GD&T part costing more 5

From my experience there is a lot of truth in the statement he made. My experience goes back quite a few years, for that matter. 20 years ago there were no local tech schools which offered courses relating to Y14.5. NASA and Micom are/were 2 major users at that time.

It is my opinion that many of the short courses offered are inadequate and serve only as an introduction to GD and T and are over-priced.

I once worked for a company that provided in-house training for all who worked with drawings. It was a major defense contractor. They used a self-teaching book, which I thought was excellent for the time. (1963)

I like your numbers 1 & 4.

I have seen some well know trainers state that all features of size should have positional tolerances and all surfaces should contain profile tolerances rather than adding FCFs only on fit and function. Most drawings are a bit of over kill and the using the noted approach will cost extra $$$$.

If Designers would only add GD & T on fit and function, then all of the areas noted with the exception of your #1 would be addressed. If you need it, apply it. That's it.

If you have positional tolerances on holes/pins where there is a fit and function, make sure that they are applied at MMC. If they reference another feature of size, make sure it is also at MMC. Tell the vendor that they would end up getting more tolerances and it would not hurt the integrity of the drawing.

Make sure that you have someone in your company quite proficient in this subject otherwise get outside assistance. It takes a long, long time to become proficient in this GD & T. It took me 10 years of training to become comfortable so get help if you need it.

Explain to the vendor what the particular applied GD & T means and hopefully, the costs should be around the same.

Good Luck!!!



Dave D.

Making prototype parts is not the same as production. Along with production and GD&T comes inspection, documentation, recordkeeping, process monitoring, etc. Most anyone can knock off a few protos with few controls.

Honesty may be the best policy, but insanity is a better defense.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

I have also experienced parts being priced much higher when GD&T is used. The people involved with the part, purchasing & machinist, do not understand GD&T. They think it requires inspection and a special expertise to make the part, so they add cost.
When GD&T is used correctly, it is usually less cost than without it.

Chris
SolidWorks 07 4.0/PDMWorks 07
AutoCAD 06
ctopher's home (updated 04-21-07)

I would say that #'s 1 and 4 are the most likely candidates with a lot of weight being given to #1. If the guy adding the GD&T was clueless he would have put a bunch of nonsense together and any shop that understood GD&T would have either no-quoted it or called with questions. I don't think #2 is it because if the part functioned correctly being built at the limits of it's tolerance based on the coordinate system then the new tolerances would at least appear looser. For example, if you have a hole position called out at 2.0 +/-.010 from an edge in both X and Y, a conversion of the same tolerance into a cylindrical tolerance zone and put into a FCF would read "positioned within a diameter of .028 WRT A, B, and C." So instead of your maximum tolerance in one direction being .010, it could POTENTIALLY be .014 depending on how far off of true position the other axis is, not to mention when you see a tolerance of .028 as opposed to +/-.010 it even looks like you have more. The exception would be if the part DIDN'T function correctly when built at the limits of it's tolerances in which case they would need to be tightened anyway. As far as #3 goes, it's in the same boat as #4. Incorrect GD&T doesn't make for a more expensive part, it just makes for an incomplete drawing. A shop that knows the difference will ask what you meant.
I teach GD&T as a side job and while I still don't know everything about it, BB's like this help me out tremendously. That being said, I always present GD&T as a language. You can understand it perfectly but if the shop doesn't, you haven't communicated squat with your perfectly Y14.5M compliant print. This entire post could have been written in grammatically correct Spanish but what good would that do for those of you who don't speak a word of it?

