Goal R.002 *Pulls hair out!* 5

[ModulusCT]

OK, so I was told to do the following by my supervisor today. I really hate having to tell him that he has no idea what he's doing and that he doesn't know the applicable drafting standard, so I thought that it would be better to simply offer a solution that does jive with the spec.

He wants to indicate R.002 +.003/-.000, but with an emphasis on trying to produce the radius at .002 rather than taking the total permissible error and shooting for the middle. His solution to this problem is to say .005 MAX; GOAL R.002, but I hate this personally because the word GOAL is not mentioned in the spec as an acceptable descriptor for tolerancing a part. In fact, I'm pretty sure there are parts of the spec that say not to do things like this.

Any suggestions? Is there a way that you can say, what my boss wants the drawing to say by using acceptable symbology and terminology?

 

[KENAT]

What is the real requirement?

Is there a reason for .002 to be the minimum? I mean, .002 isn't much of stress relief and while it may help the tool it's not clear why .001 is unacceptable.

.005 MAX sounds most appropriate from what you say.

If the toll is R.002 +.003/-.000 then you're already saying you'll except up to .005. If .005 isn't acceptable adjust the tolerances.

The tolerances define the limit, I know of no correct way to imply on a drawing that you have a preference for one end of the limit.

Posting guidelines faq731-376

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

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

 

[ModulusCT]

Thanks for the quick reply KENAT... I agree with you. This is just silly to me.

This is a lid for an enclosure I'm working on... The radius could absolutely be .001, so a better solution I think would be to say .002±.001. To state an allowable tolerance and then indicate somehow that you'd prefer it if they didn't use it seems laughable to me. Actually, I'm laughing right now!

Thanks again for the reply.

 

[CheckerHater]

To be standard-compliant you have to "hide" reference to the process.
One possible way is to create separate document - Control process, where to describe statistical requirements - how many parts will be accepted for which tolerance range.
Then you mark your dimension with <ST> and reference to said document.
This way you have clean drawings combined with unlimited number of requirements.
I am not an expert on statistical tolerancing and I am sure it is not very well standardized yet. Hope someone can describe it better way.
Also not sure radius is important enough to justify the technique.

 

[ewh]

I agree with KENAT... you are already specifying the goal, and are including an acceptable tolerance. ALL dimensions are merely goals (as nothing is perfect). The work "GOAL" adds nothing to the correct interpretation of the dimension.
Checkerhater also had an good suggestion, but I agree with him that it may be overkill for this one example.

Technically, the glass is always full.

 

[ModulusCT]

Thanks guys...

@ ewh: The problem is somewhat unique. At least the way the powers that be where I work see it. They are saying that .005 is permissible, but that the lower the value the better; so preferably, .002. Their fear is that, if we say .002+.003/-.000, the machinist will shoot for .0035 thereby giving himself the most leeway above and below the nominal value, which I think is a valid concern. It's a situation where they're essentially trying to trick the machinist into producing the part how they want, which is pretty dumb I think.

.002±.001 is not possible according to the manufacturer. They are using a chemical etching process to make the radii and can't control the size that stringently I guess.

I'm irritated because my boss and nearly every other person in my group follows the drafting standard willy-nilly and I try to be as dead accurate as possible. When I'm asked to do things that I know deviate from the spec, which I've studied for at least 12 years now, I feel like walking out! haha (I need the job though)

Anyway, I think I've convinced everyone to go with .002 +.003/-.002, which puts their target of .002 nearly in the center of the tolerance zone and still complies with all applicable specs and standards.

I work at one of those places where GD&T is seen as a bother and no one really knows what to do with it (except me of course). There is a lot of ignorance floating around here and it drives me nuts from time to time. My only ray of hope is the engineering VP who has told me in the past that if I can show him how strictly following Y14.5M and implementing GD&T can improve our product that he'll back me up.

 

[powerhound]

This is why I think there is such a thing as unilateral tolerances. Specifying a R.002 +.003/-.000 is exactly how you communicate the goal that you want a .002 radius but error of +.003 is tolerable. If the goal was R.0035 +/-.0015 then it should be shown that way.

This is what I believe.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[ModulusCT]

@powerhound: Do you think that most machinists agree with you? At the end of the day, all that matters to most people is that the part comes in the way they want, and so, creating a drawing for the machinist and taking into account his motivations is applicable.

 

[Belanger]

Powerhound is right. Saying R.002 +.003/-.000 is (supposed to be) different than R .005 MAX.

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

http://www.gdtseminars.com

 

[powerhound]

Most machinists in my neck of the woods agree with me. I've been a machinist for 23 years and everywhere I've worked, that has been how a callout like that is understood. I can't speak for the rest of the country but around here, that's how it is.

