DIAMETERS SHOWN IN LINE NOT NECESSARILY COAXIAL 2

[KENAT]

Can someone please remind me, in ASME Y14.5 is it basically just 2.7.3 that says that just because diameters are drawn coaxial there is no coaxiality requirement implied. To get coaxiality you need to add controls such as position, runout or concentric (I know, concentric is rarely if ever the right one depending which 'expert' you're talking too).

I get a lot of drawings of parts with 'coaxial' diameters without any controls on the coaxiality.

Do other checkers/peer reviewers etc find the same thing?

Has anyone seen any really good articles or explanations on this I could pass around.

Thanks, Ken


KENAT, probably the least qualified checker you'll ever meet...

 

[ewh]

I find this to be pretty common. If it is imperative that they be coaxial, I will suggest a runout or true position control.

 

[weavedreamer]

How are the holes located? If there is a basic dimension to the c/l, then some geometrical constraint becomes necessary.
A positional tolerance is a good start, of course depending on the functionality of the features involved.

 

[CheckerRon]

The largest, longest, or functionally most important coaxial feature needs to be made a datum--perhaps a 4th datum tied to the 3 main datums--and other coaxial features tied to it by position or runout.

 

[powerhound]

Usually coaxial features are located using a composite tolerance block as in FIG 5-51 and 5-52 in the standard. I suppose there are a few different means to achieve the same end in this case but I always stick to whatever callout is specifically for the circumstance. Start at para. 5.11 and see if any of those example gives you what you are looking for. The answer to your question is that just because features are shown coaxial, if there are no controls that tie them together, any relationship between them should not be assumed. Keep in mind that if each of the holes are located relative to identical datum reference frames and the datum features are not subject to size tolerance, then they are considered a single pattern. See para. 5.3.6.1 for a more detailed explanation.


Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[KENAT]

Thanks all, I'll have to do a little more reading from the suggestions that powerhound gives.

Just to clarify I'm talking all coaxial features both male & female.

In fact it's most common on shafts and the like with a number of nominally coaxial diameters but no relation between the diameters.

KENAT, probably the least qualified checker you'll ever meet...

 

[fcsuper]

In most operations I've seen, it would be very hard to have multi-diameters on the same axis (and side of the part) not be co-axial simply because these normally use one op on a lathe. In those cases, I wouldn't call out any co-axail specifications beyond what is immediately functionally required. To call it out is a bit like saying that your mother's mother is one of two of your grandmothers. However, there's nothing wrong with spelling it out.

Matt
CAD Engineer/ECN Analyst
Silicon Valley, CA
sw.fcsuper.com
Co-moderator of Solidworks Yahoo! Group

 

[ctopher]

If circles are drawn to look coaxial, and have center-lines drawn through the center at 90 deg, they are usually implied to be coaxial. Similar to two line drawn perpendicular, they are implied to be 90 deg.

Chris
SolidWorks 07 4.0/PDMWorks 07
AutoCAD 06
ctopher's home (updated 10-07-07)
ctopher's blog

 

[powerhound]

Chris,
Yes, two lines shown perpendicular on a drawing can be implied 90 degrees but that's because it's a fundamental rule in the ASME standard. There is no such rule to imply coaxiality. The biggest isue you have to contend with is tolerance. Even if it was a safe practice to imply coaxiality, what would the tolerance be? With implied 90 degree rule, it's the tolerance in the tolerance block. Showing two diameters coaxial using only a centerline doesn't give a dimension so the tolerance block cannot be used.

Matt,
You can't assume that just because features are on the same axis and on the same side of the part, that they will be done at the same time. It definitely makes more sense to do it that way but that would be like putting a tolerance of +/-.005 on a feature simply because you knew it would be made on a machine that could hold it even though +/-.5 would have been just fine. You can't assume a shop will do anything you expect that they will do. All you should count on is getting your parts made to the dimensions specified on your print.

KENAT,
I see uncontrolled coaxial diameters all the time. It's frustrating when our QC department rejects a part in which an injector tube is welded 1mm off center yet the print says nothing about how close the injector really needed to be to the center of the burn chamber. It just shows a centerline. Rework of that sort is unnecessary when the rejection is unjustified.

