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.

 

[Belanger]

SwissCheese -- another point is that you can't really control position (your item #2) without mentioning specific datums in a specific order of precedence.

I maintain that if you add enough notes to cover all of the bases and all possible contingencies, your policy will end up being as hefty as Y14.5.

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

 

[Belanger]

Dave -- yes the picture on the cover of the 2009 standard is wrong, IF it were meant to be a complete drawing.

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

 

[MechNorth]

OK, I'll be clear.

The content of the front cover is correct. I'm not sure what you're missing, but as I said, it is not complete.

'09: Fig. 4-38: Functional Datum Application - Adapter
What angularity control? I see a perpendicularity control applied to the secondary datum feature which references the primary datum in the FCF. Nothing wrong with that. How would you "locate" or "position" the secondary datum feature which is perpendicular to the primary datum???

'09: Fig. 3-30: Tabulated Tolerances
A runout tolerance does locate a circular surface element.

If you meant 4-37: Functional Datum Application - Pulley
Secondary Datum Feature B is controlled for perpendicularity to the primary datum A. What feature of size therein is not located? The only feature of size indicated therein is the primary datum feature ... are you suggesting we need to locate that to something ... to what??

If you meant Fig 3-29: Feature Control Frame Placement
Please note that it references section 3.5: Feature Control Frame Placement. It does not say that the drawing is complete. If they included all details irrelevant to the specific section indicated, it would be an overwhelmingly complex and confusing graphic, useless in a standard. Again, what makes you think that the drawing is complete?

By making these kinds of unjustsified and indefencible statements about errors in the standard, you are not doing the GD&T community a service, you are perpetrating your opinion only. The entire standard has to be taken into consideration, not just an individual graphic or section. I'm by no means saying that there aren't errors in the standard, but question them rather than attacking them. Adressed and validated mistakes are corrected in the next revision, though I understand impatience at the pace of revisions. There is a commitment to make the next revision far quicker than 15 years.

And, again, please demonstrate anywhere in the Y14.5 standard where it illustrates a feature of size being located by a +/- tolerance. I know from sitting in the meetings that the intent was to not have fos's located by +/- tolerances. If you want a definitive clarification, by all means contact ASME and ask for a ruling by the Y14.5 sub-committee; the contact information is on the ASME website.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[pmarc]

John-Paul, instead of saying "it is wrong, if..."- I would rather say it is intentionally incomplete.

 

[swisscheese]

I think I caused some confusion with:

1) FOS are within tolerance +/- T;

I meant, and let's change that to:

1) The size of FOS are within tolerance +/- T;

MechNorth - why do you say "Without invoking GD&T (specifically Y14.5)," when the draft directly references Y14.5? And in my 29 Jul 10 4:52 post I mention 2009.

John-Paul - see in the latest draft "*Best fit will apply if no datum is specified." And I'd like to see support from others that the policy can't leverage Y14.5 to stay reasonably small.

What would help me is any one or more of the following:

1) A proof that it's impossible to have a policy for dealing with non or incompletely explicitly dimensioned/toleranced CAD models.
2) Specific edits to the policy draft language.
3) Specific ambiguities in the policy that need resolution, preferably with a resolving edit.

 

[drawoh]

swisscheese,

In response to Belanger's comment...

When you quote, you will have to send your customer a numbered drawing, indicating what you will use as datums. You do not need actual dimensions if you promise to conform to the model dimensions.

The numbered drawing is as opposed to a sketch. You have a drawing list. You store the numbered drawing for future reference, and you call up the number in your quote. Any drawing you and your customer send back and forth are clauses in a contract. A sketch will not do.

I am being legally a pedantic prick here, but I think that is your objective.

JHG

 

[321GO]

swisscheese,

why don't you simply state that your manufacturing according to DIN-EN-2768?

If the customer wants more control, they need to submit a drawing with the additional T and GD&T specifications.
(in this case, you could defend to charge extra)

DIN_EN-2768 has two parts, first part deals with T based on feature size and part two deals with general part GD&T(basic GD&T stuff, to make sure things are symmetrical/straight/square).

To me, your proposal creates more problems than it's intented to solve. Like i said before, you are oversimlpifying, witch initself creates this confusion.



"If you have an important point to make, don't try to be subtle or clever. Use a pile driver. Hit the point once. Then come back and hit it again. Then hit it a third time - a tremendous whack."
Winston Churchill

 

[dingy2]

Jim:

I didn't say that anything was wrong in the standard except I did ask if certain figures were correct. If they were not correct, should they be corrected? I agree that the drawing on the front page of ASME Y14.5 - 2009 is incomplete and the 2 diameters without positional tolerances should have their location controlled in some manner, probably default tolerances.

Fig. 4-38 - I also agree that this perpendicularity control cannot have a positional tolerance since it controls a secondary datum requirement. Fig. 6-10, 6-11, 6-13 all reflect a perpendicularity tolerance without being a refinement of positional tolerance. This applies to all the angularity tolerances on features of size.

6.2 states "When specifying an orientation tolerance, consideration must be given to control of orientation already established through other tolerances such as location, runout and profile controls". Please note the word "location" rather than stating mandatory positional.