dingy2,
I have to disagree on your point about only putting GD&T where you need it. If the print states to interpret the drawing per ASME Y14.5M-1994 then shouldn't the print comply completely? If you pick and chose the components that you want to adhere to then your supplier might do the same to you, such as deciding that he doesn't think general rule #1 should apply to the part he just sold you. Now you have a .250 pin that was produced at MMC but it has straightness error of .020 and it won't completely go into the .255 hole that you intended it to because all you put as a tolerance was +/-.005 and assumed he would comply with general rule #1. When you use the term "overkill" you give me the impression that you think that the addition of GD&T is more of a nuisance than anything. I contend that a fully Y14.5M compliant print is cleaner, clearer, and is only open to one interpretation to those who fully understand it. Specifying the standard invokes a heaping helping of fundamental rules and general rules that are designed to close loopholes that suppliers have used over the years to force their customers to buy parts that are screwed up but the condition is not addressed in the standard. For example 1.4(m) states that all geometric tolerances apply to the full depth, length, and width of the feature. Now why do you think they would add this to the 1994 standard? It wasn't in the 1982 ANSI standard. I believe it was because there were a lot of suppliers that insisted that the positional callout only applied to the top of the hole and not the bottom. ASME probably heard about it and addressed it.
Anyway KENAT, I think #1 is your most likely candidate. It happens more often than not and way more often than I'd like to see.
As a side note, I go to take my ASME GDTP-Technologist level test in a month. Wish me luck.

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

OR,

5. The vendor understands GD&T just fine. But he doesn't get paid for preparing quotes, and he only gets 1/10 or 1/100 of the jobs he quotes on, so it makes no economic sense for him to put any effort into understanding what you mean with all your fancy symbols. He eyeballs the part print and guesstimates a process based on the tolerances he can pick out right off the bat. He DOESN'T HAVE TIME to do fancy calculations to find out that you are giving him 'bonus tolerances'. He quotes on what's there, and easy to figure out. If he wants the business, he quotes based on breaking even with the eyeballed process and the tolerances he can find with a few minutes' inspection of your print. He's going to estimate higher when GD&T symbols are present, just because he knows that he'll have to go three rounds with _your_ quality assurance people, explaining to _them_ what a bonus tolerance is.

If and when he gets the job, _then_ he goes over the print with a fine tooth comb, not looking for bonus tolerances, but looking for ways to fixture and/or process the part that will be significantly cheaper/faster than the process he assumed when he quoted. If he finds a way to make it cheaper, that's his profit.


Mike Halloran
Pembroke Pines, FL, USA

Powerhound:

Good luck on the GD & T exam. Study hard and you need a minimum average of at least 75%.

Maybe I did not explain what I meant by "appying GD & T where applicable" and "over kill". I did not mean that the ASME standard should not apply. It should. All drawings should state in notes that "this drawing is in compliance to ASME Y14.5M-94. That covers rule 1 and everything else in the standard including full depth.

BUT

I have seen so many drawings with all surfaces with a profile of a surface tolerance and all dimensions basic. Is it really needed on all surfaces? What if a surface has no function and relationship to the mating part? Could a +/- tolerance be sufficient?

I have seen in under notes various layers of profile tolerances where a +/- might have been sufficient. Each time one in Quality sees a profile tolerance, that surface is scanned using a CMM and this is costly. Is it really needed?

This "over kill" on the application of GD & T does drive up the $$$.

Each time a Designer places a FCF, should they not ask themselves something like "what is the function and relationship of this feature". If there isn't any, probably co-ordinate or polar tolerances are sufficient.

I hope that this explains what I meant in my prior submission.

Dave D.

Hi Dave,
Thanks for the quick reply and thanks for wishing me luck. I'd like for you help me clarify something. I don't really see the difference between calling out "profile of a surface" and a plus/minus when either one would work. For example, if you have a block that is one inch thick, you can call it 1.0 +/-.010 or you can call it 1.0 BASIC, call one side datum A, and specify the other side "profile of a surface within .020 WRT datum A. They both say exactly the same thing and should be checked exactly the same way. General rule #1 still limits the variation in size to +/-.010 at any point on the part. I know that applying a plus/minus tolerance gives the impression that it's not as critical and applying a profile of a surface gives the impression that it's very critical so if the overkill you were talking about was based more on perception than reality then I will agree with you on that point. The reality is that even if the tolerance is plus/minus, no part of the surface may violate the MMC or LMC boundary, POS simply orients the surfaces to a datum frame and +/- doesn't.

