Recommend a GD&T
Recommend a GD&T
(OP)
So we have this part fabricated from 7075-t6 aluminum. It a 4"x6" flat plate. Because of the all the machining the part becomes warped. So on the detail drawing I want to specify a GD&T. I've read through numerous books and it seems that a straightness tolerance is the one to useo rpossibly a flatness.





RE: Recommend a GD&T
When the people fear their government, there is tyranny; when the government fears the people, there is liberty. - Thomas Jefferson
RE: Recommend a GD&T
RE: Recommend a GD&T
RE: Recommend a GD&T
RE: Recommend a GD&T
When the people fear their government, there is tyranny; when the government fears the people, there is liberty. - Thomas Jefferson
RE: Recommend a GD&T
Read pages 157-161 of Y14.5M-1994 to see the differences---single individual elements for straightness vs. all elements (whole surface)for flatness.
RE: Recommend a GD&T
Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated Jul 13, 2008)
RE: Recommend a GD&T
The flatness or straightness call-out depends on the amount or warpage you are can allow and the material thickness tolerance. Remember rule #1 (perfect form at MMC). If the plate spec is .25±.01 thick, when the part is produced at .26, it must be perfectly flat. When the part is produced at .24, the part is allowed to warp by the difference between the actual thickness and the MMC: .02.
If you need the part flatter than .02, then you need to specify a flatness tolerance on one side and maybe a parallelism tolerance on the opposite side. The flatness tolerance spefication cannot exceed the thickness tolerance; anything more that .02 flatness will be incorrect (in my example). If the part is allowed to warp more that .02, you need to specify straightness to the feature of size (thickness)dimension. This will allow you to violate rule #1.
For comparison, if the part had a .01 flatness requirement,
when the part thickness is:
.26, flatness must be .00 (perfect per rule #1)
.25, flatness must be .01
.24, flatness must be .01
If you specify a .01 straightness to the thickness dimension, when the part thickness is:
.26, flatness must be .01
.25, flatness must be .01
.24, flatness must be .01
If you specify a .03 straightness to the thickness dimension, when the part thickness is:
.26, flatness must be .03
.25, flatness must be .03
.24, flatness must be .03
I hope this helps.
JV1
RE: Recommend a GD&T
I disagree,
Rule #1 does not apply to flatness since it is a surface form control... (at least it does not yet with ASME Y14.5M-1994 but possibly with ASME Y14.5M-2XXX if flatness (M) is permitted to apply to a FOS "thickness").
Straightness although can be applied to a planar FOS in the current ASME standard by specifing it under the size callout. You are correct that it is a constant value if no (M) is specified in the tolerance but it is a variable value if the (M) is specified.
In your examples Rule # 1 does apply to size so a 0.25 +/- 0.01 thickness would be limited to 0.26 "perfect form at MMC" and flatness constrained to its limit on the specified surface(s).
Straightness (M) is not constrained by Rule #1 therefore if the straightness was applied to the size callout and thickness 0.25 +/- 0.01 and straightness tolerance was 0.03(M) then the overall effctive thickness would be 0.25 +0.01 +0.03 which is 0.29.
With straightness applied to the size without (M) the overall effctive thickness would be limited to +0.03 above the actual maximum thickness.
Paul
RE: Recommend a GD&T
I would suggest, like the others, that you apply a flatness tolerance on the surface.
Dave D.
www.qmsi.ca
RE: Recommend a GD&T
It occurs to me the question none of asked directly is, "is your warpage exceeding the size tolerance of the 4 X 6 part"? What warpage your design stand and still be functional is going to determine if you go with flatness (prefect form @ MMC) or straightness @ MMC with a staightness limit you can live with.
RE: Recommend a GD&T
If the fabrication is welded then that maybe one of the reason's for the distortion, as well as using GD&T you might want to look at stress relieving the part before final machining.
Regards
desertfox
RE: Recommend a GD&T
Just a secondary point. If your surface you want to control the flatness on is interupted, then you would need to use the profile callout without any datum reference. Also you will need to callout how many surfaces it applies to.
Jeff
RE: Recommend a GD&T
JV1, good explanation above.
Jim Sykes, P.Eng, GDTP-S
Profile Services www.profileservices.ca
TecEase, Inc. www.tec-ease.com
RE: Recommend a GD&T
I'm looking at 6.5.6 & 6.5.6.1 of ASME Y14.5M-1994 and don't see where it says you have to have the phantom line or that the FCF has to point at it.
Certainly it is shown that way in the examples (figs 6-20 & 6-21), and I can see that otherwise there'd be potential for confustion but I don't see it explicitly stated.
Where I had a part with something like 100 faces (interupted by small grooves) that were nominally coplaner I didn't show the phantom lines, just the number of surfaces below the FCF.
Is this a case where for it to be an individual requirement you'd have to explicitly state this?
