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]

It's the same idea as conventional block tolerances. Used correctly it's a good way to save work and have simpler drawings/documentation.

Used without really thinking about it for whatever reason, just relying on default rather than looking at function, process capability, inspection requirements... then it's probably a bad thing.

Posting guidelines faq731-376

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

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

 

[fcsuper]

Dingy2,

The scenario you mentioned is dingy. There is no reason to specify the same tolerance twice. The general tolerance is applied "unless otherwise specified", so the only time a specific FCF is applied is when it is needed for a particular feature or set of features that need more control that what is offered by the default. (I guess you can also use a local FCF is less control is required, but if that's the case, why bother with the specific FCF.)

Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion

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

 

[dingy2]

Kenat:

Yes, having default GD&T is, in my opinion, a bad thing but it certainly is easy for the Designer. The only advantage, as I see it, is the datum structure development. Again, if the GD&T is default, then I would assume that there is no function and relationship and it certainly would not be included in the Control Plan. Default GD&T should have loose tolerances.

The function and relationship of the features is paramount in applying GD&T. I would always suggest the use of a FCF to reflect ANY feature that is vital to its function or mating relationship and, to be sure, the respective control system will be placed in the Control Plan.

Matt:

In the situation shown, the Customer forced the default GD&T including tolerances on the supplier. If the specific FCF was not shown, I know that one would not realize that it had some function or relationship and would not be controlled that well. We can say everything is important but, in reality, it isn't. I think that supplier did the best they could and reflected an important feature with a FCF.

We, who process, make or inspect the part, must know the importance of the features. If all the features were shown in a profile of a surface with a tight tolerance, it doesn't help anyone on the shop floor.


Dave D.

http://www.qmsi.ca

 

[drawoh]

Kenat:

Yes, having default GD&T is, in my opinion...

The OP is not a drafter/designer. He is the fabricator, stuck with partially dimensioned drawings. I agree that systematic use of default tolerances is not good practise, but I am the drafter/designer.

I believe that the OP's problem is having an acceptable policy, and communicating that policy to the customer. What is the strategy that sucks the least?

JHG

 

[321GO]

swisscheese,

do you even accept accompanying drawings?


Maybe we should ask this question first..

"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

 

[swisscheese]

fcsuper - You seem to have hit the problem home with "There is no industry standard for this. Y14.41 is useless." So we need to provide our own policy.

Drawoh - Correct - we need an acceptable policy for accept/reject of non-dimensioned features of CAD drawings our customers supply us and the policy communicated to the customer - specifically how to apply a single general tolerance value.

321GO - eMachineShop does not accept accompanying drawings normally but our CAD allows to annotate drawings with text, lines, GD&T, etc. But many of our customers provide no explicit dimensioning or tolerances beyond the required general tolerance.

 

[fcsuper]

dingy2,

I don't buy that argument. There is a balance to be had. The scenario you described seems unbalanced. Seriously though, the fabracator doesn't need to know something is important...they donly need to know what you tell them.

Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion

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

 

[KENAT]

Dingy, it sounds like you are almost stepping into the territory of critical V non critical dimensions. These seems a minefield to me.

While there are a few Grey areas that still leave me over thinking things every time I look closely...

Generally speaking, a good drawing sets unambiguous pass/fail criteria that should be based on function such that a part that meets the drawing requirements is fit for use, a part that doesn't isn't fit.

I'd prefer to see more loose tolerances where functionally the fit isn't as important, rather than this idea of an overall general tolerance that can virtually be ignored - to the point to repeat the same tolerance for explicit areas where it's more critical.

Posting guidelines faq731-376

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

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

 

[swisscheese]

I would be interested in comments on the following policy for handling non-dimensioned (and incompletely dimensioned) CAD models:

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

Based on a customer specified general +/- tolerance T (required by the eMachineShop CAD) the manufactured part shall be considered in conformance if all of the following are met (governed by ASME Y14.5 2009):

1) The diameters of circular features are within tolerance T.
2) The position of circular features are within tolerance T.
3) The distances between parallel straight lines of a feature are within tolerance T.
4) A surface profile of 2 * T applied overall is met.
5) Any explicit toleranced GD&T and comments are satisfied.