Fig. 3-29 (yes I meant this figure rather than 3-30). Looks complete to me except default tolerances. I really wish more drawing like this would be floating around on the shop floor where there is a good mix of linear tolerances and GD&T.

I have found that the section 2 of the standard reflects general tolerances including +/- and the application of GD&T begins stating at section 3. There is nothing including or excluding the use of +/- on locations of features of size that I could find anywhere. If you can find a statement on this subject, please let me know. Could one be in compliance to the standard if no GD&T was applied - mmmmmmm?

Jim - let you have the last kick on this subject if you want.




Dave D.

http://www.qmsi.ca

 

[MechNorth]

Swisscheese, I did miss the Y14.5 reference in your post, as I indicated above. That still doesn't make your proposal appropriate though.

Here's a core issue; if you invoke Y14.5, you invoke all of it unless you write an addendum or specific statements to the contrary, and I don't think that your note covers it. So, by invoking Y14.5, you get Rule #1 which means your toleranced size controls your form as well; Taylor's Principle allows you to do a full form check at MMC and a 2-point check at LMC. You also get a requirement to control the location of a feature of size using a geometric control, particularly position; I believe that is what youur are trying for with item #2, but it's really not clear as you don't specify any datum references. Also, the position or location control applies for the full depth of the feature, not just at the one level. Consider also that you are reducing the position tolerance rather than increasing it by going to 2T for diameter; try 2.8T.

The Y14.5 standard does not indicate in any text or illustrations that +/- tolerances can be used to locate the feature of size, so what does best fit mean in this particular instance?

If you don't invoke Y14.5, then those items aren't binding on you and you can do whatever you please because how to use and validate +/- tolerances isn't documented outside of the GD&T standards.

I do empathize, but every time I've seen a well-intentioned "compromise" like this, it's come back to haunt the company. The most successful "compromise" that I've seen is a statement that all designs not conforming to Y14.5 will be fabricated using best effort ... which leaves them pretty much in the clear when things don't work as the client expected. And yes, people keep coming back to get more work done.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[MechNorth]

Good morning, Dave,

The figures cite specific situations for orientation; again, they do not anywhere indicate that they are complete. For the concept being illustrated in each of those figures, the position dimension and control is irrelevant and therefore not included in the figure. In a production drawing, sure the information would need to be provided, but not on concept-specific drawings. It's good that you hilighted Section 6.2; it supports that on a production drawing, there would need to be a position (in these cases the use of runout, symmetry, concentricity and profile are not appropriate) control for 6-10 and also for 6-11 & 6-13 if the feature indicated was not a secondary datum feature.

Fig 3-29, yup, I think this is a good mix for this part's functionality.

Section 2.1.1.1 Positional Tolerancing Method. Note that it lists two methods, positional tolerancing and profile tolerancing, as the means of locating features ... +/- is not indicated there. Section 2.1.1(e) indicates that tolerances may be expressed in a general tolerance block referring to all dimensions on a drawing for which tolerances are not otherwise specified, however in conjunction with 2.1.1.1, it becomes apparent that general +/- tolerances are not intended to be used for locations.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[swisscheese]

321GO - Thanks for suggesting DIN - I don't have a copy but found some excerpts on the web - doesn't seem as elegant or well known as Y14.5.

MechNorth - I have no objection to Rule #1 and I do mention datum via best fit but I am open to alternatives such as giving the supplier (us) the option to select a datum if none is indicated. And I know that things apply to full depth - what is the problem? What is your objection to 2T tightening position tolerance? It seems the most natural. Where in the current draft (copied below) do you see +/- tolerances used to locate FOS?

=============

Based on a specified numeric value T (e.g. .005") the manufactured part shall be considered in conformance (governed by ASME Y14.5 2009) if:

1) The size of FOS are within tolerance +/- T; and
2) The position* of circular features (at MMC) are within tolerance zone of diameter 2T; and
3) A surface profile* of 2T applied overall is met for non-circular features; and
4) Any explicit GD&T and comments are satisfied and shall take precedence over the above.

*Best fit will apply if no datum is specified.

=============

I'm hearing a fair amount of discouragement but not much in concrete terms or example problematic scenarios. As I have said a few times, we have worked this way for years without problems - I'm just trying to polish the policy with the expertise present on this forum. I believe what I am trying to do is needed, not just by us, so why not try to improve the policy.

 

[pmarc]

OK swisscheese, maybe I'll try to point out at least few ambiguities that are hidden behind this particular policy:

1) "The size of FOS are within tolerance +/- T"
Assuming you want to do something similar to the policy you referenced in the link, you and the author are not mentioning anywhere if rule #1 applies to your drawings. So there is no connection between size and form of your FOS. Therefore perfectly straight FOS as well as banana shape things can be equally accepted.
Additionally you are saying you know the tolerances apply to full depth (length and width also), but the question is does everybody know this. Where is it written in your policy?

