Minimally dimensioned CAD drawings GD&T 3

[swisscheese]

On minimally dimensioned CAD drawings I hear Y14.41 is not user friendly, not particularly useful (and not inexpensive). I've been searching and searching for anything that provides a good set of rules for how to manufacture and inspect against CAD drawings that include only a single general tolerance. Does anyone know of or have any internal documents or web sites they would share (publicly or privately)? Thanks.

 

[KENAT]

SwissCheese - I would be very hesitant about using ISO2768 - in my opinion it's a POS. I've started several threads about it and debated it with enthusiasts take a look by all means. Maybe it can work for people the 'think DIN' however, for me who thinks ASME or BS, it doesn't work.

Posting guidelines faq731-376

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

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

 

[swisscheese]

Using the suggestion of FCF's and putting them in general notes, what do you guys think of the image linked below?

http://files.engineering.com/getfile.aspx?folder=81712e3a-1d87-4d3b-997c-e36e12b869e4&file=RDD.jpg

 

[fcsuper]

Swiss,

Curious, is there a reason you are breaking out feature of size from non-fos?

For the profile fcf, I would label that box as "Basic CAD Model" or "Apply to non-FOS" or something similar. I would also use the modifier "ALL OVER" instead of the double circle, since the double circle seems to require an arrow. Both mean the same thing, but "ALL OVER" seems cleaner for title block use, IMO

Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion

http://groups.yahoo.com/group/solidworks & http://twitter.com/fcsuper

 

[swisscheese]

fcsuper - Thanks for your suggestions - I will update the image.

I'm treating FOS and non-FOS differently for a few reasons:

1) We want a looser all-over profile tolerance so as not to unduly constrain us as the supplier which ultimately helps keep prices down, which, of course, is what many customers want.

2) In our experience, the size/position of FOS more often requires a tighter tolerance than other aspects of a design.

3) There is no profile tolerance that is equivalent to the proposed FOS size and position tolerance.

4) Our customers range from large organizations down to individual inventors and hobbyists. Some of the later understand simple +/- tolerances and that's about it. If, for example, they choose .005" as the general tolerance they might reasonably expect the distance across circular and rectangular features to be +/- .005" and the position of circular FOS to be +/- .005. (The proposed position tolerance is slightly more constrained due to the circular zone but a circular zone is generally more sensible.)

 

[MechNorth]

don't forget that there are now "irregular" fos per '09, and continuous features can now be used as fos.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[fcsuper]

Yup, ASME Y14.5-2009 has expanded both FOS and Profile "ALL OVER" principles.

Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion

http://groups.yahoo.com/group/solidworks & http://twitter.com/fcsuper

 

[swisscheese]

Taking recent suggestions and doing a little more polishing, how's this:

 

[KENAT]

Well I still like 2.8T for position;-). Also I stand by my MMC suggestion on holes at least.

My view point as I mentioned earlier is that if the person supplying the drawings can't be bothered to prepare them properly, I'll interpret them the way that gives me most usable tolerance.

That's not to say I don't try to do better for customer satisfaction etc. However I see no point committing to tighter if the customer doesn't explicitly ask for it.

I still think it's dubious, but maybe somethings better than nothing.

Posting guidelines faq731-376

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

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

 

[swisscheese]

Kenat - I appreciate, understand and partly agree with most of your comments, with the possible exception of your ummm concluding remark.

Though 2.8 T is advantageous to the supplier, it's not as elegant IMO - you have to explain where the strange number comes from, on top of explaining the policy overall. So I'd prefer to stick with 2T.

So here is the latest version.

 

[KENAT]

Oh sorry, you actually think they're going to read the policy?

Not sure about your explanation of where T comes from. I'd maybe use a few more words explaining it comes from the +-T stated on the drawing. The talk of CAD settings is a bit unclear to me.

Posting guidelines faq731-376

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

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

 

[ewh]

"+-T to pos dia is .28T"

If you have a +/- tolerance of T = .010", it can be translated into a positional tolerance of .28T = .028" DIA. using simple trigonometry. Thusly the commmon +/- tolerance of .005" translates into .014" DIA.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[swisscheese]

Kenat - our CAD has several things that lead to the tolerance policy but of course there are always people that don't read much of anything - not much we can do about that. But they are forced to enter some value for T and if they have no idea of what they are entering and don't care there is not much we can do about that either.

About 2T vs. 2.8T, I get the geometry and the math. But first, I never had a clear objective to try to replace non-geometric old style (square zone) +/- tolerancing. But even if I had, a circle is not a square not matter what size you use. There are, however two fairly logical substitutions - the circle circumscribing or inscribing the square. The former is better for the supplier, the later for the customer. I chose to favor the customer. Or is the point that most tolerances are used to insure parts mate and most mating is done with circular features in which case the circumscribed circle is just as good as the square?

In any case what would the vote be if we clean the slate and forget about replacing +/- tolerancing and just come up with a logical policy for converting a single numeric value into a tolerance policy oriented around the GD&T mind set. Isn't 2T a more logical and simpler choice?

 

[KENAT]

Hang on. I thought you were trying to interpret customer drawings which had a simple +- general tol on them, which was why you had to come up with this troublesome attempt at interpreting +- tols.

Now you're saying your CAD... If they are your drawings then I'd say do it properly. By all means have some kind of all over profile tolerance to minimize dimensions etc. as discussed elsewhere but beyond that tolerance explicitly based on function etc.

"Or is the point that most tolerances are used to insure parts mate and most mating is done with circular features in which case the circumscribed circle is just as good as the square?"

Yes. Ideally of course you'd know if it's for mating fasteners before you did the math but then we'd be back to square one.

Posting guidelines faq731-376

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

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

 

[Belanger]

SwissCheese wrote: "There are, however two fairly logical substitutions - the circle circumscribing or inscribing the square. The former is better for the supplier, the later for the customer."

This question comes up a lot (about putting the circle inside or outside the square). But instead of trying to favor the supplier or customer, the real question is this: If you look at the square tolerance zone, suppose an axis drifts out to the very corner of the square. Is it still a functional part? If the answer is yes, then you can almost always go with the circumscribed circle. But if the corner is not functional, then the inscribed circle is best.



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

 

[ewh]

If the corner is not functional, the tolerance is not tight enough.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[Belanger]

Right -- but believe me, many designers apply square tolerances zones but then say, "Well, I didn't really mean to allow it to go up AND over at the same time!"


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

 

[swisscheese]

Kenat - eMachineShop supplies customers with a free CAD package that has a field for a single tolerance number and we are polishing the policy for how we use that number. This thread so far has made good progress to that end and the input is appreciated. Again, we are talking about drawings supplied by our customers using our CAD package. (We also allow customers to use conventional explicit GD&T but the focus of this thread is on "lazy" a.k.a. RDD and NDD drawings.)

OK, I think I'm finally sold on 2.8. Latest version:

 

[swisscheese]

Just wanted to thank everyone for their helpful and patient input on this rather long thread. I think significant improvements were made to our original spec and the improved version has been put into use.