The standard says each dimension must have a tolerance except MAX, MIN, or stock dimensions. Coaxiality is no exception to this fundamental rule. Go back to what KENAT asked in the OP; 2.7.3 specifically states that features shown coaxial MUST be controlled for location or orientation. This means that you can't imply anything in this regard.


Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[dingy2]

I agree with Chris on this one and I would use the standard tolerance shown on the drawing if there was no a feature control frame.

Dave D.

http://www.qmsi.ca

 

[KENAT]

ASME Y14.5M-1994

2.7.3 Relationships Between Individual Features. The limits of size do not control the orientation or location relationship between individual features. Features shown perpendicular, coaxial, or symmetrical to each other must be controlled for location or orientation to avoid incomplete drawing requirements.

fcsuper, ctopher & dingy, I don’t see any ambiguity in what the standard says. Showing them coaxial doesn’t imply anything and while for parts created in a single turning or boring op you’d expect pretty good coaxiality the drawing doesn’t require it from just showing them coaxial. As such if they somehow create parts that aren’t close to coaxial, such that they aren’t fit for use, you have no comeback.

14.5 has a number of suggestions for general notes etc if perfect form at MMC is required but for a lot of the ones I see this is probably tighter than warranted by function.

I just looked at some training notes from Gary Whitmire and he has some explanation. If anyone has any other sources that would be great.


KENAT, probably the least qualified checker you'll ever meet...

 

[powerhound]

Dave,
If there are axes that are shown coaxial using a centerline and there is no control between the two, exactly which tolerance in the standard tolerance block would you use? The one for a three place decimal? How about a two place decimal? If you have an answer please explain the following:

1. How did you determine which tolerance to use?
2. What is the justification for going against what the ASME standard says?

While it is true that there are still some GD&T concepts that are still not completely covered in the standard, this is not one of them. The correct course of action in this case is spelled out. Anything less is..."uncivilized" (who remembers that commercial?)

Powerhound, GDTP T-0419
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[dingy2]

Powerhound:

I agree that 5.11 explains coaxial relationship very well but sometimes it may not be reflected on a drawing. Should we (I am from the Quality background) disregard their location completely? I would not.

Let's day that I saw a drawing that did not have any relationship reflected in a FCF and one feature was "right out to lunch" Visually, it is way out of alignment. I probably would use the tolerance shown in notes section of the drawing to accept or reject the visually out of alignment feature.

If the tolerances were based on the number of digits (rather than unless otherwise noted all other tolerances are +/- **) which one would I use? Well, I would look at the number of digits on the feature and go from there.

I did not see anything in the standard that said that if there was not a FCF on coaxial features, the coaxial features may be located anywhere. It might be there but I couldn't find it.

What section of the standard would I use? Section 1.4 (a) stating "each dimension shall have a tolerance". I would use that for a dimension of location too.

Yes I am stretching everything a bit but I am also trying to use a bit of common sense too.

I know that there are so many areas on a drawing that are not covered by examples in the standard and some that are covered in the standard cannot be confirmed properly and probably should not be in the newer standard.

Let the fun begin - comments?



Dave D.

http://www.qmsi.ca

 

[KENAT]

You want some fun;-)

I did not see anything in the standard that said that if there was not a FCF on coaxial features, the coaxial features may be located anywhere. It might be there but I couldn't find it.

I would have thought 2.7.3 that I typed out in an earlier post essentially says this.

If the drawing for the visibly off part didn't have any controls on the coaxiality then yes, it is to drawing so arguably shouldn't really be rejected.

KENAT, probably the least qualified checker you'll ever meet...

 

[MechEng2005]

While I am not nearly as familiar with GD&T as everybody here seems to be, I will throw my hat in anyways =)

My view would be that if all that is controlling the position is the dimension to the centerline (x & y), then both features of the same centerline will use the x & y position and the tolearance stated in the title block.

