×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Goal R.002 *Pulls hair out!*
5

Goal R.002 *Pulls hair out!*

Goal R.002 *Pulls hair out!*

(OP)
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?

RE: Goal R.002 *Pulls hair out!*

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: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: Goal R.002 *Pulls hair out!*

(OP)
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.

RE: Goal R.002 *Pulls hair out!*

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.  smile
 

RE: Goal R.002 *Pulls hair out!*

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.

RE: Goal R.002 *Pulls hair out!*

(OP)
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.

RE: Goal R.002 *Pulls hair out!*

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

RE: Goal R.002 *Pulls hair out!*

(OP)
@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.

RE: Goal R.002 *Pulls hair out!*

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

RE: Goal R.002 *Pulls hair out!*

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

RE: Goal R.002 *Pulls hair out!*

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  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

RE: Goal R.002 *Pulls hair out!*

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

RE: Goal R.002 *Pulls hair out!*

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.
 

RE: Goal R.002 *Pulls hair out!*

Quote (MechNorth):

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

RE: Goal R.002 *Pulls hair out!*

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  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

RE: Goal R.002 *Pulls hair out!*

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

RE: Goal R.002 *Pulls hair out!*

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  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

RE: Goal R.002 *Pulls hair out!*

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)
 

RE: Goal R.002 *Pulls hair out!*

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

RE: Goal R.002 *Pulls hair out!*

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.

RE: Goal R.002 *Pulls hair out!*

I think we are starting to go into the weeds with this.
While this forum does address GD&T and tolerance analysis, this issue seems to be merely one of drafting standards and interpretation.  It can be argued until the cows come home as to the best way to achieve what the OP's management is asking for, but that is beyond the purpose of the drawing.
Bottom line is that dimension = target (not suggested target).  Of course, no (non-basic) dimension can be perfect.  Tolerance = acceptable variation from target.  As noted, fabricators often juggle the allowable tolerance to ease their task and increase productivity, and without further direction this is an efficient method and is acceptable to do so.  Such a drawing as this IS NOT the place to provide that direction, as its purpose is to provide part definition, not process.  Adding terms such as "GOAL" is redundant and only serves to clutter the drawing.  The line is then crossed to start adding more terms that may be irrelevant to the part definition, such as REAM, BORE, TAP, etc which should only be used if it is critical to part function.  The presence of the tolerance seems to negate the criticality of "GOAL".  If the target dimension is not the goal, then then a dimension range should be used instead.  Issues such as the OP's are production issues, not definition, and should be addressed in other production documentation, such as a work instruction, using statistical control or other methods, but not on the defining drawing.  If there are still problems, then the tolerance is wrong, or some training needs to be given.  Ignorance of simple drawing interpretation per whatever standard used needs to be addressed.

On the other hand, if management chooses not to follow a standard, you're on your own.

Technically, the glass is always  full.

RE: Goal R.002 *Pulls hair out!*

My apologies... a couple of posts snuck in before mine which make very similar points.

Technically, the glass is always  full.

RE: Goal R.002 *Pulls hair out!*

J-P,
You're assuming that the high-school football team has the ability to track the start point, kicker's capabilities, end point, calculate the trajectory, force and velocity.  Unfortunately only a few colleges & the NFL have those abilities.  The reality for everyone else is ... get it thru the uprights, or it doesn't count.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

RE: Goal R.002 *Pulls hair out!*

Well, running a professional manufacturing company should involve some sort of consideration of capability, shouldn't it? Quite different than a high school team where all players are given playing time.  (Obviously I was referring to a football team at a higher level.)

Bottom line in all this: Though all parts within a given range are acceptable, the designer is still trying to communicate something by assigning a unilateral or unequal bilateral tolerance.  

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Goal R.002 *Pulls hair out!*

I don't disagree with the second statement, J-P.  The problem is effectiveness of communication.  I would usually visit the Process Planner and the individual machinist to get the point across.

As for the first point, "should" is the operative word there.  Reality is vastly different, and most companies of small-to-moderate size don't play on the same technology field as the big boys.  Most companies just try to do their best (i.e. "tightest") processes and check the parts for acceptance.  It's a gross waste of money because companies are wasting huge amounts of personnel and machine resources where they don't have to.  Not terribly different from a company that bids on a project with GD&T on the drawings, but has never done it before; they crank up the price and just do their best without knowing what it all really means ... praying they get it right.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

RE: Goal R.002 *Pulls hair out!*

I don't think it is an effectiveness of communication issue so much as it is an inability to understand the different methods of tolerancing a dimension.  You shouldn't need new procedures or processes to train someone in correct dimension interpretation.
Bi-lateral (targeted but variance allowed), unilateral (targeted but variance allowed), geometric (targeted but variance allowed) or range (general - don't care where the final dimension ends up as long as it is within the range); the OP's issue is covered once those four types of tolerancing are understood.  Creating new procedures or processes to redefine such practices will only unnecessarily complicate things, and that will snowball as time goes by.  Technology is great, but I still stand by Training and KISS first.
I truly appreciate the knowledge being shared in this forum, but more and more often it seems that theory is over-riding practicality.  This is understandable when new principals are introduced or refined, but the OPs issue is cut and dried dimension interpretation.  You can discuss theory all day and still not completely agree, but sometimes drawings actually need to get to the floor.

Technically, the glass is always  full.

RE: Goal R.002 *Pulls hair out!*

(OP)
"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: That's the concern. I don't know if it's well founded. In your opinion it is not, but the problem is convincing my boss of that fact.

"I guess you have a way to tell the difference between a .002 radius and a .005 radius."

Nope! We don't inspect our parts /facepalm. We operate with a policy where we trust our manufacturers to give us good parts. We only do what's called a first article inspection, which means that we measure the assembled end product, not its constituent parts.


"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."

@ajack1: Well, that's just what my dept. head told me... He probably doesn't know himself. That's a good point though. It's unfortunate that I've got to deal with all of this silliness, but there are a lot of sensitive egos where I work I guess.

