Implied Concentricity tolerance on coaxial diameters???

[BlaineW]

My question regards a shaft with a through bore and several steps of diameters on the OD, two of which are bearing surfaces. I am a fairly young engineer and somewhat new to GMT, and I'm dealing with a lot of old prints made back in the 80's and 90's. Most of them only contain size tolerances for the OD's and no relationship between any of the diameters. I have been trying to find out if there is any sort of default tolerance implied by diameters on the same axis or if they could in theory be misaligned .050" and still be ok "to print" as long as they meet the size requirements(approx. .0007"). Could anyone reference me to any standard that clarifies this?

I intend to designate a circular runout on the bearing surface diameters, but that doesn't take care of the other diameters which aren't as critical(.006" size tolerance)...is it necessary to specify the runout of each of these individual dia's or does the size in any way control the position relative to one another?

The only reference I have for something similar is the implied 90 degree angle that defaults to the title block angular tolerance, but I can't find anything similar for diameters on the same axis.

Thanks,

Blaine Williams
Manufacturing Engineer

 

[dingy2]

There is nothing implied in ASME Y 14.5M - 94 on a on a feature to feature relationship.

If you want it, place either circular or total runout on the feature where a relationship is needed. If it is not important or there really isn't a relationship, please do not place GD & T on the feature.

Too many engineers place GD & T on features that have no function or relationshiop driving up the cost.

Dave D.

http://www.qmsi.ca

 

[KENAT]

On the other hand, if you do need it don't be afraid to use it.

You don't have to have a particularly tight tolerance just because you are using GD & T. The tolerance value should be driven by function/tolerance analysis.

On the other hand if you are using shops that don't understand GD & T then pretty much any you put on, even if it actually relaxes tolerances compared to non GD & T dimension scheme, then the price will likely to up.

 

[KENAT]

That's go up.

 

[Tunalover]

An old dilemma indeed!
The "old way" of controlling the coaxiality of concentric features is to write an awkward note. The other way is to not provide a note at all; it is implied that the features are coaxial. Either method provides the same result.
The "Y14.5M way" is to create a local datum on one of the diameters and call out the coaxial diameters relative to that one using positional tolerance feature control frames(of course providing the same result as the first two methods).
Many machine shops will charge more for the second and third methods even though the results are identical for all three!



Tunalover

 

[CheckerRon]

If you don't control the other diameters relative to your bearing diameters, just how eccentric can they be? I don't buy all this "Oh Gee, they will up the price" scare. If an outside shop doesn't know how to handle it, get a new shop. I it is your own shop, educate them. With a shaft with two opposed bearing diameters on it. Specify the longest bearing dia as datum A, specify the other with a runout or position tolerance relative to datum A (probably .001 or so based on the tolerances you note)and call the second bearing diameter Datum B. now specify the rest of the diameters, including the bore runout or position relative to datum A-B. make the non-cricial diameters looser, but consider balancing problems too, in doing so. By the way, it is GD&T. GMT is time.

 

[ctopher]

I agree Ron.
I thought GMT was the inspector's initials.

Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 10-27-06)

 

[KENAT]

I didn't mean to imply you shouldn't use the GD&T, I just wanted to highlight the problem so the OP didn't get an unpleasent surprise.

The corrective actions of either training or finding a new supplier would be my preference.

 

[CheckerRon]

That brings me to my two favorite phrases.
"People don't do what you expect, they do what you inspect."
And this one regarding "hard dimensions vs. centerline dimensions. "Dimension for inspection---let the machinist determine his own centerlines.

 

[BlaineW]

Thank you for all the replies, and yes I did mean GD&T not GMT, so much for proofreading We make the parts in house, so as much as I'd like to sometimes, I can't find a new supplier hah!

This whole thing came up because our QC department was trying to reject parts and was asking that a tolerance be added to the print arguing that it had to be held to something.

I was struggling with finding a balance between overcomplicating the part and not giving too much leeway to our machinists in making it. As I said I intend to restrict the bearing surfaces with a runout, but I think I'd rather leave the rest of it alone and trust that common sense will keep it reasonable, as it is not critical to the function of the part. I just wanted to make sure there was no "unwritten rule" that I couldn't find that might satisfy everyone.

Thanks again

 

[KENAT]

Just FYI, on a number of parts lately I've still put a positional or runout on what could be considered non critical 'coaxial' diameters.

I've used a pretty loose tolerance value that should be very easy to meet but it's still there just incase anyone gets any funny ideas.

 

[CheckerRon]

I agree with KENAT. Exactly what I was saying in my post. Showing turned diameters of the same centerline with no geometric relationship specified somewhere on the drawing means no concentric or axial control.

 

[MikeHalloran]

Guess what: o-ring grooves with a finish to spec, corner radii to spec, held to .002 diameter, but eccentric to the surrounding diameter by .020, leak rather badly.

Yell at the supplier about the parts not conforming, he replies, "... not conforming, to _what_ dimension?"

So much for implied tolerances.

The parts were PVC, which moves around some, but I still have no idea how he managed to make them so badly. I had a lot of time to contemplate the question; I had to buy the lot.



Mike Halloran
Pembroke Pines, FL, USA

 

[MechNorth]

Use the GD&T! On ALL features? YES!!! Even for a general tolerance. Everything needs to be tied back to your datum system or you WILL get crap, and you WILL have to pay for it. GD&T is Geometric Dimensioning & Tolerancing, NOT Geometrically Tightened Dimensioning & Confusing Tolerancing To Increase Costs. If something is not very critical, OPEN the tolerance. If something is very critical, TIGHTEN the tolerance and look at some extra controls. As mentioned above, you WILL care about warpage, eccentricity, flatness, roundness, and a host of other qualities that you ASSUME will be built into your part by a competent machinist. The reality is that when a court sees that something is not controlled, the supplier cannot be held liable for what the client "assumed" would be done. It's been established in numerous court cases.

Blaine, GET SOME GD&T TRAINING; it's good that you know enough to ask for help, but it's a steep learning curve and you'll only get there by training. There are a number of earlier posts on this site that give good references to numerous training suppliers...some are even members of this forum. Good luck on the tough treck ahead.

Jim Sykes, P.Eng, GDTP-S
Profile Services
CAD-Documentation-GD&T-Product Development

http://www.profileservices.ca