Major benefits of GD&T usage 6

[pmarc]

I would like to start this thread based on some thoughts that came to my mind during answering to Evan's post about surface interpretation of position tolerance:

http://www.eng-tips.com/viewthread.cfm?qid=286461&page=1

As I said there, I have a feeling that quite a lot of GD&T users (at least the ones I work with) would say that hard gaging is the only way for checking positional tolerance at MMC. But since they know it is not really possible to use gage simulators in verifying their design (let's say because there is a company strategy that prohibits hard gaging usage), they simply do not apply M modifier, even if they feel it would be reasonable or even required from functional point of view. By doing this they intentionally or unintentionally loose one of the biggest advantages of GD&T language over traditional coordinate dimensioning - tolerance zone is becoming unnecessarily fixed in size regardless of feature of size.

That's why I wanted to ask you Guys about your experience with any other important benefits of GD&T usage that you feel are not utilized properly or not used at all in your everyday's pratice.

Any remarks are really welcomed.

 

[ctopher]

I used to use GD&T everyday. Up until about 7 years ago it has been minimized to reduce cost (according to management/finance/etc). I still try to practice it, but usually I am chastised for spending too much time for using GD&T.
A lot of machinist and 'purchasing engineers' these days don't understand it anyway.
There are a lot of benefits, especially making quality and accurate parts that actually fit together like they are designed to. Unfortunately making $$ overrides quality anymore. I have heard "Send it to China, who cares about GD&T. They don't understand it there anyway".

Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion

 

[dingy2]

Chris:

There are companies that have adapted and then shelved the application of GD&T but my philosophy on its application is a bit different from most here. This may be due to the fact that I have in the past measured products with linear tolerances using CMM equipment.

If a feature has a function and mating relationship, use it. If not, linear or angularity tolerances may be appropriate.

I do agree that many people still do not understand GD&T and the 2009 edition with its various boundary conditions for datums would blow them away. I still see datum gauges using a V-cone (RFS) where the drawing reflected MMC. Training for the last couple of years has been difficult to obtain (non-existent) with some companies just starting to have a training budget.



Dave D.

http://www.qmsi.ca

 

[drawoh]

Chris:

There are companies that have adapted and then shelved the application of GD&T ...

We need to choose our words carefully here. A company can adopt GD&T, train everybody, check drawings to ensure everyone is using it correctly, and then require their fabricators and inspectors to follow the drawing instructions. The results will be better communication between the designer, drafters, fabricators and inspectors, as well as compentently prepared drawings. All this is very desirable.

Alternately, a company can purchase the standard, write a note on its drawings stating that they conform to ASME Y14.5-2009, and then continue doing everything the way they have been doing it for the last thirty years. You have manuals, and perhaps some training, but very few benefits.

On top of that, GD&T is nothing more than a language. A language allows us communicate clearly and unambiguously, however, this is not the only thing we have to do. You have to organize the drawing clearly. You have to understand the requirements of the part. When you apply the GD&T, you have to understand the manufacturing process so that you specify realistic tolerances. If the realistic tolerances do not work, you have to re-think your design. Ultimately, the ideas you are clearly communicating in the language, can be stupid.

I am not aware of GD&T being systematically taught at the college or university level. I have been told that all my co-workers understand the standard, even though I am pretty certain that they do not.

I tell people that documentation is a link in a chain. There are a bunch of other things that have to work too.

JHG

 

[dtmbiz]

And....

1994 std 5.3.2.1 this note was added....

"NOTE: In certain cases of extreme form deviation (within limits
of size) or orientation deviation of the hole, the tolerance in terms
of the axis may not be exactly equivalent to the tolerance in
terms of the surface. In such cases, the surface interpretation shall
take precedence."

 

[MechNorth]

The most fundamental, and in my mind most critical/valuable part of GD&T is the indication of how to set up a part for measurement. Even without geometric tolerances there is huge value in just being able to reliable communicate the setup for repeatability. Many other value-added aspects to GD&T, but datuming starts it all off.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[TheTick]

What I like best about GD&T is that datums are explicit. No asking "center of what?" or "which edge do I measure from?".

 

[321GO]

Quote:
"they simply do not apply M modifier, even if they feel it would be reasonable or even required from functional point of view."

I think "they" make sense by purposely excluding it.

Correct me if i'm wrong, but adding that "M" modifier simply increases production costs. Simply use a realistic (large enough)tolerance zone that you know the manufacturer can easily achieve without problems.

Then, quality control is straightforeward and fast(in the zone, ok, outside not ok). In reality the holes are in the correct position because the manufacturer can achieve them easily (which he acknowledged by quoting on your drawing). Furthermore in the unlikely scenario that they are really off, the manufacturer will nearly always accept that fact and compensate/correct his mistake (again i don't think that will happen often).

In my understanding the "M" modifier can often be avoided by aplying a realistic (large enough)tolerance zone.

I believe such "overdone GD&T" profoundly works against it.

 

[321GO]

Quote:
"Send it to China, who cares about GD&T. They don't understand it there anyway"

In fact, there is a great deal of sense in that statement( for the better or worse).

 

[Belanger]

Quote:
"Correct me if i'm wrong, but adding that 'M' modifier simply increases production costs. Simply use a realistic (large enough)tolerance zone that you know the manufacturer can easily achieve without problems."

I'd like to gently correct you on that. The "M" modifier always lowers production cost. (The only exception is the cost expended by training production personnel on how to read GD&T, but that's a different discussion.)

You can't make a "large enough" tolerance zone, because the zone that you would be talking about would have to be one designed for worst-case size (smallest hole/largest pin). The point of the "M" is to provide tolerance beyond the given amount, but only if the size of the feature is adjusted to accommodate it.

