GD&T part costing more 5

[KENAT]

I was talking to another Engineer the other day and the old chestnut came up of.

“Well I had a part without GD&T which I’d got prototypes for. I then had the GD&T guy take a look and add GD&T and when I sent the new drawing to the vendor it came back significantly more expensive” – (this is a paraphrase of a longer conversation)

In this case the GD&T guy was my checker, before he was laid off, who had 40 years of experience, had used GD&T for a long time, had training, been a level 3 checker in aerospace/defence etc. So while not infallible he was pretty darn good, certainly the best I’ve ever worked with.

Now the only ways I can see this would have happened was:

1. The vendor didn’t understand GD&T. I’ve seen/heard of places that seem to charge an extra % or more for each Feature Control Frame. Basically if they see any FCF etc they increase the price, even if the tolerances are actually effectively ‘looser’.

2. The part wasn’t originally dimensioned/toleranced adequately to ensure function and fit and so in the process of adding GD&T tolerances were tightened but due to functional requirements not inherently because of the addition of GD&T.

3. The GD&T was added incorrectly based on the function of the part. I can especially see this being the case if the person doing GD&T wasn’t familiar with the function of the part and the Engineer didn’t provide all the necessary information/mating part details etc.

4. (Kind of a variant of 3) The person adding GD&T didn’t have a clue what they were doing.

Knowing the guy who did the GD&T I know it wasn’t 4 and I doubt it was 3 so I’m guessing it was 1 or 2.

It looks like it’s going to get taken to management, not specifically this case but the whole concept of drawing checking and what we’re trying to do with adopting standards and I know this kind of thing is going to be one of their main points. Saying it was 2 won’t be popular or win me any friends and if it’s 1 they’ll say “why use GD&T then” rather than “we better find some competent vendors”.

So I’d appreciate any input-

Does anyone else have any possible reasons for the price difference?

I’m sure some of you get this thrown up to you, what is your response?

Thanks for the help.






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

 

[KENAT]

We have people who put the extra large holes and fender washers but without even applying GD&T.

As well as GD&T we're meant to be looking at making parts cheaper/DFMA so the increasing cost is a concern to us as well.

I'm trying to be careful in what GD&T I apply to other peoples basic designs/drawings. Partly because not being fully familiar with the part it's difficult to make sure you're not unecessarily tightening it. I'm also really missing the experienced guy who got canned, I used to bounce a lot of things off him. Hence I've been looking at the standard so much.



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

 

[powerhound]

Well I guess we'll just have to agree to disagree Dave. We're just saying the same thing over and over again. Datums are independent of outer boundary. General rule #1 applies to +/- tolerances whether you want to accept it or not. A 1.0 +/-.010 thick plate must slide between two plates of equal of greater size spaced exactly 1.010 apart and the local size cannot violate the LMC boundary (.990). Any error in straightness cannot create an outer boundary of more than 1.010. That's why the summary of general rule #1 is "perfect form at MMC". At MMC any error in straightness will cause a violation of the outer boundary of the part. This is all in the standard. Paragraph 2.7.1 is where it starts. It specifically addresses where only a tolerance of size is specified...no symbols or FCF's. I get the impression by you ending your posts with "I hope this helps" and "does this help?" that you aren't even entertaining the thought that I might have a valid point.

You said:
If I saw the 1 inch dimension on a drawing, then I would probably use a vernier calipers or maybe a micrometer and measure the feature in, probably, 3 places. Each place would have to be in specification. No big deal here.

My response:
Actually you've done nothing to verify that the outer boundary of the feature conforms to general rule #1. If your print specifies Y14.5M then you must check this or risk passing a bad part as good.

You said:
It has always been understood that if we measure a +/- tolerance, the feature cannot be outside the specifications. Your example of 1 inch with a +/- .010 has a USL of 1.010 and a LSL of .990. This was understood prior to rule #1 of ASTM Y14.5M-94. As a matter of fact, not too many understand that rule anyway.