"On the other hand, if management chooses not to follow a standard, you're on your own."

@EWH: Yeah, we're 'soft ANSI', which means that our drawings do not say 'interpret per ASME Y14.5M'. We're supposed to make our drawings to the spec, but our (micro)managers reserve the right to do whatever the hell they want with it. Therefore, no one really knows or cares what the spec says at the end of the day. Hence, my grey hairs.

 

RE: Goal R.002 *Pulls hair out!*

(OP)
"I truly appreciate the knowledge being shared in this forum, but more and more often it seems that theory is over-riding practicality."

@EWH: It's OK by me... I enjoy the conversation.  

RE: Goal R.002 *Pulls hair out!*

Drawing says what is acceptable.  So strictly yes R.002 +.003/-.000 communicates exactly the same thing as R.0035 +/-.0015.

You may get a machinist that believes that with unilateral tols you try and get as close to the nominal value as possible but can't guarantee it.

Like I said, if .005 isn't acceptable then adjust the tolerances, and if need be find a different process or change mating parts...

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: Goal R.002 *Pulls hair out!*

I still say be careful.  Sure, Kenat, that works for onesies/twosies, but if the OP is talking about a mass-production environment, then that cavalier philosophy will goof up the tolerance stacks.  This is why the Monte Carlo method is so useful -- it can assign different "weight" to those variables in a stack that are favoring more on the plus (or minus) side.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Goal R.002 *Pulls hair out!*

KENAT,
 I don't believe that the two callouts communicate the exact same thing. While the tolerance zone is the same width and disposed between the same dimensions, the message is different between a unilateral and bilateral callout..

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

RE: Goal R.002 *Pulls hair out!*

It still seems to me that you are debating fly poo.

The manufacturer has already stated that they cannot hold a +/- .001 limit so in order to be sure that all parts are over .002 radius they will have to aim for something over .003 radius.

Personally I very much doubt that an extra .0005 on either side of the limit will mean that they can consistently produce good parts on an etching process as the radius will never be "true". Although how you are going to measure a radius that isn't a true radius to within 0.0005 I have no idea.
 

RE: Goal R.002 *Pulls hair out!*

Powerhound, from an inspection pass/fail criteria they do communicate the same thing.  If push comes to shove that is what an Engineering drawing to ASME stds does - define what will be accepted.  Per 1.4 of the 94 std it generally doesn't relate to the production process.

Now you can argue that in this case the process materially affects the end performance ... but I think that's pushing it.

Out of interest Powerhound & Belanger, where in the standard are you interpreting it to say that unilateral tolerancing implies that you get as close to the nominal value stated as possible rather than aim for the middle of the range or other variations?

As ajack & others suggest it seems the real problem is that they are on the limit of their process capability.  In which case .00X MAX again starts to sound like the way to go where X is less than the 5 which is apparently problematic to the OP's boss - I don't think we established that 0 radius was functionally unacceptable did we?  

Or perhaps you address this with the process spec suggested above, or find a way to live with .005...

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: Goal R.002 *Pulls hair out!*

I would also question the design intent on trying to hole such a tight tolerance for a radius in the first place.  That can be extremely expensive, even for parts that engage each other.

There is no such thing as a goal in any standard.  The very concept shows a radical misunderstanding of reality of tolerances. The best way to communicate the reference goal is as you alrady stated above.  State the .002 as the nominal.

Matt Lorono, CSWP
Product Definition Specialist, DS SolidWorks Corp
Personal sites:
Lorono's SolidWorks Resources & SolidWorks Legion

RE: Goal R.002 *Pulls hair out!*

KENAT,

  I'm not arguing the point from an inspection pass/fail criteria, I'm arguing it from a designer to machinist perspective. There are certainly cases where the nominal dimension of a unilaterally toleranced feature is more favorable and the favor declines as you move towards the other end of the tolerance band, for example, the slip fit of a shaft in a hole. A shaft may be toleranced +0/-.025 and the hole +.025/-0 with .025 of clearance built into the parts at MMC. If both parts are produced at MMC they will have .025 of clearance and less slop between them at assembly. While this condition is favorable, there still must be some tolerance allowed so .075 of clearance is allowed in the design but there will be more slop between the parts. You can aim for there always to be .050 of clearance between the parts and be okay but if you can consistently hit .050 of clearance then you can consistently hit .030 and since that is what the designer has preferred, why not just do it? If you process is not capable of consistently holding the .050 but staying within the tolerance zone, then that's when you should leave it alone.

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

RE: Goal R.002 *Pulls hair out!*

Kenat, you asked  "where in the standard are you interpreting it to say that unilateral tolerancing implies that you get as close to the nominal value stated as possible..."

Wouldn't it be implied from paragraph 1.3.63, which says that the tolerance is permitted from the specified dimension?  Also see paragraph 1.3.22, which states that a dimension defines the form, size, orientation, or location of a feature.

Put the two statements together: the dimension says "here's what I want," and the tolerance says, "here's what I'll accept." Sure, you are legal to make the part anywhere within range, but if all those parts please the customer equally, then everything on every print should be limit dimensions.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Goal R.002 *Pulls hair out!*

I would generally agree with Kenat on this one.  A designer might try to imply a certain target or preferred value by selecting a certain nominal, but it's not enforceable.  At the end of the day, the tolerance defines goalposts.  

J-P,

I'm not a designer, but I would hesitate to infer a desired target from the nominal dimension that a designer has chosen.  I have heard of other reasons why a certain off-center nominal might be selected, such matching a common tool size and not wanting to modify the CAD data.

If the dimension says "here's what I want" and the tolerance says "here's what I'll accept", then the logic of unilateral tolerances could be questioned.  A unilateral tolerance would say "I won't accept something that's on the wrong side of what I want, even by a millionth of an inch".  I've even seen +/+ and -/- (unequal unilateral?) specifications, in which the specified value was outside of the tolerance range.  This would say "I won't accept what I want".