I agree that what matters is whether the parts meet spec or not, regardless of what the GOAL is; however, there are ways for the designer to communicate that he prefers a dimension be closer to one end of the tolerance band than the other, and this is one way to do it. A general note is another.

What matters to the machinist is not always what matters to the designer. Do you believe R.002 +.003/-.000 communicates exactly the same thing as R.0035 +/-.0015?

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[MechNorth]

The unilateral tolerance is the most likely way to get the point across, however ... CNC operations will work to the nominal geometry (whatever it was modelled at), an inexperienced machinist (or programmer) may well go for median. Many experienced machinists will go for median as well, to minimize manufacturing time and ensure it is within range.

If it is somehow essential to functionality that the part(s) be fabricated at the one limit, then a non-Normal distribution is needed.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[powerhound]

I've learned a lot of things over the years but a couple of the most important lessons I've learned are:

1. Never assume you know how a part will be made. Just because it's round doesn't mean it will definitely be made on a lathe and just because diameters are co-axial doesn't mean they'll be made in the same set-up.
2. Never assume you know what a machinist will think or do. The most experienced ones can poop you out a good part before you can even guess what stock size they'll start with.

Just put your requirements on the drawing and let them figure out how to do it. I guess you have a way to tell the difference between a .002 radius and a .005 radius.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[ajack1]

Given the information from the OP I would say the process is the problem not the way it is dimensioned.

They state that .002 +/- .001 is not achievable but that .002 to .005 is, which however you dress it up is +/- .0015 so that extra half a thou must make all the difference.

Therefore to produce parts that are within limit the only way they can go is to aim for .0035 and even then some parts will be smack on bottom limit and some smack on top.

If that is not acceptable you need to find another process or another supplier who can hold tighter limits.

 

[Walterke]

Many experienced machinists will go for median as well, to minimize manufacturing time and ensure it is within range.

How else would you do it? It seems to me that this is the best way to meet the demanded requirements...

The .005 is either allowed or it isn't (unless, as said before, a statistical tolerance is included). If it's not allowed, they should change the tolerance.

NX 7.5
Teamcenter 8

 

[MechNorth]

Walterke,
Experienced machinists, particularly those with manual experience, will work to the least material removal size; it allows them to rework things if needed and reduces cutting time. It was the basis of the old "hole & shaft" system, which is still the basis of limits & fits tolerancing.
NC programmers, working from a CAD model, machine to the nominal (CAD) size for the most part, without checking on the tolerances other than to make sure that the machine & tools are capable; they don't typically catch or compensate for a skewed / unilateral tolerance.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[powerhound]

Lets look at a different scenario. Maybe using an example with a wider tolerance range will better illustrate my point.

If a shaft is toleranced at 25mm 0/-1 should one, as a matter of standard procedure, automatically strive to produce a 24.5mm part? Clearly the part will be in tolerance and will be accepted, but if 24.5 +/-0.5 was what the designer preferred then wouldn't that be the tolerancing format?

Drawings and GD&T are used to communicate design intent. If every unilateral tolerance is automatically adjusted to be bi-lateral then one is ignoring what the designer is trying to communicate.

To be clear: I am not saying splitting the range is wrong, it just ignores a form of communication by the designer.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X5
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[MechNorth]

PH, once the drawing leaves the engineering group, manufacturing economics come into play, and that's where such decisions are made unless they are specifically told otherwise. Personally, I don't believe in unilateral tolerances because they increase the probability that half the parts will be out of spec based on a normal-distribution manufacturing process.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[CheckerHater]

I am a big fan of unilateral (even unequal bilateral) tolerances but only as a way to indicate preferred fits for the purpose of harmonizing the tooling.
I believe that GO/NO GO gage for DIA 25h11 should quote cheaper than DIA .98169+/-.00256.
Otherwise tolerance is just what it is - the tolerance. As long as measurement falls wthin the range, the part is good.
Also, splitting the range in half and using median value is common practice in tolerance stack-up calculation. So I don't think there is any "assumed" interpretation for any kind of tolerance. (except statistical)

 

[Belanger]

If you're a football team, do you care only that the kicker gets the ball through the uprights, or do you care about how close to the target he kicks each time?

Of course, it's the second one you're after. So bilateral vs. unilateral is more than just window dressing.

I, for some function reason, I want the target shifted off center a little, wouldn't my "targeting" kicker be more in line with the overall objective?

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

http://www.gdtseminars.com

 

[MintJulep]

The nominal dimension defines the perfect part. Seems pretty clear that the nominal should be the "goal".

Tolerances define the allowed variation from the nominal that the design can tolerate and still work correctly.

If your design cannot tolerate a part that has dimensions within tolerance then the tolerances are wrong.

R.002 +.003/-.000 perfectly communicates that you want a radius of .002, but will accept anything from a sharp corner to R .005.