Minimally dimensioned CAD drawings GD&T
Minimally dimensioned CAD drawings GD&T
(OP)
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.





RE: Minimally dimensioned CAD drawings GD&T
Dimensioning and tolerancing go hand in hand, so a general tolerance such as "all dimensions get ±0.5 mm" only makes sense if the dimensions for which that apply are explicitly stated. While the world of CAD has obviously been a great development for designers, the only "general tolerance" that would truly apply to an undimensioned CAD model is a geometric tolerance such as profile of a surface "all over."
Think of a part shaped like a staircase. If the only thing we have to go by is the CAD model along with a single general plus/minus tolerance, then we have confusion: should I measure from the floor to the first step and apply the plus/minus? Should I measure from the floor to the second step of the staircase and then apply the plus/minus? But what if I measure from the first to the second step and now apply the same plus/minus... see the problem?
If these drawings are being given to you by in-house engineers or by your customers, you have every right to pose this question to them, since they are giving you ambiguous instructions.
John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
RE: Minimally dimensioned CAD drawings GD&T
h
But nowhere have I found the details of a reasonable set of rules and conventions. It sounds like Y14.41 might be what we need but I heard it is not very useful so did not yet purchase it.
Your suggestion of profile of surface is the kind of thing I am looking for but would like to determine if that is an accepted approach and whether there are other approaches.
Your statement "only makes sense if the dimensions for which they apply are explicitly stated" makes me wonder if you accept the concept of "implicit dimensioning" that CAD provides and the time savings that MDD provides. I know well the ambiguities illustrated by your staircase example. The question is how to define a set of conventions that resolve those ambiguities.
We have processed thousands of orders using Minimally Dimensioned Drawings via our CAD and, essentially, a single tolerance, using our own set of ambiguity-resolution rules. This approach has saved our customers countless hours and has allowed our non-engineer customers to design and order parts with minimum hassle.
But we want to align our rules with an accepted convention - hopefully one that is reasonably practical to implement and understand by customers and inspectors.
Jim Lewis
emachineshop.com
Online Machine Shop
RE: Minimally dimensioned CAD drawings GD&T
RE: Minimally dimensioned CAD drawings GD&T
Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion
&
RE: Minimally dimensioned CAD drawings GD&T
Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion
&
RE: Minimally dimensioned CAD drawings GD&T
I think this discussion is drifting away from your requirement.
My minimally dimensioned, you mean that quite a few features are not dimensioned at all, much less, controlled by tolerances. This can make sense. If you are manufacturing electric toothbrushes shaped like Garfield the cat, orthogonal drawings with tolerances are not functional.
You must have accept/reject criteria. An orthogonal drawing with a complete set of dimensions and tolerances provides this.
Step back from the formal documentation procedure, and work out a practical way to specify, then accept or reject your parts. Your document process and standards will follow logically from this.
RE: Minimally dimensioned CAD drawings GD&T
So, how are you going to do that, if you don't know the specifications? How can you "defend" your part?
Isn't RDD a shroud for cutting corners at the expense of diligence..
RE: Minimally dimensioned CAD drawings GD&T
thread1103-239768: Current state of Model Based Definition is one of the more recent and has links to others.
14.41 seems almost more for the CAD companies to tell them what their CAD package needs to be able to do, rather than for every day folks creating MBD data packs.
That said, it is of some limited use.
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
As far as I know, MBD has nothing to do with eliminating dimensions. Necessary dimensions are still necessary, but appear in model space and not on a drawing. Y14.41 attempts to clarify how to apply dimensioning in model space (or model/drawing space when drawings are used).
As KENAT noted, Y14.41 does lean heavily in establishing what CAD systems need to be capable of.
"Good to know you got shoes to wear when you find the floor." - Robert Hunter
RE: Minimally dimensioned CAD drawings GD&T
But he is asking what that default plus/minus tolerance refers to. It can't be any randomly selected dimension, because that leads to tolerances which will be fighting each other.
I already gave my two cents, but I'm just trying to help keep the thread on track for the OP...