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

RE: Goal R.002 *Pulls hair out!*

Perhaps I'm thrown by having seen metric type fits where the nominal shaft/hole size or similar is given and then the tolerances based on that - sometimes the -/- or +/+ that axym mentions.

Sorry Powerhound & Belanger, you still haven't convinced me.  It seems you're still trying to take advantage of aspects of the human psyche or something rather than what the standard explicitly says.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: Goal R.002 *Pulls hair out!*

Good point about the plus/plus tolerance, Evan.
 

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Goal R.002 *Pulls hair out!*

Evan,
   
"A designer might try to imply a certain target or preferred value by selecting a certain nominal, but it's not enforceable."

This statement makes it sound like you think I'm trying to say if the target dimension is not met then the part is not good. Again, if the part is in tolerance--regardless of how the tolerance is disposed from nominal--then it should be accepted. The only thing that should be enforced is whether or not it is in tolerance.

"I'm not a designer, but I would hesitate to infer a desired target from the nominal dimension that a designer has chosen."

Does this mean you would infer that even though a tolerance is shown as 0/-0.5 that what the designer really meant was +/-0.25 but just didn't know how else to express it?

"I've even seen +/+ and -/- (unequal unilateral?) specifications, in which the specified value was outside of the tolerance range.  This would say 'I won't accept what I want'."

The +/+ and -/- are an exception to this for obvious reasons. It makes no sense to me why this even exists as it causes confusion and scrap parts. I used to work at a place that had JIS prints like this. There was one part in particular that we would scrap once or twice a year because a new machinist would automatically see +/- instead of +/+ and he would adjust his cutter comp to put the dimension right in the middle of the values which always resulted in a scrapped part. It seems like the next order of that part would come around right about the time everyone forgot about the last time it was scrapped and always with a new machinist and we would go through the drill all over again.

As I said in a previous post on this thread, where I live, most machinists will machine a part as close to the nominal dimension as they can because they interpret a unilateral tolerance as the designer telling them what they would prefer but also what they will accept if they don't get what they prefer.

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

RE: Goal R.002 *Pulls hair out!*

powerhound,

I'm not thinking that you're trying to say if the target dimension is not met then the part is not good.  I'm just saying that there is nothing enforceable in the implied target.  If the designer specifies 0/-0.5 and gets a batch of parts that are all at -0.499, and the implied target was completely ignored, the designer has no basis for objection.  I believe that you would agree with this, but I have met designers who would have a different opinion.

I'm not inferring that the designer might specify a unilateral tolerance when they really meant equal bilateral, just because they didn't know how else to express it.  But I have seen instances where they would specify an unequal bilateral or unilateral tolerance for other CAD-related reasons.  One was that a fit requirement had changed and they didn't want to change the model.  Another was that the assembly was modeled with zero clearance, and so the tolerances were all unilateral +0/-.XXX.  I'm not saying that these are good design practices, just examples that I have seen.

I would agree with you that the +/+ and -/- specs are poor practices, and often generate confusion and scrap parts.  I have seen similar problems with unilateral tolerances, where the dimension was programmed at nominal and a batch of borderline parts was made.

As you can probably tell, I'm coming at this from a QA/inspection perspective.  We don't care what the designer wanted, all that matters is what they'll accept ;^).  I don't doubt that most machinists would infer the designer's preference and try to make the dimension as close to the nominal as possible.

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

RE: Goal R.002 *Pulls hair out!*

As Kenat posted and others agreed, there is no standard that tells anyone reading a print how to interpret the intent of a particular tolerancing scheme other than "make it in this range".  Unless you provide a different distribution requirement, there is nothing to guide the machinist away from your baseline normal distribution.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

RE: Goal R.002 *Pulls hair out!*

...nor is there anything to guide the machinist towards your "normal" baseline distribution.

By the way, what is "normal" and what criteria is used to classify it as such?

This must just be a Texas thing. It looks like everyone else is from the north. I guess we just do and think about manufacturing differently.

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

RE: Goal R.002 *Pulls hair out!*

KENAT,

"Sorry Powerhound & Belanger, you still haven't convinced me.  It seems you're still trying to take advantage of aspects of the human psyche or something rather than what the standard explicitly says."

This is a negative spin. Using the phrase "taking advantage of" implies something bad. Why not say we're relying on the machinist to use common sense and realize that if the designer wanted to use a +/- dimension then he would have, but since he didn't there must be a reason. I'm not arguing that my interpretation is in any standard or that it can even be legally enforced, I'm only saying that from a machining standpoint 0/-0.5 tells me something different than +/-0.25. QC just checks to see if the part is in tolerance. The part is already made by that point so it doesn't matter what the goal of the dimension is. That has to be addressed at machining.

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

RE: Goal R.002 *Pulls hair out!*

Powerhound,

One of the first lessons I was taught by one of my early mentors is that there is no such thing as common sense.  You cannot rely on anyone knowing what you think you know.

Matt Lorono, CSWP
Product Definition Specialist, DS SolidWorks Corp
Personal sites:
Lorono's SolidWorks Resources & SolidWorks Legion

RE: Goal R.002 *Pulls hair out!*

Ah come on Powerhound, I would like to think we've fought alongside each other in these virtual GD&T trenches long enough not to let this point come between us.  

I wasn't intentionally negatively spinning it, after all we say things like 'take advantage of MMC' all the time and I don't think that's a negative connotation is it?

For part drawings I tend to have to work toward the 'level 3' type category where they can be sent to any more or less competent shop and we'll get good parts.  I have little input in vendor selection for prototypes, and even less for production especially a few years down the line.  So I tend not to take advantage of things like you're alluding too with your take on unilateral tolerances.

I'm sure some, perhaps many, machinists will think like you're saying but I'm far from convinced it's all or even most and as I think we both believe it's not explicitly in the standard either way so not enforceable.

Have a good day Powerhound.

Oh, and I'm not from the Northwinky smile

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: Goal R.002 *Pulls hair out!*

I heard of a study many years ago where non-symetrically toleranced parts were measured coming from many different suppiers. It was said that the results showed that nearly every suppier aimed for the middle of the tolerance limits. If you are generating a 3D solid model, where should the surfaces lie? If you are fitting a point cloud to a CAD model, what will you get for results?

