Is this GD&T correct
Is this GD&T correct
(OP)
Hi People!
I'm looking at a drawing and am trying to convince myself that I'm reading it wrong, but I can't. It just doesn't make sense to me and everyone I've shown it to so far agrees, but we're not confident enough with our GD&T knowledge to say it's definitely wrong, as it'll be wrong on many drawings, and dates back nearly a quarter of a century, across a number of suppliers, none of which have said, "no, that's rubbish!".
Is it logical to specify a thickness of 3.9/3.8 (so, ± 50 microns) and have a flatness tolerance band on both sides of 250 microns. I suspect that the 250 microns should be 25 microns, but am not 100% confident. I'm thinking that based on the faxt that flatness is measured between two parallel planes, that the parallel frame is not required and I could just get away with the flatness tolerance? and that the drawing is over constrained? Or am I wrong? Also do I need a datum for a flatness tolerance?
Many thanks
Simon
I'm looking at a drawing and am trying to convince myself that I'm reading it wrong, but I can't. It just doesn't make sense to me and everyone I've shown it to so far agrees, but we're not confident enough with our GD&T knowledge to say it's definitely wrong, as it'll be wrong on many drawings, and dates back nearly a quarter of a century, across a number of suppliers, none of which have said, "no, that's rubbish!".
Is it logical to specify a thickness of 3.9/3.8 (so, ± 50 microns) and have a flatness tolerance band on both sides of 250 microns. I suspect that the 250 microns should be 25 microns, but am not 100% confident. I'm thinking that based on the faxt that flatness is measured between two parallel planes, that the parallel frame is not required and I could just get away with the flatness tolerance? and that the drawing is over constrained? Or am I wrong? Also do I need a datum for a flatness tolerance?
Many thanks
Simon
Best regards
Simon NX7.5.4.4 MP8 - TC 8 www.jcb.com





RE: Is this GD&T correct
Most important question is: are you working to ISO or ASME drafting standards?
In ASME world you are most likely right: flatness normally is a refinement of size tolerance.
Things are different in ISO world though.
You appear to be working for international company, so it would be better if you clarify the rules of your office.
RE: Is this GD&T correct
Cheers
Si
Best regards
Simon NX7.5.4.4 MP8 - TC 8 www.jcb.com
RE: Is this GD&T correct
In this case the drawing is correct.
ASME is using what is called “Envelope requirement” meaning that THE ENTIRE PART is supposed to fit within 3.9 envelope but LOCAL MEASUREMENTS, say using a caliper, should be no less than 3.8.
Under said requirement obviously your flatness cannot be larger than 0.10.
ISO operates under “Independence principle” which means, as you normally use two different tools to measure thickness and flatness, your thickness LOCAL MEASUREMENT with caliper should be within 3.9/3.8, and flatness measured with indicator INDEPENDENTLY from thickness should be no more than 0.25.
Judging from the appearance of your part (sheet metal-ish) one could imagine it to maintain its thickness well, but being slightly bent. So the ISO way will actually make sense. (If you are dealing with dowel being pressed into part, Envelope requirement actually works better).
This is why you can also specify Envelope requirement in ISO and Independence principle in ASME as necessary.
If my explanation wasn’t clear enough, many people on this forum will be glad to clarify the case to you.
RE: Is this GD&T correct
Best regards
Simon NX7.5.4.4 MP8 - TC 8 www.jcb.com
RE: Is this GD&T correct
RE: Is this GD&T correct
Paul
RE: Is this GD&T correct
RE: Is this GD&T correct
But I'm not that experienced so I could be wrong
Cheers
Si
Best regards
Simon NX7.5.4.4 MP8 - TC 8 www.jcb.com
RE: Is this GD&T correct
RE: Is this GD&T correct
RE: Is this GD&T correct
RE: Is this GD&T correct
RE: Is this GD&T correct
First of all, like in ASME, its value has to be greater than applied form tolerance. In this case it obviously does not full this requirement.
Secondly, parallelism tolerance requires a datum reference. Some can say that these two leaders indicate that one surface is datum feature for the other. And okay, that could make sense, if one of the leaders was terminated by triangle and not by arrow. Since it is not, it is pretty unclear which side serves as datum feature and which is toleranced one. The print could be much more specific about it.
And finally, such way of attaching feature control frame with both - datum feature and toleranced feature - was withdrawn by ISO 1101 in 2004 edition. I do not have a copy of this standard with me right now, but I am sure you can find proper statement in one of the appendices to the document.
RE: Is this GD&T correct
I agree with pmarc that parallelism is most likely wrong. It would make much more sense if its value was greater than flatness.
If the drawing itself was prepared before 2004, not using “triangle” termination is not that much of a sin.
Long ago it meant that choosing side for a datum is irrelevant. By calling one side of symmetrical part a “datum” you would imply that that side is somehow more important than other which might not be the case.
In fact, you could actually terminate the datum symbol with an arrow, as shown on the picture.
Naturally, all of this is very, very former practice.
RE: Is this GD&T correct
Sorry, but if it was done to a previous standard, if it in-fact references that previous standard is it still "wrong"? The ASME game is not played that way. Like I said this stuff doesn't magically disapear just because the standard changes. If "they" change the rules of the game, why are the people who tried to follow it to blame, that is very bad form, IMHO.
RE: Is this GD&T correct
Much appreciated.
Si
Best regards
Simon NX7.5.4.4 MP8 - TC 8 www.jcb.com
RE: Is this GD&T correct
Yes, if the print is dated before 2004, this way of tolerance frame presentation is acceptable (I mean, assuming that the triangle is there instead of one of the arrows).
RE: Is this GD&T correct
Does your latest example come from any official ISO document?
I have ISO 1101:1983 in front of me and there is something similar shown in Table 2 and in couple of other pictures, however only as an example of toleranced feature indication.
When it comes to datum feature identification there is always triangle required (filled or unfilled). Similar-to-op technique is shown for instance in figures 36 and 37. But the triangles are there.
http://files.engineering.com/getfile.aspx?folder=4...
It is not that I nit-pick on arrows or triangles. I have been through cases when lack of proper datum feature identification, like here, created a lot of troubles.
RE: Is this GD&T correct
Like I said, it’s all things of the very distant past. Maybe it’s better that way.
RE: Is this GD&T correct
The text part is as follows:
"4.4 If two associated features are identical and there is no reason to give preference to one as a datum feature, then the tolereance is indicated as in figure 19."
Figure 19 is a parallelism callout as shown on your document.
I think it is a interesting and valid concept, myself.
RE: Is this GD&T correct
If it’s from 1976, it may be listed in the back of pmarc’s 1983 as “former practice”. I wonder…
RE: Is this GD&T correct
The only problem I have with the concept IS any reference to a datum, in the classic sense. A datum is a reference to the "a concept of perfection". I want "imperfect face" to "imperfect face", I see value in that concept, no more constrained conditions needed, just as it sits, just like the old time shop practice.
RE: Is this GD&T correct
Unfortunately I do not have a copy of replaced ISO/R 1101-1:1969 to see earlier practices.
RE: Is this GD&T correct
Sorry to hear that.
It’s just what I found in the back of 2004:
RE: Is this GD&T correct
RE: Is this GD&T correct
RE: Is this GD&T correct
What I like about your document fsincox, is that using capital letter to identify datum feature is not a requirement but rather an option.
The standard sure went a long way since that.