My response:
The first part of your statement refers to local size. If a part with +/- .005 measures -.006 then of course it's bad , I'm not arguing that point. I'm talking about outer boundaries here. The second part of your statement along with our discussion up to this point leads me to believe that you are one of those who doesn't understand the rule but I've seen your credentials on your website though so I'm not sure why you're not understanding what I'm trying to say. Maybe I'm not communicating effectively.

You said:
Now we get into measuring. It is NOT 100% accurate. If I saw a +/- tolerance, I would take 2 or 3 measurements with a vernier or micrometer, 1 in the middle and then 2 on different edges and report the results. This feature is not important to the fit or function of the part.

My response:
The first part of your statement - Accuracy is not the issue as much as making sure the part is in spec or not. You won't necessarily have to know what the measurement is, you just need to know what it isn't. This is where GO/NOGO gauges are handy. Also, the results you report would only verify local size and not the condition of the outer boundary. The second part of your statement - whether or not the feature is important should be independent of whether or not it's checked correctly and to specification.
Okay, it's late enough. I guess this is one for the books unless there have been longer ones. Take care and I hope I haven't ired you, I don't mean to.



Powerhound
Production Supervisor
Inventor 11
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[fcsuper]

The discussion here between Powerhouse and dinky2 are really making my point. How much time is involved in this effort of figuring it out.

At is appears now, more time is spent figuring out positionals and profiles than figuring out coordinates. The arguments as to why this is so (e.g. comments about "stupid people") are fruitless because the arguments themselves are part of the time being spent. This is why positionals and profiles should only be used on critical features, even if it is technically better (when applied properly) in other cases. It's the time it takes to figure the things out and argument about them, not necessarily the time it takes to follow through on them.

Even in this discussion, two people I would think who are in a position of authority to talk about this can't agree.

BTW, powerhouse, you can't "agree to disagree" and then continue on that arguement. That's not agreeing to disagree...it is more like establishing the presumption that more arguement is necessary. hehehe Don't get me wrong, I don't mind the continuation of the argue, as it is enlightening in several ways.

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

 

[fcsuper]

BTW, I would just like to confirm that you two [bold]are[/bold] talking about different things. powerhouse is discussing boundry condition and dinky2 is discussing importance of a feature. These are two very different topics. However, both affect f/f/f and either other.

To extend dinky2's comment on something that powerhouse said: Why would you have a go-no-go gauge for a feature that you know doesn't affect f/f/f? If it's not critical, then it's not critical. If it's not critical, why (for example) call out positional tolerance that requires three datums to describe it (whether those datums are easy to obtain or not).

To extend powerhouses's comments about something dinky2 said, Positional tolerances are followed through upon using the same methods as linear coordinate dimensions, and are under the same sort of restraints. Positionals simply provide you with a more realistic approach to establishing a tolerance for the features in question. Following this logic, the machinist doesn't nothing different in making the part for positionals than they do for linear coordinate.

Is this an accurate summary?

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

 

[powerhound]

Haha, I had every intention of ending the thing after saying that we could "agree to disagree" but got way off on a tangent. I finished up my thoughts and hit the submit button. When I went back and re-read my post I realized what I had done after I read the first sentence. Sorry about that.
Your statement on the use of a GO/NOGO gauge presumes that it's a known fact that he feature is non-critical. I have put forth no such notion. Let's say that the feature isn't critical though. If it's out of tolerance, do you still pass it because it's not critical? If your answer is "no" then whether or not it's critical is a moot point. It still has to meet spec., right? If your answer is "yes" then why check it at all?
Your statement about positional tolerances needing 3 datums to describe them assumes that holes that are coordinate toleranced will be perpendicular to surface on which they are indicated. This is not a safe assumption. If there is no geometric tolerance, then fundamental rule 1.4(m) does not apply. There is nothing that constrains the orientation of the hole, so it can be out of perp by more than would allow the part to be usable. Having 3 datums indicates which surface the hole should be relative (or perpendicular) to. This doesn't make it more complicated at all. It only specifically defines how to set the part up and how to check it.
Your statement about the machinist doing nothing different whether the location is coordinate or positional is correct. The difference rears it's ugly head in inspection.
This has definitely been an enlightening thread for me as well, but to be honest, up to this point I thought that the veterans on this forum were a little more on-board with complete compliance with the standard. A 100% geometrically dimensioned and toleranced print is not more complicated to those that understand what it means. The problem occurs when people see the symbols and assume it means tighter tolerances. It rarely does.
Anyway, good day to all.