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

All things being equal, I do hafta agree that GD&T when using positional or profiling should be a little more expensive because of the methodology employed in following the set up requirements is more, even if the tolerance is actually looser.

With simple D&T, the feature simply has to fall within a particular (usually square) tolerance zone. However, the real feature size affects which tolerance is applied in positional GD&T, since the tolerance varies based on the feature size (material condition). So, instead of just one tol zone, the vendor now as to know a range of tol zones. A premium should be expected for this, but not a huge premium unless every dim was replaced with GD&T. Just my opinion though.

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

So another Option then:

5. The vendor didn't bother taking the GD&T into account when preparing pricing to save time or for whatever reason.

While I'd have major concerns over using a vendor like this it's not my decision and it is an option, thanks Mike. It’s pretty close to #1 but I guess distinct enough to mention.

In general case #4 is a hot contender, in the particular case I detailed though this wasn't at all the case. The guy who helped with the GD&T is really good.

Maybe I should explain more about option #2. From what I've seen/can gather a lot of the engineers/designers here don't do anything approaching even a minimal tolerance analysis on their designs. In fact some even say that due to the level of precision we (or at least they think we) require on finished assemblies that we shouldn’t insist on anything near 100% interchangeability and should put up with having to match parts on the shop floor or just rejecting a significant number of components. As such they’ll happily design parts that don’t go together at anywhere near worst case, in fact even if you do some kind of statistical analysis, from the one time I remember doing it on someone’s design, it was scary.

The philosophy seems to be “if I can throw down a quick CAD sketch and get a prototype made that works then that’ll be fine for production too”.

Doesn’t help that our place is loathed to qualify new vendors, doesn’t have an estimating department and rarely competitively tenders items.

On the question of when/whether to use FCF, I’m inclined to think ASME Y14.5-M 1994 section 2.1.1.1 is pretty clear for dimensioning the location of Features of Size.

2.1.1.1 Positional Tolerancing Method. Preferably, tolerances on dimensions that locate features of size are specified by the positional tolerancing method described in section 5. In certain cases, such as locating irregular-shaped features, the profile tolerancing method described in Section 6 may be used.

I know a lot of people will say ‘preferably’ doesn’t mean it’s mandatory… To my mind though if it’s in there then even if not mandatory you should follow it unless you have a really good reason not too. Of course saving $$ may be a pretty good reason. Also I’m wondering if it probably means positional is preferable to profile except in certain cases.

However, I too have heard of the GD&T trainer who wants to profile almost everything.

Powerhound, good luck. I’ve asked about my company getting me certified but they haven’t seemed overly keen, I may ask again as I’ve taken up checking duties.

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

Kenat you seem to answer your own question.

You state, “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)

Then you go on to say, “The philosophy seems to be “if I can throw down a quick CAD sketch and get a prototype made that works then that’ll be fine for production too”.

Doesn’t help that our place is loathed to qualify new vendors, doesn’t have an estimating department and rarely competitively tenders items.

Do you not think that this is where the real problem lies and that however the parts are dimensioned is just a side issue?

Without wishing to sound rude it seems you are adding to the problem rather than trying to solve it.

Yes it is where the real problem lies but sadly my remit is limited.

It is somewhat like banging my head against the wall and I'm considering alternative employment but as long as I'm here I'm trying to do the best job I can.

The philosophy is mixed, we have various people who claim to support us but I no longer take anything at face value.

Will admit, I'm not quite sure I see how trying to improve the quality of drawings is adding to the problem however, just fixing the drawings wont solve all the problems, of this I'm well aware and may dig up new ones such as the increased part cost, is that what you mean?

Should I not do my job because it will be at least partially negated but others?