This makes me wonder about bonus tolerances on holes. Where is the middle of the tolerance zone? What should a supplier aim for? If the designer wants Cpk, what are the implications?(Just ignore this since it is off topic.)

Peter Truitt
Minnesota

RE: Goal R.002 *Pulls hair out!*

From the point of view of a former production machinist, precision sheet metal worker, and welder (and son of a career uber machinist (yes,that matters)), and design and GD&T guy, and now learning more about inspection person, same limits means same effect..

Stating same limits in some way other than equal bilateral often means either a constrained or lazy designer who is not allowed to, or doesn't want to, move the feature on the 3D model when it is discovered that it is not in the center of the optimal tolerance limits.  Once in a while a situation will be encountered for which an unequal tolerance should be specified, but most of the time equal bilateral is better.  While the standard allows a variety of equal, unequal, and unilateral specifications (& should continue to do so), it's notable that no standard describes that the effect being different unless the limits actually differ.

If you wish to think that two specs that state the same limits in different ways actually have differing effects, then of course you can continue to wish that this be so...  In some cases with some people (who think like you do), there will be a difference.  A difference that cannot be counted on is not a difference I want to acknowledge though.

If you really want a difference then ask Don Day about his proposed "delta modifier"...  Now that would be a way to make those wishes be true.  Until then, I like equal bilateral unless I run into one of those very rare cases that unequal happens to be the better choice.  Don hasn't brought up the delta modifier for quite a few years now, so it doesn't appear that it will be adopted any time soon.  I would probably be in favor of adopting it, but for now I think there are bigger issues that need improvement.

Dean
www.d3w-engineering.com
 

RE: Goal R.002 *Pulls hair out!*

I'm pretty sure I never said that stating the limits in different ways has a different effect. In fact, I know I never said it. I said it communicates a different message.

Man, why do I keep saying one thing and everyone hears something else? I feel like I've had to state and restate the same thing over and over again because I keep reading rebuttals to arguments I'm not making.

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

RE: Goal R.002 *Pulls hair out!*

Oops, in that case we may have fallen into some illogical religious battle a bit like "right to Lift" V "right to choose" situation.

In which case apologies if I've misinterpreted you and how about we call it a day before it gets ugly.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: Goal R.002 *Pulls hair out!*

"I'm pretty sure I never said that stating the limits in different ways has a different effect. I said it communicates a different message."

what's the difference?
By 'communicates a different message', I assume you mean the machinist should look at the 0/+X tolerance in a different way as he would look at a +X/-X tolerance. Hence, you expect a different result(not aiming for the center of the tolerance), or a different effect.
This may be a semantics discussion though. If I'm wrong, please educate me.


On a sidenote:
To everyone who says they rarely encounter +/+ or -/- dimensions: they are used quite a lot in fittings (bearings, axles, etc.)
At least if you work according to ISO standards. I don't know about ASME.  

NX 7.5
Teamcenter 8

RE: Goal R.002 *Pulls hair out!*

Sorry KENAT I wasn't referring to you. I was referring to Dean's comment about a different effect.

When I see the word "effect" in this context, I'm taking it as a different outcome. And from that perspective, parts that are in tolerance have one outcome, parts not in tolerance have another outcome. I thought he was saying that I was arguing a good part/bad part argument. Upon reading Waltereke's response I think I overthought that too much.

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

RE: Goal R.002 *Pulls hair out!*

poerhound,
I'm in your camp here.  The dimension is what is being asked for, the tolerance what will be accepted.
Simple communication and in no way should be confused with lazy design.  Some designs may perform better at a dimensional extreme than others.

Technically, the glass is always  full.

RE: Goal R.002 *Pulls hair out!*

(OP)
This information is disappointing. So essentially, my tolerancing method is irrelevant. The machinist will use the total tolerance and shoot for the middle. Yuck.

I'm not a vegetarian because I dislike meat... I'm a vegetarian because I HATE plants!!

RE: Goal R.002 *Pulls hair out!*

I believe your tolerancing method is fine, as does a single other person on this thread. Tell you what, send your parts to Texas to get made and they'll be made by folks who care what you're trying to say.

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

RE: Goal R.002 *Pulls hair out!*

They only make BIG parts in Texas. Try Rhode island for .002-.005.

Peter Truitt
Minnesota

RE: Goal R.002 *Pulls hair out!*

Hold on, everyone ... back up to Dean's post:
"Once in a while a situation will be encountered for which an unequal tolerance should be specified, but most of the time equal bilateral is better."

Well, what if I have one of those "situations" where an unequal tolerance makes sense?  You're all telling me (and a minority of others) that it ain't gonna happen, because we all know -- wink, wink -- that the manufacturer will simply aim for the mid-point.

In other words, then, there really is no such situation "for which an unequal tolerance should be specified"!!

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Goal R.002 *Pulls hair out!*

Powerhound,
I wasn't replying to anything you said in your posts.  I was commenting about what I think of unequal bilateral and unilateral tolerance zones.

John-Paul,
The cases I'm referring to for which an unequal tolerance would be OK are those such as when a long narrow plastic part may have a slight curve in one direction which is acceptable since another part in the assembly will tend to straighten out the plastic part, but if the plastic part were to bow the other way that would not be acceptable...  There may be a feature towards the middle of the part which is best handled with an unequal tolerance to provide more tolerance in the "acceptable bow" direction and less in the other direction.  This would be done because it may not make sense to model the part bowed in the acceptable direction, but it's OK to allow the tolerance zone boundary to be unequally disposed about the straight ideal geometry.  Once that unequal spec is there it is very likely that manufacturing will make the middle of the tolerance zone their target.  They may do that not by moving steel within the tool, but by tuning the cooling in the mold tool to make parts that bow slightly in the acceptable direction.  This is an example of what I meant by saying "Once in a while a situation will be encountered for which an unequal tolerance should be specified".