Powerhound
Production Supervisor
Inventor 11
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[dingy2]

Powerhound:

This is my last kick on this topic.

I absolutely agree with you on the outer boundary on the 1 inch thick material. To confirm this to rule #1, one would lay the part on a granite table, zero up the table top and then go to the highest point on the other side. Yup, you are correct that the set up is the same as a profile set up.

Would I confirm the thickness as shown above if I saw a +/- tolerance? No - I would confirm it exactly what I said I would and the same as you have in the past. If there was a function and relationship, my checking method would change.

I have seen vendors get caught in this one and the Designer has covered their butts well here but the drawing was not as clear as it could have been. If I saw a profile of a surface tolerance on the feature, I would know that there is a function and relationship on this feature.

Here is a tip for all the Quality Engineering types out there since I know you can get caught on rule 1.

Review all features of size on a drawing and find out their respective function. If you have a hole or pin and it does have a function (another pin going into the hole) mark up your drawing using a FCF with 0 straightness tolerance at MMC. One will need a straight pin of its smallest allowable size to confirm a hole to rule 1 which simulates assembly. On a pin, one would need a sleeve with an ID of the largest allowable size (MMC).

All dimensions on a drawing are numbered. Number these marked up feature control frames as well.

Yes, Powerhound, sometimes communication is difficult.





Dave D.

http://www.qmsi.ca

 

[KENAT]

Powerhound, I'm inclined to go along with your line of thought.

A lot of people for some reason tend to think if a feature has GD&T then it's more "critical" than other features and/or tend to use GD&T only on features they consider "critical".

I don't see this as being correct based on what 14.5 (or the equivalent BS/ISO etc from what I remember) actually say.

However, because many (most?) people in the industry think like this it has a significant impact. Even if the person creating the drawing knows what they are doing if the people interpreting the drawing think this way then it can artificially increase costs.

And don’t get me started on the whole notion of “critical” from a dimensioning point of view. A dimension has tolerances (even if supplied through GD&T), these tolerances should be driven by function. Just because a feature isn’t tightly toleranced doesn’t mean it’s not ‘critical’ to stay within that tolerance. If a drawing of a part is toleranced correctly then isn’t it ‘critical’ to meet tolerance for all dimensions? I realize this can’t be taken to extremes, for instance a cable that’s one or two thousandths longer than the max tolerance is probably fit for purpose and could be passed on a waiver but isn’t the general principle correct?

An inspection plan should surely be based on better grounds than simply “which features have the tightest tol”/”which features use GD&T”? Then again I’m not an inspection expert so better stop there.

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

 

[121560]