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

Rational: 1 to 3 captures the reasonable expectations that T will apply to diameters of circular features, the position of holes and the size of slots and rectangular pockets. 4 provides a looser catch all. 5 is self evident.

I'm not a GD&T expert and would like to hear comments on tuning and perhaps simplifying the above approach and its wording.

 

[321GO]

If direct manufacturing from 3D is to be deploid successfully, 2D drawings with functional dimensions/individual tolerances and GD&T specifications are still necessary, period.

If one does not recognise this, one must also recognise that the approach is then unsuitable for certain products/customers.

The Germans also have a standard for this specific issue(manufacturing from 3D). They clearly state that in such setup, RDD drawings are still necassary (mainly for inspection), besides the actual 3D solid.

Again, without these necessary 2D RDD drawings, the process is half baked IMHO.

"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

 

[ajack1]

Surely this all depends on what you are trying to dimension?

For many years automotive OEM’s (including Germans) have been working with minimally dimension drawings and the CAD as master for things like body panels, where the main body is a set of sweeps and curves that could not be measured in any other way other than a surface profile but all holes (except drainage holes and access holes) have positional and size tolerance applied to them. This works fine, it is how everyone works, so it seems silly to debate if it is possible or not.

For something like a cam shaft or complicated spindle, the complete opposite is true an overall surface profile would just produce junk.

 

[ewh]

It also depends on the software used by the company and it's vendors. There are CAD packages out there which can document any applicable toleracing in the model. As long as the inspection department has the software to read those models, no dimensioned engineering drawings are required. The same model can be used for design, manufacture and inspection. There are also programs that can directly read the GD&T requirements from the model.
I strongly agree that there are few companies currently taking advantage of this technology, and some sort of 2D drawing still must follow the part through to delivery in the vast majority of situations; however I bristle whenever absolutes are used claiming it can't be done. Period.

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

 

[KENAT]

I think the distinction is that the information beyond 'basic' geometry that a drawing contains still needs to be communicated in MBD, not that there actually needs to be a 2D drawing. Whether it be more or less 'dumb' solid with a separate minimally dimensioned 2D drawing (which with current interchangeability of CAD seems to me the most robust technique for most applications) or by embedded information in the model or some other way is not directly significant.

Swiss cheese, I don't like your #4 - it's not intuitive. If you're sure the people sending you drawings are working to your 'standard' that's no an issue. However, I suspect you might end up with a lot of cases where they expect just T on the profile etc. and haven't read your in depth standard. You then get to argue back and forth, your ass may be legally covered if your spec is mentioned in your bids etc, however, it may not make you popular and could cost you business.

You could try applying the +-T as an equivalent equal bilateral surface profile tolerance (so 2T) which is to me most intuitive.

If you are really concerned over holes then you could add an additional positional tolerance of dia .28T (circling the square, approx square root 2) for all holes and similar features of size that per GD&T (at least 14.5M-94) should normally be located by position tolerance.

Keep the qualifier about any explicit tolerances being met.

While this still leaves plenty of room for misunderstanding, I think it's maybe less. At least it provides a fairly literal conversion of both +-T size of hole and +-T location of hole.

Posting guidelines faq731-376

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

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

 

[PeterStock]

A slight modification to swisscheese's proposed company standard:

1) The diameters of circular features are within tolerance T1.
2) The position of circular features are within tolerance T2.
3) The distances between parallel straight lines of a feature are within tolerance T3.
4) A surface profile of T4 applied overall is met.
5) Any explicit toleranced GD&T and comments are satisfied.

I would suggest providing this to a customer or potential with suggested values for T1 true T4 with approximate costs attached. I also suggest you add something about what would be the case if you were provided a just a dumb model, nothing on it to indicate what are the mating surfaces etc.

Also you should add something about standard finishes.

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services

http://www.infotechpr.net

 

[KENAT]

Peter, I think Swiss Cheese rules were an attempt to say how they'd interpret single overall +- tolerances.

Your rules don't help with that.

Posting guidelines faq731-376

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

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

 

[swisscheese]

Kenat - Thanks for your detailed input. You are a bit more advanced that I, so would you kindly clarify "applying the +-T as an equivalent equal bilateral surface profile tolerance (so 2T)". I intended an equal bilateral zone of T on each side which I believe is a profile tolerance of 2*T. And you lost me on "positional tolerance of dia .28T (circling the square, approx square root 2)" - in the context of Y14.5 my reference to "position" implies a circular zone and don't see a need to constrain position tighter than T. And what do you mean by "similar features of size" - I'm figuring circular features will be covered by position and odd shaped features by profile. You are welcome to propose an edit of the policy if you like.