John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
RE: Minimally dimensioned CAD drawings GD&T
I just checked out 14.41 and it addresses this in section 8.
However, all it says that I think is directly relevant is that One or more general notes defining plus and minus tolerances may be specified. (8.1)
Then at 8.3 it says to use existing drawing standards for plus and minus tolerances.
To me a +- tolerance, with out an explicit dimension to apply it to is ambiguous, especially one tolerances start to stack.
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
I finally got a copy of Y14.41 which appears to offer essentially no help.
As I mentioned, there is one suggestion to apply the tolerance value as a profile of surface but I would like to know if that is the accepted approach or there are others. I see some disadvantages of that particular policy at least based on our objectives: to have a policy that that reasonably reflects what a common customer would expect the general tolerance to mean; and a policy that does not dramatically increase rejection rate by undue constraints. For example, I would think that a common customer would expect the general tolerance to, in part, apply to the true position and diameter of holes, but if the general tolerance is applied as a profile the acceptance criteria would be far more constrained, not something that would help us stay price competitive.
RE: Minimally dimensioned CAD drawings GD&T
It sounds like you are the fabricator, and you are receiving partially dimensioned drawings. You need to tell customers how you are going to manage their drawings and CAD models. You expect to be paid after the following...
- You will meet all dimensions and tolerances specified on the drawings.
- In the absence of a specified dimension and tolerance standard, you will interpret drawings as per ASME Y14.5M-1994 (ASME Y14.5-2009?)
- In the absense of specified dimensions, you will fabricate to the CAD model.
- In the absense of specified tolerances, you will position holes to Ø0.3mm, and hole profiles to 0.6mm
Modify units, numbers and standards to suit you, and get your lawyer to translate everything into legalese.How about that?
RE: Minimally dimensioned CAD drawings GD&T
are you such an "eMachineShop"?
Normally (elaborate) 2D drawings are needed for the manufacturer to understand the demands (tolerancing/GD&T/surface treatments/painting scheme) of the customer's part.
Now, how can you do this if there is no such drawing? I'm confused.
Good afternoon...I would like to patent "the wheel"
RE: Minimally dimensioned CAD drawings GD&T
For example, a mold file for a composite part would have, in the SOW, controls placed on the part surfaces, any critical feature locations,and indexing tooling balls. The rest of the design/toleranceing we leave to them and are usually pleased with what is delivered. Of course, this design work cost is included in the quote.
"Good to know you got shoes to wear when you find the floor." - Robert Hunter
RE: Minimally dimensioned CAD drawings GD&T
So, I iterate my suggestion earlier. If you are using model based definition, I recommend envoking ASME Y14.5-2009 and using the ALL OVER modifier on a general profile FCF that applies to your whole model. If you need to control profile with datums, then identify those datums on the drawing with additional locally noted profile FCF for those specific features. This allows you to use the drawing to identify important specific dimensional specifications without detailing the entire part. It also allows you a traditional and well understood method to make other specifications, such as material, finish, markings, etc.
Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion
&
RE: Minimally dimensioned CAD drawings GD&T
So when you place the default profile of a surface - all over in notes, does this specify features that are important to its function and relationship or all features?
Does this really "allow you to use the drawing to identify important specific dimensional specification without detailing the entire part"?
Dave D.
www.qmsi.ca
RE: Minimally dimensioned CAD drawings GD&T
For some plastic parts we do similar (though as we still reference the 94 version it's a bit iffy). We have a general surface profile. Then the mating holes are explicitly dimensioned and positional toleranced.
The intention is the same as a general +- tolerance, but done in a way that I think is more robust for un-dimensioned 3D forms.
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
The features shown with a default profile of a surface may have a less impact on their function and relationship (probably none) and one should think of them the same as a +/- default tolerance. No heavy inspection applied on these surfaces - maybe initial samples only.
This reminds me about one company I visited. Their customer forced them into placing a default profile of a surface tolerance of 0.5 mm relative to a primary, secondary and tertiary datums. Yet, on the same drawing there was a particular surface that was profile of a surface shown in the FCF of 0.5 which is the same tolerance as the default. They told me that the profile shown in the FCF was important to its function while the default wasn't. It had the same tolerance as the default. mmmmmmmmm???