Manufacturing will tend to do things in a way that is better for them...  If the tolerance is tight relative to their capabilities then they'll shoot for the middle of the zone, or possibly stay towards a metal safe region as was mentioned in another post, to help ensure an acceptable part.  If their process is capable enough to given them more confidence then they may shift to one side of the tolerance zone to allow a cutting tool or mold tool to wear, bringing the feature through the middle of the tolerance zone, then eventually to the other side of the tolerance zone, in order get more useful life from their tools.  To hope that manufacturing will target a stated value that is not centered within the limits may be OK, but it's not a hope that I hold out much hope for.

Dean
www.d3w-engineering.com
 

RE: Goal R.002 *Pulls hair out!*

Quote (belanger):

Well, what if I have one of those "situations" where an unequal tolerance makes sense?

The only time I (am thought to) use unilateral tolerances is when applying fittings. If you want a shaft to fit in a hole you dimension the shaft D+0/-0,5 and the hole D+0/+0,5, depending on the fitting.

In this case, I have no problem with the shaft being -0,25 and the hole being +.25. It's just easier (and in my eyes, more logical) then dimensioning the hole D,25+/-0,25.

I hope this makes sense.

NX 7.5
Teamcenter 8

RE: Goal R.002 *Pulls hair out!*

Waltereke,
  Unilateral tolerancing on features of size is the only scenario I can think of that even makes sense. It's the only thing I've ever even had in my mind when responding to these posts so yes, what you have said makes perfect sense.

"Manufacturing will tend to do things in a way that is better for them..."

.......

 

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

RE: Goal R.002 *Pulls hair out!*

Rather than applying unilateral tolerancing on the two parts, I think it is better to make the stated value of each be the center of its respective tolerance zone and use an equal bilateral tolerance on each.

While the person designing the two parts may view the unilateral tolerances on each as logical, those making and inspecting the two parts may be in two different places.  Since they're only looking at one of the two parts the tolerance won't look too logical to them.  If the size tolerances are made a "critical" or "key" characteristic with Cpk requirements, the supplier will be driven to the center of the tolerance zone anyway in order to make Cpk as high as possible.  This is another reason why I think equal bilateral is a better approach.

So, equal bilateral is better if Cpk is a requirement, safer in environments where the 3D model gets to manufacturing a week or two before the drawing does, and a bit easier to work with in most manufacturing environments since the stated value will be centered and that is also likely the target size, unless manufacturing has their own reasons to choose a non-centered target value.

Dean
www.d3w-engineering.com
 

RE: Goal R.002 *Pulls hair out!*

Well, then, can anyone give a logical reason why the GD&T system allows a unilateral (or unequal bilateral) profile tolerance?  

If you all think that unilateral plus/minus tolerancing is useless, you should logically champion the same about profile.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Goal R.002 *Pulls hair out!*

What's this 'all' business.

I've pointed out that for typical drill tolerance & similar it has merit.

For 'shaft basis' and similar standard 'nominal' size applications it has some merit though also can be problematic.

I don't think I even said never to use it.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: Goal R.002 *Pulls hair out!*

KENAT,
I don't see where it's problematic at all. The only thing I see as problematic are the +/+ and -/- tolerances that have come up in this thread.

Dean,
Bringing up Cpk takes this discussion in a whole direction that is different from what we've been discussing up to this point. So far we've only been talking about parts that are in tolerance or not. Cpk introduces not only if the parts are in tolerance, but where are they in the tolerance band and how close together are they to each other. So IF a designer was, in fact, trying to communicate a preference by calling out a unilateral tolerance, would he pretty much be SOL if Cpk was a requirement?
 

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

RE: Goal R.002 *Pulls hair out!*

Discussion of +/+, -/-, and unilateral/unequal bilateral profile tolerances raise issues of modelling and drafting.  If engineers design a part at its limit of size, then they have to use unilateral tolerances.  From a detailing perspective, unilateral and unequal bilateral tolerances make sense as a convenience.  That's one side of the fence, though.  The other side is what manufacturing needs to work with, and that's a tolerance zone as opposed to a limit; they typically like to split the zone and go there as the target.  Inspection just needs to make sure it's in the zone, so whatever the tolerance is on the print, they use.

Jim Sykes, P.Eng, GDTP-S
Profile Services  www.profileservices.ca
TecEase, Inc.  www.tec-ease.com

RE: Goal R.002 *Pulls hair out!*

"From a detailing perspective, unilateral and unequal bilateral tolerances make sense as a convenience."

Maybe so, but it also makes sense from a manufacturing perspective if you actually care about what's actually being shown on the drawing. If you just don't care...well, you can't teach that.

"they typically like to split the zone and go there as the target."

Not me, and not anyone that I've ever worked with. Maybe it's not even a Texas thing. Maybe it's an Austin thing.

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

RE: Goal R.002 *Pulls hair out!*

John-Paul,
I tried to explain the type of situation for which an unequal tolerance would be the best choice in my post on the 23rd at 0:08...  Since I addressed it to you I was hoping you would see it.  Maybe you don't agree with the example..?

Dean
www.d3w-engineering.com
 

RE: Goal R.002 *Pulls hair out!*

Personally I can see both sides of the argument. But maybe that is because I don't live in Texas.

I was brought up on the hole and shaft system and it makes perfect sense to me. Say you have a 32mm shaft and on it there are a series of conditions, maybe a press fit, a slide fit, a roller bearing, a phosphor bronze bearing, a vee belt pulley, etc.

You can look up all the fits for these that are pre determined and all manufactures that I am aware of for example that make roller bearing will call these up and show them and the fit required for the mating part, so whilst no one item will be 32 +/- xx they will all be based around 32mm and easily available as off the shelf items.

I have no idea how much you would increase the cost by making all bearings, pulleys etc one offs. Strangely enough all bearings are based around the ID or OD. I would guess if you don't do this the logic is you would call up a 6.01 dowels pin, or whatever the figure would be rather than a 6mm dowel pin, now that would confuse me.