 

[KENAT]

By features of size I mean per the ASME Y14.5M-1994 definition at 1.3.17. Per section 2.1.1.1 you should preferably use positional tolerance for locating features of size. That's my justification for suggesting it.

Your question on the overall surface profile equivalent to +-T brings to light one of the issues with lack of clarity on how the +-T could be interpreted when not applied to actual dimensions, but nominal geometry.

I was taking the +-T as a tolerance of how far a point can vary from its theoretically perfect location. As such I was proposing using an equivalent surface profile of 2T. As the machinist this works in your favor giving you the maximum tolerance zone. For example, on something like the length or width of the part, you actually end up with a tolerance of +-2T - although no point has moved more than T from it's 'perfect' location.

I think maybe you were applying +-T to 'features of size' and the like, or measurements from a pseudo 'datum'. In this case you apply a surface profile of T to give you an effective +- tolerance on the length or width of the part etc. of +-T.

It's your choice. If people aren't going to take the time to give me a fully dimensioned drawing, or explain how they expect their partial dimensioning applied, then I'd suggest applying the interpretation that gives me the most error budget so I'm more likely to make 'good' parts - so long as you make it clear in the contract this is what you're going to do.

On the position when you convert a square +- tolerance to position it's common practice to switch to the equivalent 'diameter' - at least for holes or circular boss's. This is based on the assumption that you have mating hole patterns with fasteners going through them or the like. For your position diameter you usually pick the circle that the square will fit into. The concept being that if the feature that sits in the corner of the square is acceptable, then it can be that distance from the center of the tol zone in any direction. So you end up with a circle fit on the corners of the +- square.

For example, say you have a zone of +-.005 (so a .010 square). Well Pythagoras theorem tells us the distance across corners is sqrt2 * the length of the sides. So in this case the 'equivalent' diameter is .014. Hence my suggestion to use a pos tol or sqrt2*2T.

thread1103-235569 talks about the topic of converting +- to position tolerance etc. in some detail.

It's easier to explain some of this graphically but I have too much work to create the required illustrations. Plus, whenever I do some pedantic wanna be checker usually picks it apart and that's not good for my blood pressure;-).

Let me reiterate, I think trying to have a +- overall tolerance without dimensions to apply it to is a bad idea as it's so ambiguous and as shown above can have multiple potential meanings.

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 now see and apologize for creating some unnecessary confusion with "+/-" in my July 25 draft. I intended the following (I also combined 1&3):

====

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

1) Features of size are within tolerance +/- T.
2) The position of circular features are within tolerance zone of diameter T.
3) An equal bilateral surface profile of 2T applied overall* is met.
4) Any explicit GD&T and comments are satisfied.

* Except to circular features (which are controlled by #1,2).

=====

I welcome your comments or edits on this corrected draft.

 

[KENAT]

Seems to me your position tolerance is tighter than need be. I think +-.28T is justifiable if you're doing a literal translation of +-T to pos tol dia. Even if you want to be more conservative then I'd suggest at least dia 2T. You might also want to think if you want this to apply RFS or at max metal condition. I'd think an argument could be made that applying dia .28T @ MMC is appropriate. After all a FCF without a qualifier is assumed MMC in newer ASME standards, and as I'm said I'd think the literal translation of +-T to pos dia is .28T.

I'm having trouble articulating my thoughts but it seems that 1 & 3 might conflict sometimes. Not just holes are features of size, slots are the other common example. Also, arguably for a regular shaped part, the overall shape might be a feature of size. Although as it's more a case of 1 being tighter than 2 maybe you're OK so long as you meet 1.

I still think it's a dubious idea, prone to misunderstanding but maybe you're on the path to at least clarifying your interpretation.

Posting guidelines faq731-376

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

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

 

[drawoh]

KENAT,

Swisscheese is the fabricator, not the designer. If he is confident he can fabricate to tight tolerances, all power to him. It can be a good reason to go to his shop, rather than to the grease monkey down the street, or to China.

JHG