Should this be the approach to take?
Dave D.
www.qmsi.ca
RE: Minimally dimensioned CAD drawings GD&T
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.
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
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
&
RE: Minimally dimensioned CAD drawings GD&T
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.
www.qmsi.ca
RE: Minimally dimensioned CAD drawings GD&T
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?
RE: Minimally dimensioned CAD drawings GD&T
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
RE: Minimally dimensioned CAD drawings GD&T
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.
RE: Minimally dimensioned CAD drawings GD&T
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
&
RE: Minimally dimensioned CAD drawings GD&T
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.
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
=============
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.
RE: Minimally dimensioned CAD drawings GD&T
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
RE: Minimally dimensioned CAD drawings GD&T
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.
RE: Minimally dimensioned CAD drawings GD&T
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." - Robert Hunter
RE: Minimally dimensioned CAD drawings GD&T
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.
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
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
www.infotechpr.net
RE: Minimally dimensioned CAD drawings GD&T
Your rules don't help with that.
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
RE: Minimally dimensioned CAD drawings GD&T
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: Calculating Positional Tolerance 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.
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
====
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.
RE: Minimally dimensioned CAD drawings GD&T
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.
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
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.
RE: Minimally dimensioned CAD drawings GD&T
I'm not saying he doesn't aim for tighter tolerances.
However, if his customers can't even be bothered to properly request certain tolerances, why offer tight ones?
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion
&
RE: Minimally dimensioned CAD drawings GD&T
====
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) 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.
=====
Do you see any serious problems or ambiguities with this?
RE: Minimally dimensioned CAD drawings GD&T
aren't your terms confusing?
ASME Y14.5 2009 does not support one single tolerance, the tolerance is dependent on the size of the feature, or i'm i wrong?
So, if you accept one single T, you by fact do not confirm to ASME Y14.5 2009.
To me, it seems you are ignoring the complexity of this issue.
"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
RE: Minimally dimensioned CAD drawings GD&T
It's true that looser tolerances are often used for larger features and a customer is welcome to specify that, but the policy is intended to give a simple rule that covers model aspects that don't have explicit GD&T. We have been working this way for years.
Certainly GD&T *can* and often is complex, but it does not *have* to be. As long as the policy is clear, customers will know what to expect and inspection will know how to inspect.
RE: Minimally dimensioned CAD drawings GD&T
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
I was taught that the fundamental reason of using GD&T on drawings is precise and unambiguous description of designer's intent, so as a result clear and full definition of part's geometry.
Maybe this will sound brutal, but I believe such RDD ideas are in total oposition to GD&T philosophy. Sorry to be so general, but it would require writing quite a long essay to describe all ambiguities that stand behind this kind of policies. And you would have to write even longer text to make this vague areas clear. And in the consequence this short policy would have to be at least a few page document.
RE: Minimally dimensioned CAD drawings GD&T
Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion
&
RE: Minimally dimensioned CAD drawings GD&T
RE: Minimally dimensioned CAD drawings GD&T
Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services
www.infotechpr.net
RE: Minimally dimensioned CAD drawings GD&T
As for Y14.41, the '03 release was the first kick at the can; it was needed as a bridge to guide CAD companies on how to set up their software for a common set of functionalities, and start the transition over to model-based GD&T application. Work has started on the next revision, and we'll see what comes of it now that at least some of the original requirements have been implemented in CAD (though most CAD is way behind as of today). For those that see it as a useless document, that's from a users' perspective; look at it from an overview perspective of CAD and engineering, and you'll see that it was a foundation stone.
Many companies have been using a note "ALL OVER" or "GENERAL TOLERANCE" with a surface profile control for better than a decade, with great success. Some, unfortunately, don't understand how to use it effectively and therefore make it a burden rather than a useful tool ... then again, from this very forum we know that observation is equally true of many GD&T implementations. "ALL OVER" symbol is new in '09; previously, all we had for symbology was the "ALL AROUND".