I agree with Kenat; (1. The vendor didn’t understand GD&T. I’ve seen/heard of places that seem to charge an extra % or more for each Feature Control Frame. Basically if they see any FCF etc they increase the price, even if the tolerances are actually effectively ‘looser’.) the solution is collaborate with your vendors like Dingy2 suggested. The real cost of machining is setup time, multiple machine op's, non-std tooling, non-recurring eng'g chg's (expedite cost ) and tolerance, for example a round tolerance zone has 58% more area than a rectangular tol zone with out even considering bonus tol as hole postion departs from mmc. Also consider the capability of the machining process, for example calibrated CNC machines typ achieve feature to feature hole locations +/-.002 or +/-.001 it is to your company an eng'g benefit to take issue with any percieved additional cost when using GD&T. With todays technology design engineers can easliy estimate cost and should like using solidcam inconjunction with solidworks. "I also agree with all that Powerhound wrote". With one exception when protyping I typ apply GD&T to features/surfaces that effect fit,form,function all other minor characteristics I generously rect tol +/- well within the machining capability to time constraints. A company I worked for partnered with there select vendors giving them 3rd party software enabling to program from solidmodel.

 

[ajack1]

121560 wrote “A company I worked for partnered with their select vendors giving them 3rd party software enabling to program from solidmodel.” A star for you my friend.

Speaking as a vendor one of the problems we face is people sending in jobs for quotation that you know you have very little chance of winning, they are often a fax or a pdf that are barely readable and they want the quote in the next four hours, you simply have to cover your rear.

If you select vendors and they know that they stand a 1 in three chance of winning the work they will quote more carefully. It is also wrong IMO to assume the vendor does not understand the drawing, he may well see a certain limit that he thinks requires extra set ups could only be done on one specific machine the inspection would be a nightmare, any number of reasons. Also don’t forget the vendor is not quoting to the limits he is quoting to ALWAYS be inside them in a worse case scenario. All this is before you get into the nitty gritty of what is actually asked for so well illustrated by Powerhound and Dinky2.

If you want quality parts at competitive prices talk to your vendors, they maybe able to reduce costs by just changing the way the part is dimensioned or by you explaining exactly what you want again I refer to the discussion between Dinky2 and Powerhound.

The big issue here as I see it is the “jobsworth syndrome” the designer designs the part to agreed standards, the checker checks the job to required standards, the required number of quotes are received to the required standards but no one looks at the bigger picture.

Maybe if everyone sat back and looked at it from the other persons point of view things would run a lot smoother?

 

[powerhound]

ajack1,
I agree with what you said about there being possible extra set-ups which could potentially jack up the price of the part. The OP said that GD&T was added so I don't know if that means that there were form callouts added where there previously were no form callouts or if some square tolerance zones were converted to cylindrical. Adding form callouts could definitely increase the cost while changing from a square to a cylindrical tolerance zone SHOULD either not affect the price or decrease the price. I really like what fcsuper said about how the machinist does nothing different whether he has +/- or positional tolerances. A shop will never be able to consistently produce a part that has tighter tolerances than the machine can hold. If I saw a drawing for a part that had a coordinately toleranced hole position of +/-.001 and one for the exact same part except the tolerance was +/-.030, the difference to me would be I would have to center or spot drill the hole of the tighter toleranced hole first before drilling it. I have no control over how repeatable the operation would be and I have no significant control of drill bit deflection past center drilling the hole so the only real increase in price would be based on one extra drill step (center drill) and then if I felt I would lose a part - based on such a tight tolerance vs machine capablity, not operator error- I would probably charge extra for that. The thing about what I'm saying is that the price would, and probably should, increase based on the tight tolerance, not GD&T or my inability to interpret a print using GD&T.
I also agree with you about talking to vendors when things happen such as the incident that prompted this thread. I can guarantee you that I would be asking them why the part was suddenly more expensive to make if the GD&T that I added was simply converting square zones to cylindrical ones. As I said before, adding form tolerances where there previously were none, could possibly be justification for added expense but the tolerances would have to be refinements of form error already allowed by the general tolerances. In fact if they are not refinements, they are illegal. I can't believe I'm doing this on a Saturday...again.

Powerhound
Production Supervisor
Inventor 11
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[PSE]

One thing to consider that may increase the cost of a GD&T part is that of metrology. When you start introducing callouts that cannot be measured with micrometers/calipers or simple tooling, you then start moving into CMMs etc. This increases costs.

Regards,