2. "The position* of circular features (at MMC) are within tolerance zone of diameter 2T"
--- You are asking what is wrong with 2T diameter of positional tolerance for the circular features? Is it a tightening of tolerance? Yes, it is. Please look at attached sketch. You will see what I believe was MechNorth's point.

http://files.engineering.com/getfil...c7f1-42de-aa13-c971c9428e1e&file=position.JPG

By specifying 2T cylindrical position tolerance you are making tolerance zone even smaller than in traditional +/- dimensioning method, of course if traditional +/- positional tolerance was meant to be specified at 2T.

--- Why are you assuming MMC on positional tolerance every time? There are some very fundamental functional requirements (e.g. symmetry, centering or alignment) where MMC is not prefered. Of course MMC gives a lot of benefits, but only when the function of component requires that. So if you want use MMC everywhere you can simply misinterpret designer's intent. The reason of it is you did not receive precise instruction from designer, because he did not dimension his part.

3) "A surface profile* of 2T applied overall is met for non-circular features"
If you do something like this you assume that tolerance zone is fixed regardless of a feature's size. This might sometimes work, but is some cases - where the assembly is important - there could be bigger size tolerance for a rectangular slot when corresponding groove is not at his MMC.

General comment: as I said in one of my previous post, you would need to write very long document to cover all the possibilities than can occur for a part's geometry. I gave you only few remarks, but I believe other folks could deliver more. If you are in close contact with a designer this idea can work - because you will explain everything verbally, but when the designer is far away and does not speaking your language you could have serious troubles.

 

[Belanger]

Swiss--

FYI, when Pmarc refers to "Rule #1" he is talking about Y14.5's Rule #1 (aka the "Envelope Principle"), not the first rule of your policy.



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

 

[swisscheese]

Pmarc - Thanks for your comments. In reply:

1) I don't know what link you refer to and I am the author. MechNorth wrote "by invoking Y14.5, you get Rule #1 which means your toleranced size controls your form as well". Since the policy invokes Y14.5 and I want size to control form and don't want bananas, what's the problem? Similarly, by referencing Y14.5 we are clear about the full depth issue. So again, what's the problem?

2) Thanks for taking the time to create the drawing illustrating types of tolerance zones but I understood all that previously. "By specifying 2T cylindrical position tolerance you are making tolerance zone even smaller than in traditional +/- dimensioning method" - I'm aware of that and it was intentional - what's the problem?

3) Kenat suggested MMC but I'm open to revision of that. But remember, the policy is for covering missing information and any customer can override with whatever GD&T they want.

4) Again, the customer is welcome to specify any overrides.

You wrote, "you would need to write very long document". I am yet to be convinced we can't leverage Y14.5 to keep the policy short. In fact the policy so far in this thread actually shrunk 27 characters.

I'm getting the impression that asking for advice on how reduce use of GD&T in a GD&T enthusiast forum may not be the smartest thing I have done.

John-Paul - Yes, I know.

 

[Belanger]

OK (about Rule #1) -- I just wanted to clarify.

But I still don't get it, fellas. If SwissCheese is invoking Y14.5, then why not use the methods prescribed by Y14.5 to invoke things such as "profile all over" or "position at MMC within a diametrical tolerance zone" -- they're called feature control frames!

Swiss, if your customers don't know GD&T, then I kinda think that invoking Y14.5 is a bad idea from the start. I know you are seeking concrete recommendations rather than mere critique. Yet everything you are trying to do already has established methods, and I'm just concerned that walking this fence between Y14.5 but not using GD&T will be confusing...

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

 

[swisscheese]

John-Paul - It was my intention all along to "invoke" things in Y14.5. But I could use some help with the language of the policy. I didn't say our customers don't know GD&T. Some of them do, some don't. But even the ones that do often rely on our approach without problems. I don't know what you mean by "Yet everything you are trying to do already has established methods". If you mean a policy already exists for ambiguity resolution of non-dimensioned CAD models, a lot of people are keeping it a secret.

 

[Belanger]

It's as simple as this: Instead of a verbal note saying, ""The position* of circular features (at MMC) are within tolerance zone of diameter 2T," you can make that into a feature control frame (position symbol, diameter symbol, number, although the datums might need to be more specific).

And it doesn't have to be tagged with a specific feature; I've seen many traditional drawings that have feature control frames within the general notes paragraph. My suggestion is just to use established symbology wherever possible rather than words. The fact that it is to be a general tolerance for the component doesn't prevent the use of GD&T symbols.

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

 

[swisscheese]

Oh - good idea. I have no problem with that.

 

[ajack1]

What is the saying “A camel is a horse designed by a committee.”

 

[MechNorth]

Pmarc, tks for the following up; JP too. I've been out of town.

Swiss, I understand what and why you're doing. I just know from significant experience that such "policies" snowball into a monster. Anybody here familiar with the old GM GD&T Addendum? A company that I used to work for "customized" gd&t to fit their business-unit needs as they saw them; it ended up with a bit of ISO, a bit of ASME, some "conventions", and a lot of "if-then-else" type of conditions ... all well intentioned, but crippling nonetheless. Aside from suggesting that you fully deliniate gd&t and "traditional" drawings, I can't in good conscience advise any wording that would be helpful. Good luck.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com