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

Matt,
The only special methodology employed in checking a positionally toleranced feature as opposed to a coordinately toleranced one is that the size of the feature being checked affects the tolerance allowed when a MMC modifier is used in the tolerance portion of the FCF. You check each one exactly the same way but with a positionally toleranced feature you use the handy dandy chart in the ASME standard to determine the actual amount of positional error. In the case of a single feature you would check the error in X and in Y. Lets say the tolerance is +/-.005. If you are .005 off in X and .005 off in Y then you are actually a straight linear distance of .007 away from your target which would put you within a diameter of .014. If you can miss your target by .007 and still be good then there is a lot of wasted tolerance with a square tolerance zone.
All of that aside, the only added expense that may be involved in a geometrically toleranced print is that functional gauges may be required for certain concepts like datum shift, but coordinate tolerancing doesn't provide for that at all and, thus, parts that could be usable wind up in the scrap pile.
KENAT,
Your last comment about not doing your job because you get resistance really hit home with me. I have the same problem where I work. We recently had a major shift in leadership and I was given the task of challenging the status quo and making people give damn good reasons for why things are done the way they are done so I took that to heart. One of our issues is that we have spent years building and checking parts based on what we think the customer wants instead of what they've specified on a print because what they've specified is utter nonsense. Things like "flatness within a diameter of .004 at MMC, WRT A, B, and C at MMC" and the leader is pointing to a surface, not a feature of size. What in the world are they really trying to say with a callout like that? Anyway, I made the mistake of rejecting prints like that and insisting on some clarification before I sent junk like that out to the shop floor to let them deal with it and get beat up when they make what they think the print says and QC checks what they think the print should say and now we have 2 different versions of what the print says, so who is right? Of all the people I expected resistance from, the QC manager was the one I'd least expected it from. To make a long story short, I've given up that pipe dream and I'll quote anything that comes across my desk no matter what the print says. I won't even attempt to enforce the standard anymore. That may not be the right thing to do but I'm viewed as more of an anal ASME thumper than a draftsman anymore because of my adherence to standards. These aren't even prints that we make, they are customer prints and when junk like I described is defended by someone who should know better, I realize that the problem goes waaaaaaaaaay deeper than I ever could have imagined.

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

Powerhound,
I know. But just think about how much more thought goes into determining the specification of a postional verses coordinately tol'd dims, and the reverse by the vendor. There's a ton of comments about peoples inability to do this quickly on this topic board. That really speaks volumns about costs. Maybe it's not just as easy as the ideal would have us believe? There really is a lot more thought that goes into the handling of positional tolerances. That thinking takes real time. Time is money. Sure, you can find someone with the experience to do all the figuring more quickly, but how long did it take that person to get to that level of understanding? It wasn't over night.

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

Powerhound:

Using your example of 1 inch thickness with a +/- .010 and comparing it to a profile tolerance is not the same.

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.

Now let's compare that situation to having one surface as datum A and using a profile of a surface of .020. First of all, you are stating that the part mounts on datum A by designating that surface as a datum. I would have to set up on that surface (probably using a 3 point set up). I would then using an indicator on a height gauge (or CMM) zeroing off on datum A and move it up 1 inch. Now I would sweep the entire surface with my indicator using a +/- .010. This method is pretty extensive when compared to a +/- tolerance.

I would suggest only using a profile of a surface when there is a function and relationship of that surface to datum A and also to the mating part.

I will give you an example of "overkill" that I see on some drawings.

I was finishing training in a company and they gave me a new drawing that had just come in from corporate. This was a drawing of a chain saw tooth but ALL dimensions on the drawing were basic and in notes they have 4 or 5 levels of profiles. Someone asked me what they should do with a drawing like this? I asked what features were important from a function and relationship point of view and there were only 2 of the surfaces. I suggested redrawing it showing the profiles on the 2 surfaces only and then using a +/- on the others prior to release for tooling.

No wonder vendors jack up the price when they see "overkill" on a drawings such as the above. I probably would too.

I hope this helps.

Dave D.

