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]

I can't help but wonder if the premise of the question is fundamentally flawed. (I'm not picking on you, Swisscheese, but the practice which I gather someone else is foisting upon you.)

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

 

[swisscheese]

I don't think it is fundamentally flawed but perhaps we need to clarify that the objective is how to interpret Reduced Dimension Drawings. Here is one discussion that might help clarify the issue and shows that large companies have worked on this:

http://www.solidmuse.com/2007/01/reduced-dimension-drawings-part-1.html

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

 

[TheTick]

Use the same tolerance everywhere, except where you need something different.

 

[fcsuper]

In your notes or title block, you can use the Profile GD&T callout with the ALL OVER modifier. This applies the Profile tolerance to the entire model equally.

Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion

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

 

[fcsuper]

BTW, for that, you'll need to invoke ASME Y14.5-2009 on your drawing. (ASME Y14.5M-1994 has a much more limited definition of ALL OVER that wouldn't work in this case, IMO.)

Matt Lorono
Lorono's SolidWorks Resources & SolidWorks Legion

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

 

[drawoh]

swisscheese,

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.

JHG

 

[321GO]

Fine, you want to save some time on the drawing part of the job, but you still need to be able to do quality check on the finished product, don't you?
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..

 

[KENAT]

MBD and the like has been discussed a few times, maybe some of those threads will help you out.

thread1103-239768 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.

Posting guidelines faq731-376

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

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

 

[ewh]

I guess I'm confused as to what is at issue here... RDD have been around for several years now without bringing companies to a standstill. As noted above, RDDs are valuable when defining irregular parts. Keep in mind that RDD means "reduced dimensions", not "no dimensions".
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." - [small]Robert Hunter[/small]

 

[Belanger]

I think the OP's question is this: Suppose we have a design with no specified dimensions -- just a default plus/minus, as in the old title block tolerance that has been around for decades.

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

 

[KENAT]

Having had a quick look at the link the OP gave, and one of the examples there-in, I see your point Belanger and they may be talking literally +-.

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.

Posting guidelines faq731-376

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

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

 

[swisscheese]

Thanks for the many comments but let me clarify what I am looking for. Perhaps Reduced Dimension Drawings is not the right term. The reality is that many of our orders from customers ranging from experienced engineers at space agencies down to individual inventors provide NO explicit dimensions. The eMachineShop CAD provides a field for general tolerance and all customers specify a value - say +/- .005. We inspect parts against that tolerance using certain rules about how to apply the tolerance for accept/reject. We would like to align those rules to what others are doing in the industry who have adopted RDD or perhaps NDD. Perhaps what is unusual with us and part of the confusion is that we encourage not only RDD/NDD but we provide the associated rules for how the general tolerance is used when explicit dimensions are not provided.

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.

 

[drawoh]

swisscheese,

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...

[ol]
[li]You will meet all dimensions and tolerances specified on the drawings.[/li]
[li]In the absence of a specified dimension and tolerance standard, you will interpret drawings as per ASME Y14.5M-1994 (ASME Y14.5-2009?)[/li]
[li]In the absense of specified dimensions, you will fabricate to the CAD model.[/li]
[li]In the absense of specified tolerances, you will position holes to Ø0.3mm, and hole profiles to 0.6mm[/li]
[/ol]

Modify units, numbers and standards to suit you, and get your lawyer to translate everything into legalese.

How about that?

JHG

 

[321GO]

swisscheese,

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"

 

[ewh]

We are often in the position where we have to send a tooling vendor just a model file along with a statement of work, which specifies critical dimensions/tolerances. As for the rest of the design, we rely on the vendor to design the tool around the function.
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." - [small]Robert Hunter[/small]

 

[fcsuper]

There is no industry standard for this. Y14.41 is useless.

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

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

 

[dingy2]

Matt:

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.

http://www.qmsi.ca

 

[KENAT]

dingy, it typically applies 'unless otherwise stated'. Any features that require different tolerances should be appropriately detailed.

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.

Posting guidelines faq731-376

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

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

 

[dingy2]

Kenat:

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.

http://www.qmsi.ca