KENAT,
Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently?
RE: Recommend a GD&T
Fig. 6-21 shows the relationship (phantom) line between the individual surfaces, and the two datum surfaces being coplanar by means of leaders directly to the surface. In this instance, where the features are separated by other features, the only option would be to use leaders directly to the surfaces. The two center surfaces are shown coplanar & located wrt the datum by means of the leader directly to the phantom line.
So, as long as the leader goes to the phantom line relating the features, or the leaders go to all of the related features you would get the same meaning.
The problem that I see most often is that someone will use (1) flatness on 2 surfaces thinking that they get coplanarity, or (2) a surface profile on an extension line leading to only one surface, which leaves it ambiguous as to which surfaces are intended.
Tks for keeping me honest, Kenat.
The situation you mention is fairly common. I've dealt with it in a few ways; without the phantom lines,
(1) add a note "ALL SURFACES AT THIS LEVEL", if all surfaces at that level are to be included,
(2) after indicating the number of surfaces add a note "MARKED 'X'" or "EXCEPT MARKED 'X'", when only some of the surfaces are to be considered,
(3) combinations and variants of 1 & 2, which describe which features are to be considered / excluded.
Also, the same methodology can be used to control the co-cylindricity of nominally-cylindrical coaxial features.
Jim Sykes, P.Eng, GDTP-S
Profile Services www.profileservices.ca
TecEase, Inc. www.tec-ease.com
RE: Recommend a GD&T
Another frequent case is Fig 4-20, interrupted surfaces, picture wanting a coplanarity on these surfaces.
Could do it by flatness, datum B to datum A, but maybe Profile, 2 surfaces like Figure 6-21 also? Maybe not from an inspection point of view. What do you think?
RE: Recommend a GD&T
I thought I'd done really well to use surface profile instead of flatness and then you bring the phantom line thing up
There was no way I could use phantom line in my case, the item was only 12" OD and had like a spider web pattern of small grooves. However your note (1) may have been a good idea.
I'm not sure I'm going to go force a rev of the drawing but I'll keep it in mind for next time.
Thx
KENAT,
Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently?
RE: Recommend a GD&T
For Fig 4-20, you'd have to establish flatness on whichever was to be the primary datum (A?), and then locate the secondary (B?) to the primary by a surface profile wrt Datum-A. In fact, on Fig. 4-20, there is no indication of a coplanarity requirement, so the surfaces could be stepped (by design) by 5mm, and you could still (theoretically) use compound datum plane A-B.
Sorry about the Cheerios, Kenat. Buy you a round at the pub to make up for it?
Jim Sykes, P.Eng, GDTP-S
Profile Services www.profileservices.ca
TecEase, Inc. www.tec-ease.com
RE: Recommend a GD&T
True, Fig. 4-20 just covers A-B datum plane, and not necessary the alignment of the surfaces wrt each other, but obviously I was thinking of in-line surfaces with a feature between, and using that picture as an example.
I guess I would also prefer your suggestion of flatness on datum A & profiling datum B surface wrt datum A, rather than specifying profile similar to Fig. 6-21 (the double arrow callout).
RE: Recommend a GD&T
Jim Sykes, P.Eng, GDTP-S
Profile Services www.profileservices.ca
TecEase, Inc. www.tec-ease.com
RE: Recommend a GD&T
So I take it then that my interpretation of the standard is correct as I stated above. I've re-read 6.5.6.1 and my brief explaination above still seems valid to me. Of course additional information shown on the drawings to correctly establish which surfaces you're talking about in the callout are definitely valid and required for accurate assessment. Your method you described is what is shown in fig 6-20, but I'm sure there are other creative methods that might be used based on the uniqueness of the geometry itself.
RE: Recommend a GD&T
Jim Sykes, P.Eng, GDTP-S
Profile Services www.profileservices.ca
TecEase, Inc. www.tec-ease.com
RE: Recommend a GD&T
RE: Recommend a GD&T
I've been on the receiving end a few times, don't let it get to you.
KENAT,
Have you reminded yourself of FAQ731-376: Eng-Tips.com Forum Policies recently?
RE: Recommend a GD&T
It's funny that I never did call it flatness if it is an interupted surface, and we don't even know if the original poster had an interupted surface. Oh well at least there are a lot of references to the standard and people can figure it out for themselves.
Jeff
RE: Recommend a GD&T
One of the problems with this kind of forum is that what we type and what the readers interpret aren't always the same; there's a lot of subtleties in the spoken language that aren't picked up in text. I got corrected twice yesterday for stupid things (stupid as in on my end) where I'd left things open to interpretation or used common terms instead of proper ones.
Welcome to the club.
Jim Sykes, P.Eng, GDTP-S
Profile Services www.profileservices.ca
TecEase, Inc. www.tec-ease.com