a PPAP, and all the fun stuf that goes along with that, so changing a print is an incredibly long process, probably not worth the time or the money to roll another print change on a question such as mine.

If anyone is familar with AIAG requirements, are suppliers allowed to make changes to shop drawings as long as the part meets supplied print? We are required to submit a numbered drawing and dimensional report, do added dimensions have any effect on this?

Travis K.

 

[dingy2]

You certainly can have in-process drawings that meet the customer's requirement but the drawing used for your sample submission will have to be the customer's drawing with all dimensions numbered.

Dave D.

http://www.qmsi.ca

 

[drawoh]

As much as I would love to call up this customer and have them change their prints, they make up 90% of our business so the risk I run when pointing out problems like this is very high. ...

Definitely, this not a drafting problem.

Are you willing to face the consequences of shipping your parts, as is. I would think a customer to makes up 90% of your business should get special treatment.

JHG

 

[dgallup]

For a PPAP you only measure the dimensions of the customer print. If they are all good you have met the drawing requirements. You are not required to meet dimensions that are not on the print. You will have fulfilled your contractual obligations. You may not get repeat business.

 

[gadkinsj]

I am an engineer in a "global" company. I feel that if my name is on the print and there is some question as to what my intention is, I very much appreciate a call from the fabricator for clarification. When i get that call, I answer the question then follow up with a rev'd drawing. Its best for me to clear up the ambiguity before the next guy who doesn't even care makes the part.
If there is a part I designed that ends up in India and we have a problem with it. Our policy is to ship me out to figure it out. and I don't like the food. So if there is a question ask away.