If production personnel simply ignore the "M" then they'll end up with the tolerance zone that you would have been giving them without the "M" anyhow.

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

 

[321GO]

Quote:
The only exception is the cost expended by training production personnel on how to read GD&T, but that's a different discussion."

And that is exactly what i mean with "extra costs". Someone has to to do these inspections, wether it be in/outside the company. Eithercase it will be reflect in the total costs.

Furthermore, the personel has to understand this principle also, which is often problematic.

Quote:
"You can't make a "large enough" tolerance zone, because the zone that you would be talking about would have to be one designed for worst-case size"

Yes, indeed, but what's "impossible" with that? The tolerance zone has to be based on "worst case" to start with.

 

[Belanger]

On the training aspect of the cost: agreed. (But the "M" itself doesn't increased production or inspection cost.)

On the tolerance zone size: I meant that without the "M" you'd be stuck with that tolerance amount only. But with the "M" there may be more tolerance allowed that what is stated on the drawing. That sure sounds like a cost-saving opportunity!

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

 

[321GO]

This "M" discusion somewhat refelects "the problem" with GD&T IMHO. The basic principle (a tolerance zone) is simple and intuitive, but the "bonus" zone is not. If something is not (easily)understood, it is less likely to be accepted, i.e. sooner cut for cost savings.

Again, with current (accurate)CNC machining and a realistic chosen tolerance zone, i don't see the need.

 

[Belanger]

Once you learn how and why the "M" is used, I think you'll find it to be a cost saver and actually quite intuitive based on fit/function of parts.



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

 

[321GO]

But i was also alluding to fact of general acceptance/practicality of GD&T.

The modifier is well understood between GD&T inspectors on the floor, but difficulties arise when "higher up" needs to be involved in case of problems.

The modifier "forces" these managers with a concept that is IMHO not that intuitive, thus creating (some) frustration and in the end not helping the acceptance of GD&T, sort of.

 

[drawoh]

...

Again, with current (accurate)CNC machining and a realistic chosen tolerance zone, i don't see the need.

I keep claiming here that any idiot can produce functional machining drawings. Machining is accurate enough to make most parts work without any special effort by the machinist.

This is true, even of the drawing is hopeless crap. At some point, the machinist can assume the drafter is an idiot. They can make the part to the nominal dimensions to machining tolerances, and no one will be the wiser.

When you get into sheet metal, castings and weldments, the standard drawing tolerances are more accurate that what can be achieved by the fabricators. Now, you can screw up badly. If you cannot apply realistic tolerances to your drawings, you cannot do a tolerance stackup, and identify and fix design problems. You cannot identify the one or two really critical tolerances the fabricator may be able to hit if were taking your drawings seriously.

JHG

 

[321GO]

Yes, of coarse tolerances are different for machined vs. casted parts, there are two seperate standards (at least here in Europe). DIN-ISO-2768(part 1) for machined dimensions and DIN ISO 8062 for casted dimensions.

 

[pmarc]

I have to say the discussion went in very interesting direction.

Based on my experience I can tell you that I dealt with numerous applications where standard (or whatever we call them) tolerances were not enough to assure part's functioning. Manufacturer received from design dept. drawings with easy-to-achieve tolerances and was very happy of that but the produced detail did not function properly in assembly and re-work was necessary.

What I mean is that very often designers must define narrow tolerances (tighter than preffered by manufacturer) to fulfill part's function. And this is a place for M modifier and all other GD&T things which seemingly look to be "cost raising". They help manufacturers in situations when tight tolerances are difficult to meet.

So I have to fully disagree with the statement that: "<M> modifier simply increases production costs". This is one of the myths which probably stems from poor GD&T knowledge amongst people involved in development of different types of products (designers, manufacturers, inspectors, managers etc.) and is repeated very often.

It was also nice to read that every idiot can produce functional machining drawings Quite interesting point of view...

 

[321GO]

drawoh:
" I keep claiming here that any idiot can produce functional machining drawings."

I'm baffled to see somebody with practical experience make such a statement.

Furthermore, I was trying to make the case that the M modifier is less important when there is a large diameter differences between the holes and bolts. When not, it DOES make sense, i never said it did not.

I tried to state these different bewteen such situations, but discussion is pointless sad to say, i won't further participe.

 

[drawoh]

321GO,

The diameter difference and the positional tolerance should be under your control. If you have one, but not the other, you are in trouble.

Problem:
Specify a tapped hole and a clearance hole for an M6 screw clamping a thin plate to a base.

I call up an M6X1 H6 hole with a positional tolerance of Ø0.3mm. I do not bother with MMC/MMB here because the bonus tolerance does not help me assemble the thing. If I had some of the inspection tools described above, I might look into it.

My clearance hole will be positioned to zero, at MMC/MMB. This means that my perfectly located hole must be just big enough to clear an maximally inaccurate screw. I need to clear Ø6.3mm, and I add a little in case the tapped hole is not perfectly perpendicular. I could have added a projected tolerance to my tapped hole. My minimum hole is Ø6.4mm. My maximum clearance allows for maximum error in location and drilling. I allow 0.5mm for drilling, and 0.3mm for a positional tolerance. My maximum hole is Ø7.2mm.

I have never discussed this with our machine shop, but I have one complaint only about tolerances like this. He accepted my explanation. Obviously, I do not anticipate receiving a part with a hole that measures Ø6.4mm.

If I do not call up MMC/MMB, I must specify a feasible positional tolerance, how about Ø0.3mm? My smallest hole must allow for this, plus a small safety margin. Ø6.7mm. My large hole accounts for the drilling accuracy. Ø7.2mm.

The zero positional tolerance provides a larger, more flexible error budget.

JHG