I can also see that where a complex model is involved to start putting unilateral tolerances on it means a complete remodelling job for someone, where machining directly to CAD is the only option.
 

RE: Goal R.002 *Pulls hair out!*

Quote (powerhound):

it also makes sense from a manufacturing perspective if you actually care about what's actually being shown on the drawing
Can you please point me to where in your standard it says you have to 'care' about the drawing?


Also, on a side note: people, please use quoting, it's really not that hard...
just type [quo*te name]"stuff you want to quote" [/quo*te]
(remove the *)
 

NX 7.5
Teamcenter 8

RE: Goal R.002 *Pulls hair out!*

Quote (name):

"Can you please point me to where in your standard it says you have to 'care' about the drawing?"

It doesn't say that anywhere. Sorry about the confusion.

Thanks for showing me how to do that with the quotes. I've always wondered how you guys did it.

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

RE: Goal R.002 *Pulls hair out!*

well Fcsuper then I humbly retreat myself from this discussion.
Though it was probably used in a different context.
'caring' for a drawing sounds a bit too much like 'common sense' to me, which is a very dangerous term to use, as most of you here will agree.

Powerhound, click the 'process TGML' link (not the box) under the reply box to find some more code you can use (bold,  italic, hyperlinks  etc)

NX 7.5
Teamcenter 8

RE: Goal R.002 *Pulls hair out!*

When I need to fit a pin or bearing, I get out my 20th edition Machinery's Handbook or some bearing design guide on the internet. I will see unilateral and unequal-bilateral values and I will continue my design process thinking in that mode. When it is time to create the CAD model, I will convert it to equal-bilateral because the suppliers I use will usually want my CAD model and I know that there is less chance for tooling error if everything is presented to them equal-bilateral. (I usually design medium-volume products produced from molds.) So, at this point, I am reducing risk. But I will also be wondering if the supplier (undetermined at this point) will utilize inspection technology that may, at no extra charge, generate value-added process capability data that I can use as feedback when I work on the next generation design or use to compare which suppier is using less of the available tolerance. Recently, I have been receiving graphical inspection reports that show how well the actual part compares to my CAD model. I can adjust the length of 'whiskers' eminating from the CMM probe points that show if the part is trending bigger or smaller. Numerical data also shows how much of the available tolerance has been used as a percentage. The software best-fits the CMM data to the CAD model and equal-bilateral feels very, very intuitive. So using equal-bilateral tolerances may be beneficial if you want to posture your design for utilizing automation and other new inspection technology. Certainly there are many fine products that are either made in  low volume or at higher volumes but within companies where established in-house methods effectively utilize unilateral and unequal-bilateral.

Peter Truitt
Minnesota

RE: Goal R.002 *Pulls hair out!*

(OP)

Quote (Walterke):

Also, on a side note: people, please use quoting, it's really not that hard...

Awesome! Thanks!

I'm not a vegetarian because I dislike meat... I'm a vegetarian because I HATE plants!!

RE: Goal R.002 *Pulls hair out!*

Walterke,

As I learned from an old mentor, there's no such thing as common sense.  BTW, just in case it wasn't clear, I made up the STD reference as a joke. :)

Matt Lorono, CSWP
Product Definition Specialist, DS SolidWorks Corp
Personal sites:
Lorono's SolidWorks Resources & SolidWorks Legion

RE: Goal R.002 *Pulls hair out!*

Quote (Belanger):

"If you all think that unilateral plus/minus tolerancing is useless, you should logically champion the same about profile."

J-P,

I do champion the same about Profile.

The reporting of actual values and other numerical data for Profile tolerances has been much more difficult than it really needs to be, largely due to disagreements over how to handle unilateral and unequal bilateral zones.

With a unilateral specification, there is a discontinuity where the characteristic suddenly jumps from nominal to nonconforming.  There is no way to report data for this type of spec that does not suffer from counter-intuitive or misleading results for certain cases.

I understand that the standard allows the use of unequally disposed zones, but I do not consider it to be a best practice.

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

RE: Goal R.002 *Pulls hair out!*

Dean ... of course I saw your post.  But while you set up a good reason for using unilateral tolerancing, you admit that it doesn't really matter in the end.  Thus my comment: Apparently all the greatest intentions don't change the idea that the unilateral tolerance means nothing different than an equal bilateral tolerance.
You also brought up the excellent point of capability.  In this age of lean mfg, six sigma, etc., it's one thing to be merely legal, but there are many other parameters that are important when it comes to stacks; this is why I still hesitate to jump into the camp of saying that unilateral tolerances are meaningless.
I don't disagree with you in terms of what actually happens in the shop.  While the max/min limits are really what make or break the part, I'm just saying that a unilateral tolerance communicates something.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Goal R.002 *Pulls hair out!*

Quote (Belanger):

I'm just saying that a unilateral tolerance communicates something.

You're absolutely right!

It communicates that a given dimension can be bigger(or smaller) then the given dimension, but not smaller(or bigger)

NX 7.5
Teamcenter 8

RE: Goal R.002 *Pulls hair out!*

Agreed, Walter.  But it seems that the prevailing opinion here is that the "given dimension" itself means nothing.  (Other than a convenient way to discuss a nominal value in conversation.)
 

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Goal R.002 *Pulls hair out!*

I just reread my sentence and noticed it is quite confusing, though you seem to understand what I was trying to say.

I understand you (and other people) try to explain to us that there is a difference between a X+0/+0.5 and a X.25+/-0.25 dimension, but all throughout this (pretty long) thread, I have not seen anyone define the difference, without using words as 'common sense' or 'what the designer means'.
Technically there is no difference, so there is no reason why a machinist shouldn't strive for the X.25 dimension, regardless of the way it was noted on the drawing.

Just my opinion though, which, apart from my school days, unfortunately only has a whole 2 years of actual experience to back it up. But this is how I was thought to use tolerances.  