Jim Sykes, P.Eng, GDTP-S
Profile Services www.profileservices.ca
TecEase, Inc. www.tec-ease.com
RE: Minimally dimensioned CAD drawings GD&T
I absolutely agree with you that "position of a feature of size is not established with +/-". They must be shown in basic dimensions.
Now, the location of a feature of size may be different. I know of many examples in the newest standard that show this without positional but, as you stated before, you found a disclaimer of some sort.
I would suggest just looking at the cover of the 2009 standard and note that not all of the features of size have their location shown in positional tolerances. Let's see, the diameter of 99 - 100 and also the diameter 56.6 - 57.6 on the cover are not shown in positional - mmmmmmm.
Dave D.
www.qmsi.ca
RE: Minimally dimensioned CAD drawings GD&T
Please, Dave, list for us some of the examples you suggest are in the standard wherein "locations" of features of size are controlled by +/- tolerances.
I've taught a number of people, including several other instructors, who initially held a similar perspective to yours. Many think that "preferred" and "should", etc. give you carte-blanche to do anything because it isn't specifically precluded. Those who have worked to establish voluntary standards know that those are about the strongest words that can be used outside of a federally mandated standard. Federal standards can use the words "shall", "will", "must", etc. as specific directives, but voluntary standards cannot because they have specific meaning under the law. ASME produces voluntary standards in that you are free to adopt them, and there is typically no specific legal action (other than contractual and civil liability) for twisting them out of shape. I understand that many companies have done /are doing /will do it as you endorse, however that is not supported in the Y14.5 standard or any other published standard, voluntary or mandated. Just because some people drink & drive without having had a terrible incident, it doesn't mean that it's acceptable or appropriate. Society moved beyond acceptance of DUI, hopefully industry will accept that GD&T has some distinctly right and wrong methods, per whatever standard is adopted.
Jim Sykes, P.Eng, GDTP-S
Profile Services www.profileservices.ca
TecEase, Inc. www.tec-ease.com
RE: Minimally dimensioned CAD drawings GD&T
Yes MechNorth you did. When giving suggestions to the OP on how to come up with a way of interpreting the meaningless +- tol with no dimensions I referred to ASME Y14.5M-1994 several times.
The OP is more or less forced to accept drawings this way. He's trying to come up with a moderately robust way of interpreting it, explicitly detailing this way, and referencing it on all quotes/contracts.
I still don't like it, but I'm not completely without sympathy for the OP. I suspect refusing to take these drawings, or charging to redraw them etc. may be a business limiting approach. Certainly you can try and educate the other party but when that fails, or risks alienating them, is the OP's basic idea - though problematic - so unreasonable?
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
That being said, however, I can't see it standing up in court as it's not by any means clear. I've been stuck in pissing contests before about who's right, and nobody wins in the absence of a defined & prescribed standard. Otherwise, it's all "best effort". I don't have a better solution, either, but I would hate to see SwissCheese walk away from this with a warm & fuzzy that this is going to be effective and protective.
Jim Sykes, P.Eng, GDTP-S
Profile Services www.profileservices.ca
TecEase, Inc. www.tec-ease.com
RE: Minimally dimensioned CAD drawings GD&T
If SwissCheese comes up with a reasonable document detailing how +- tolerances will be applied to nominal geometry by his organization, and that document is referenced on contracts then so long as the document is reasonably robust it should be some use.
Surely it's the fact that it's in (or referenced by) his contract that gives it some standing - not that it is or isn't correct to 14.5 or the like.
As someone mentioned, it may be worth talking to a lawyer, though of course the chances of them knowing what's going on with a topic like this are slim.
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
Are you stating that the front page example of the 2009 ASME Y14.5 is wrong?
Dave D.
www.qmsi.ca
RE: Minimally dimensioned CAD drawings GD&T
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
Dave, if you're going to make a statement about +/- tolerances being used in the standard ('09) to locate features of size, you really need to back it up, or you should reasonably retract that statement to sift some of the mud from the waters.