Hi Dave,
I see your point about only checking local size but according to general rule #1 features may not exceed the outer boundary determined by MMC of the part. This includes features of size that only have a plus/minus tolerance. If you are checking local size within tolerance, how do you know that the outer boundary is not being violated? If the 1.0" block (or plate) was produced at MMC (1.010) and has a straightness error of .005 then your actual outer boundary is 1.015. If you only checked this with a caliper or micrometer, you would only be checking local size and you wouldn't detect the straightness error, or any error in form for that matter, and would be in violation of rule #1. If Y14.5M is specified on the print, then your part would have to comply and in this case perfect form at MMC would not be detected by the method you specified. Obviously a note saying "Perfect form at MMC not required" would solve the problem but that's not what we're talking about. If the part were produced at 1.009, there would only be a straightness error of .001 allowed. If the part still had .005 of straightness error the outer boundary would still be 1.014 and still be out of tolerance. Whether or not the people that made the print actually knew about rule #1 and would check it based on that is beside the point. I'm talking about what is correct according to the standard. If the standard is specified on the print then the part should be checked accordingly.

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

Powerhound:

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.

The USL & LSL would be the same if we had a profile of a surface tolerance of .020 but here one would require a datum for reference. There is no reference datum here but only a width dimension.

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.

If it was a profile of a surface, I would set up on the datum plane assuming it perfect and then scan the surface using a +/- .010 around the basic dimension of 1 inch. I could also use a CMM to scan it. This feature is important to the function and relationship and that is the reason for reflecting it in a profile tolerance.

I could have a +/- tolerance and the part could be within specification since we are measuring a width but the same part could be out-of-specification using a profile tolerance. Why?? We need a datum surface and that surface may not be flat but we have assumed it flat.

mmmmmmm- does this help or not???

Again, I would suggest applying a profile of a surface where there is a fit or function. If not, go +/-.



Dave D.

Well thanks for the posts everyone. You've given me some food for thought.

We have a Design Room Manual that states to follow ASME Y14.100 with especial attention to 14.5 & GD&T. This was approved by the various heads of departments. So it's not a case of me just trying to enforce my will, I've been tasked to help enforce the DRM that in turn invokes the standards. That said written policies & procedures here mean almost nothing so just referring people back to the standard and telling them ‘because it says so’ won’t achieve much.

I’m trying to win people over with convincing arguments and wanted to make sure my arguments were fairly sound.

When I started out with GD&T I thought it was only for critical features etc but as I got to know more about it I became convinced of its wider application. Seems quite a few of the posters here still have doubts about its wider application, with some arguments that aren’t easy just to put aside.

Well, guess I need to do some more learning/research.


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

I was a fan of GD&T until I saw it blindly implemented by an IDIOT drafting supervisor.

He opened up the clearance holes in a relatively simple plate held down by (14) x #10 screws, so that every possible plate would fit every possible substrate. He wound up with .281 clearance holes around screws with a shank diameter of .190, and a head diameter around .250. So if the plate was in the ideal, desired position, and all the holes were in the ideal positions, which is the most likely result, the heads of the screws drive right through the plate and don't retain it. His solution to _that_ problem was extra large flat washers under each screw head ... which still left the location of the plate, relative to certain mating assemblies, uncertain. His solution to _that_ problem was a locating fixture, unique to that product, which had to be provided for each assembly station, and for each of 500 service engineers worldwide.

The project manager was too stupid to see that as a problem or too weak to fire the dumbass. It wasn't _my_ project, so I couldn't get any traction to do anything about it. It took several more millions of dollars in unnecessary fixtures for someone in authority to wake up, too late to save the company.

----

I actually _like_ using GD&T symbology to communicate design intent, especially when dealing with an international workforce, because it's language independent. Even with a monoglot workforce, it beats the hell out of the stilted notes I've seen over the years.

But it's hard to do it right, and it's harder to convince stupid people that they're doing it wrong.




Mike Halloran
Pembroke Pines, FL, USA