NX 7.5
Teamcenter 8

RE: Goal R.002 *Pulls hair out!*

Here's a simple analogy to illustrate the difference.  Suppose I want to redecorate my living room. My wife sends me to the paint store, telling me to get hunter green.  "But if you can't find the exact shade," she says, "get a pale green or maybe even a light blue."

Now if the store has hunter green, but I come home with a can of light blue paint, that's within spec, right?   So all is well, as far as the wife is concerned!  But I had the capability to get closer to the "desired dimension."   So the desired dimension can be thought of as a "datum" from which acceptable variation is measured.  But I agree that in the end, there is no legal difference when it comes to accept/reject criteria.

Obviously, I'm not saying that manufacturers purposely try to go for the bare minimum to achieve a passable part.  But my point is that there is still some meaning to the "desired dimension," and besides your reference to common sense, the closest thing in Y14.5 would be the latter part of paragraph 1.3.22.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Goal R.002 *Pulls hair out!*

I would say that manufacturers do the bare minimum to achievable passable parts, well sort of.

I was always taught that in a production situation tools or cutting dies wear, i.e. shafts get bigger and holes get smaller over time, so you should start near the limit furthest away to allow the maximum run time whilst still staying in limit.

Also say a piece of stock material will conform to the limits you would not buy an oversize piece and machine it down just in order to get nearer to mid limit. The same applies to holes if you can get away with just centre drilling and then drilling you would not start adding extra processes like reaming, boring or honing just in order to get nearer to mid limit.

 I would think most manufacturers try to produce acceptable parts in the most cost effective way, rather than aiming for mid limit however it is toleranced.
 

RE: Goal R.002 *Pulls hair out!*

(OP)

Quote (ajack1):

I was always taught that in a production situation tools or cutting dies wear, i.e. shafts get bigger and holes get smaller over time, so you should start near the limit furthest away to allow the maximum run time whilst still staying in limit.

I wonder if it would be advantageous to design parts with this in mind? Maybe when designing parts that will be created as part of a mass production cycle.

I'm not a vegetarian because I dislike meat... I'm a vegetarian because I HATE plants!!

RE: Goal R.002 *Pulls hair out!*

It depends on the design.

Say you get optimum part performance at .XXX and have an operating tolerance range of +.000/-.005.
.XXX +.001 will not work in this design.
.XXX -.005 is the other limit in the design and will work, but not at optimum.

If we are talking racing, for example, I think the machinist is going to do his best to achieve the requested dimension.

Mass production introduces the trade-offs of "median" dimensions.

 

Technically, the glass is always  full.

RE: Goal R.002 *Pulls hair out!*

Production does not need to be very massive before process capability of small features becomes unrealistic, especially when considering measurement uncertainty and bias. I must wonder what the process capability has been or will be achieved in the OP.

Try this: Ask ten people to do a simple tolerance stack analysis on three mating parts where non-symmetrical tolerances are specified and see how many people get the right answer. Then do a similar exercise adding a hole position with bonus tolerance. Any right answers, now? Now make all of the tolerances symmetrical and see how many wrong answers. How many migraine headaches resulted? I like to mitigate risk and using symmetrical tolerances is a significant part of that effort in my designs.
 

Peter Truitt
Minnesota

RE: Goal R.002 *Pulls hair out!*

Ewh I would not doubt for one minute that for things like race engines machinists would aim for the optimum size, especially high end racing, F1, Indy car and the like.

What I was trying to say is that limits will be used by machinists not only to aid production but also to dictate the process and keep the costs down.

For example if you could take a piece of boiler plate and laser or water jet a finished part that would meet all criteria it is highly unlikely that anyone would fully machine the same part and start polishing, honing etc just to get nearer to the mid limit or desired size. Or at least if they did it would be a good idea to use them now as they probably won't be in business next month.
 

RE: Goal R.002 *Pulls hair out!*

I am not disagreeing with any of these manufacturing or inspection points; I'm aware of manufacturing realities.  I'm just trying to point out that the requested dimension has a purpose in the definition of the design.  That's all.  While manufacturing and quality may take the total tolerance allowance and aim for the median in fabricating and inspecting the part, the original design intent is still documented and preserved.  If the design needs to be changed in the future, such toleranced dimensions should raise a flag to the revisor that there may have been a reason for such tolerancing, other than mere laziness.  Why force mediocrity when [i[design[/i] excellence is within grasp?

Technically, the glass is always  full.

RE: Goal R.002 *Pulls hair out!*

Peter, your example illustrates one big pitfall of always thinking in terms of symmetrical, bilateral tolerances.  And that is the idea of "bonus" and "shift" tolerances when performing a stack analysis.

Bonus tolerance is usually not equal bilateral.  Guess how most people handle it?  They ignore it.  Or they try to plug it in and just figure on splitting it down the middle around a nominal.

It is possible to make it bilateral for a stack done with the strict nominal/plus-minus format, but it gets confusing with the LMC being the nominal and the ± tolerance being the stated amount and the bonus put together.   The method I prefer for stacks is simply a two-column method (one for max, one for min).  It still requires some thought when it comes to bonus and shift, yet it's very straightforward and can easily accommodate RSS and other statistical factors.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Goal R.002 *Pulls hair out!*

Quote (ewh):

Why force mediocrity when design excellence is within grasp?
A tolerance on a dimension is usually a reference to the possibilities of the machine and thus, the price of the part.
If you laser out a circle out of a sheet of steel, the tolerance on the diameter will be around +/-0,2. This means that your laser is not capable of determining the dimension of your part any better then this tolerance.
you won't send a drawing to a laser shop with a +/-5mm tolerance, nor with a +0/+10mm tolerance. In stead, you'll send them with either a +/-0.2mm or a +0/+0.4mm tolerance (numbers as examples only), where one means "it has to be around diameter X" and the other means "it has to be close to diameter X, but DEFINITELY not smaller"
In the latter case, the diameter will be programmed on diameter X,2mm, to make sure most parts are within the requested tolerance zone.

Knowing the tolerance of where your product will be machined is part of the design progress. That, or, the machine used to create your part will be dependent on the applied tolerance on the drawing.  