X = 2 inch
Y = 4 inch
Tol. = +/- 1/4 inch

Then one feature may be located at X=1.75, Y=3.75
and the other at X=2.25, Y=4.25

Thus, the stated allowable deviation in coaxial is:
(2*(.5^2)^.5 or approx. 0.7071 inches

I hope this adds to the conversation (I have no formal training in GD&T and we don't use it where I work, so the conversation is a little hard to follow sometimes).

-- MechEng2005

 

[dingy2]

Kenat:

Thank you.

Yes you did find something that stated it clearly but it also stated that it "must be controlled for location or orientation to avoid incomplete drawing requirements".

So now I look at a product and 1 of the coaxial features is so far out of alignment that we could consider it a cam. I could say "the drawing is a bit messed up" and accept the product. It's not my problem.

Maybe I would try and get in touch with the Designer. If the Designer said it didn't matter, the product is OK.

I have seen so many drawings with terrible application of GD&T, wrong datums, etc. Sometimes we try to figure out what the Designer wants rather than what they have on the drawing. Is that wrong?

What would you people here do if i coaxial diameter is so far out that it is a cam and there wasn't a FCF controlling the location of the features? Let it go?

Let's get some thoughts here. This is real life stuff that happens all the time on the shop floor.

Help me out here.

Dave D.

http://www.qmsi.ca

 

[ewh]

Dave brings up a valuable point. While legally a "cammed" feature may meet the drawing requirements, we have to keep in mind what the customer really needs. To maintain a good relationship, we should strive to give the customer at least what he needs, and more where we can. Many drawings may be vague and incomplete, but if the purpose of the part is understood we can add value to our product by meeting those needs, even when the drawing information given is lacking.
Granted, things could be much easier if everything was clearly spelled out, but this is the real world, and customer satisfaction is very important.

 

[vc66]

dingy2,
I definitely don't think it's wrong that you're trying to help out the designer, but I believe there is some necessity in explaining why things are incorrect.

My feeling is that the standard is pretty clear. The problem arises when the callout (or lack thereof), affects form, fit, or function. If this is the case than the part needs to be rejected, and the designer needs to be told why. If the incorrect part does not affect any of these three, then it should be dispositioned UAI. In this case, however, the designer should still be told that this is bad practice.

My .02 cents.

V

Mechanical Engineer
"When I am working on a problem, I do not think of beauty, but when I've finished, if the solution is not beautiful, I know it is wrong."

- R. Buckminster Fuller

 

[KENAT]

"Sometimes we try to figure out what the Designer wants rather than what they have on the drawing. Is that wrong?"

There would be an argument that the machine shops etc. shouldn't have accepted the job, and certainly shouldn’t have made the part, without first asking for clarification of the drawing; or at least letting the customer know their assumptions. Trying to guess what someone meant is fraught with potential errors. Shops that accept ambiguous drawings and so have to do this are arguably perpetuating the problem of unclear drawings. The designers get away with it so many times they never learn different.

For this specific case you could perhaps cover yourselves by adding something to your standard terms stating something like “For diameters shown co-axial but with no explicit drawing requirement perfect orientation at maximum material condition with regard to related features will be assumed” however this may have a cost impact.

If the parts already made and is visibly bad I’d maybe inform the designer/customer that the part as made is eccentric to X inch, that the drawing gives no requirement for coaxiality and ask them to disposition the part. If they say the part is scrap it would then be up to you/your organization to decide if you eat the cost in the name of customer relations or charge the customer.

I should make it clear that my OP is from the point of view of drawing checker, trying to avoid this problem in the first place by teaching the designers better and enforcing adherence to drawing conventions/standards.

In my checking role I have to try and figure out what the designers trying to say a lot, of course I can almost always easily talk to the designer but I have some feeling for the problem. I've also had to look at old drawings for which the designer is long gone and they are often ambiguous, in this case I often have to guess just like you if I can’t determine it based on function.

I thought one of the major points of drawing standards was to avoid such ambiguities.


KENAT, probably the least qualified checker you'll ever meet...

 

[ewh]

Yes, KENAT, that is the purpose of the standards. That is why your job is so important. My last post was addressed more to those who have no control over the drawings they have to use, but I agree with you 100% that ambiguity has no place on a proper drawing.