Jim Sykes, P.Eng, GDTP-S
Profile Services www.profileservices.ca
TecEase, Inc. www.tec-ease.com
RE: Minimally dimensioned CAD drawings GD&T
You didn't answer my question on whether the front page example was wrong. Maybe the example should have deleted the features of size not shown in positional?? I would think that ASME should at least have the front cover example correct.
There is not a statement anywhere that mandates that features of size must be shown using position. There is a recommendation in the 94 & 2009 standard though. There is also a recommendation of not using concentricity but it does not say it is wrong to use it.
There are so many examples in the latest ASME revision on cylindrical products where the feature is shown with an angularity tolerance and no positional. Fig. 4-38 is an example. Is this figure wrong?
Fig. 3-30 reflect many features of size without positional tolerances. Is this figure wrong or maybe we can use the disclaimer you found a little while ago.
Must angularity tolerances on features of size be a refinement of positional? I can't find that in the standard either. How would one show the location of a hole where only perpendicularity is shown?
I realize that you promote default positional and profile of a surface tolerancing. Does that really reflect the design intent of the part? Should the features that truly have a function or mating relationship be specified separately or is everything lumped in to the default?
Dave D.
www.qmsi.ca
RE: Minimally dimensioned CAD drawings GD&T
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
RE: Minimally dimensioned CAD drawings GD&T
John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
RE: Minimally dimensioned CAD drawings GD&T
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 www.profileservices.ca
TecEase, Inc. www.tec-ease.com
RE: Minimally dimensioned CAD drawings GD&T
RE: Minimally dimensioned CAD drawings GD&T
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.
RE: Minimally dimensioned CAD drawings GD&T
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.
RE: Minimally dimensioned CAD drawings GD&T
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
RE: Minimally dimensioned CAD drawings GD&T
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.
www.qmsi.ca
RE: Minimally dimensioned CAD drawings GD&T
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 www.profileservices.ca
TecEase, Inc. www.tec-ease.com
RE: Minimally dimensioned CAD drawings GD&T
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 www.profileservices.ca
TecEase, Inc. www.tec-ease.com
RE: Minimally dimensioned CAD drawings GD&T
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.
RE: Minimally dimensioned CAD drawings GD&T
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://
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.
RE: Minimally dimensioned CAD drawings GD&T
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
RE: Minimally dimensioned CAD drawings GD&T
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.
RE: Minimally dimensioned CAD drawings GD&T
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
RE: Minimally dimensioned CAD drawings GD&T
RE: Minimally dimensioned CAD drawings GD&T
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
RE: Minimally dimensioned CAD drawings GD&T
RE: Minimally dimensioned CAD drawings GD&T
RE: Minimally dimensioned CAD drawings GD&T
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 www.profileservices.ca
TecEase, Inc. www.tec-ease.com
RE: Minimally dimensioned CAD drawings GD&T
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
ht
RE: Minimally dimensioned CAD drawings GD&T
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
&
RE: Minimally dimensioned CAD drawings GD&T
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.)
RE: Minimally dimensioned CAD drawings GD&T
Jim Sykes, P.Eng, GDTP-S
Profile Services www.profileservices.ca
TecEase, Inc. www.tec-ease.com
RE: Minimally dimensioned CAD drawings GD&T
Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion
&
RE: Minimally dimensioned CAD drawings GD&T
RE: Minimally dimensioned CAD drawings GD&T
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.
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
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.
RE: Minimally dimensioned CAD drawings GD&T
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.
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
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." - Robert Hunter
RE: Minimally dimensioned CAD drawings GD&T
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?
RE: Minimally dimensioned CAD drawings GD&T
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?"
[b]Yes.[b] 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.
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?
RE: Minimally dimensioned CAD drawings GD&T
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
RE: Minimally dimensioned CAD drawings GD&T
"Good to know you got shoes to wear when you find the floor." - Robert Hunter
RE: Minimally dimensioned CAD drawings GD&T
John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
RE: Minimally dimensioned CAD drawings GD&T
OK, I think I'm finally sold on 2.8. Latest version:
RE: Minimally dimensioned CAD drawings GD&T