NX 7.5
Teamcenter 8

RE: Goal R.002 *Pulls hair out!*

Again, I'm not questioning manufacturing/fabrication methods.  I feel that is a different issue, to be aware of definitely, but it does not address the pure design aspect.  You start with a problem, seek the best solution and then tolerance accordingly, ensuring that the original design intent is captured as well as that the part is manufacturable.

Technically, the glass is always  full.

RE: Goal R.002 *Pulls hair out!*

Sorry for off topic question, but where are you in CT ModulusCT? I work right in East Windsor.

RE: Goal R.002 *Pulls hair out!*

Quote (KENAT):

per ASMEstds it's function that is the primary driver of assigned tolerances

In that case the machine used to create your part will be dependent on the applied tolerance on the drawing, which is what I ended my previous post with.

@ewh: if I want to design an axis that slides into a hole, I'd go for a sliding fitting, which, according to ISO is describes as a H-h fitting (for example)
This would result in a axis with diameter X+0/-z and a hole diameter X-0/+z.
This results in a minimum 'passage' of 0 and a maximum passage of 2z.
The design intent here is NOT for the axis and the hole to be as close to X as possible, with a tolerance of z. Aiming for the middle is exactly what I want here.  

NX 7.5
Teamcenter 8

RE: Goal R.002 *Pulls hair out!*

Walterke,
This may be, and that is fine; you know what you want (though I question the minimun "passage" of 0 - there is such a thing as line-to-line interference).  It depends on design intent, and that scheme obviously meets your requirements.

Design intent - in the design phase, as on a drawing, you really don't usually care how your requirements are achieved.  I don't care what machine you use to create my parts, as long as the parts meet the requirements.  You could whittle it out with a pocket knife for all I care.
Realistically, I do have to be aware of manufacturing capabilities and adjust my tolerances to allow for them, but again, I'm not questioning manufacturing/fabrication methods.  I am addressing the definition of the "ideal" design, which will have to accommodate those issues before the drawings are released, but not when the design is being conceptualized.  When I am starting a new design, manufacturing is not my first consideration.  It is an important consideration that must be addressed, but that is a different issue.  My first concern is how to make this design as good as possible within reason.  When that is accomplished, then I can adjust the tolerancing to accommodate down stream functions, while keeping the "ideal" definition intact.  I do not want to lose the definition of the "ideal" design to accommodate manufacturing/quality, when sufficient tolerances are already provided.  Unilateral tolerancing is one tool to accomplish that, and a competent machinist should be able to take that data, adjust it within the parameters of his tools and continue making good parts, while being aware of the intended target as defined on the drawing.
Many of the participants in this forum seem to be most concerned with manufacturing/inspection, and that is good, as it is a reality we must deal with.  I don't feel that it needs to be given such weight as to let manufacturing/quality drive the definition/documentation of the engineering design.  Putting other functions before the design function is putting the cart in front of the horse.
 
 

Technically, the glass is always  full.

RE: Goal R.002 *Pulls hair out!*

(OP)

Quote (jctoce):

Sorry for off topic question, but where are you in CT ModulusCT? I work right in East Windsor.

Is there no way to private message someone on these forums?

Anyway, yeah, I'm very familiar with East Windsor. I work in Simsbury... Where do you work in EW? What's the name of the place?

I'm not a vegetarian because I dislike meat... I'm a vegetarian because I HATE plants!!

RE: Goal R.002 *Pulls hair out!*

That should probably be directed to jctoce; I'm in TX.

Technically, the glass is always  full.

RE: Goal R.002 *Pulls hair out!*

I think he meant East Windsor.

What part of TX ewh? I thought I was alone here.

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

RE: Goal R.002 *Pulls hair out!*

Nope... work in Houston, home in San Antonio.  Which part of the republic are you in?

Technically, the glass is always  full.

RE: Goal R.002 *Pulls hair out!*

Austin area. Work in Cedar Park, live in Round Rock.

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

RE: Goal R.002 *Pulls hair out!*

Nice... want to trade?  SXSW is coming up!

Technically, the glass is always  full.

RE: Goal R.002 *Pulls hair out!*

ewh: Was going to make the trip to SXSW this year but couldn't find the time unfortunately!

ModulusCT: Genex Turbine. Right off of 91, same plaza The Wood Group is in. I am very familiar with Simsbury too, just moved out of Barkhamsted. Couldn't find a way to PM and it's been all too long since I have hijacked a thread :) Is there a way to PM?

RE: Goal R.002 *Pulls hair out!*

I think it's already been hijacked - sorry about that.

It might not be SXSW yet, but I did score Radiohead tickets for next week!

Technically, the glass is always  full.

RE: Goal R.002 *Pulls hair out!*

...also, welcome to the forum, jctoce!

Technically, the glass is always  full.

RE: Goal R.002 *Pulls hair out!*

Quote (Walterke):

"If you really want a difference then ask Don Day about his proposed "delta modifier"..."

Can anyone elaborate on this?
Frank

Nice quote trick.

RE: Goal R.002 *Pulls hair out!*

ModulusCT:  Presumably your supervisor is not the designer.  I have to wonder if the designer is more concerned about maintaining the .010 wall thickness.  The point is that the designer must be included in the discussion.  What's so important about that radius as opposed to the referenced .012 radius?  This part looks almost like it started out in life as a punched piece of .010 sheet stock, but the numbers don't quite add up.

RE: Goal R.002 *Pulls hair out!*

(OP)
slipstream44: He's not the designer. I am! He tends to micromanage all of our stuff though. To answer your question, there is absolutely no good reason why the .005 MAX radius is important. The .012 radii is reference because with constant wall thickness of .01, it's already given. This is an older drawing done by someone else that I'm not modifying and in the process trying to bring up to some kind of realistic standard.

It's a mess. I'm pushing it through the way I want it... and we'll see what happens next.

I'm not a vegetarian because I dislike meat... I'm a vegetarian because I HATE plants!!

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources