Question regarding Datum and tolerances on it as well as feature
Question regarding Datum and tolerances on it as well as feature
(OP)
I have a heat sink with 3 plateaus. I used a Flattness call out of 0.30mm and named that my Datum A.
Now I have additional features which I want to have a tighter tolerance of 0.02mm wrt Datum A.
Does the feature tolerance become insignificant because Datum A has a larger tolerance? Or does the feature tolerance become "with respect to" whatever plane datam A lies on?
Now I have additional features which I want to have a tighter tolerance of 0.02mm wrt Datum A.
Does the feature tolerance become insignificant because Datum A has a larger tolerance? Or does the feature tolerance become "with respect to" whatever plane datam A lies on?





RE: Question regarding Datum and tolerances on it as well as feature
Believe it if you need it or leave it if you dare. - Robert Hunter
RE: Question regarding Datum and tolerances on it as well as feature
Are you sure of that or might you want to rethink it?
If the Standard applied it Y14.5, I do believe that the referenced surface will have to be flat within .02 to satisfy the parallel requirement of .02.
RE: Question regarding Datum and tolerances on it as well as feature
Mike Halloran
Pembroke Pines, FL, USA
RE: Question regarding Datum and tolerances on it as well as feature
We had a similar situation recently and I put together the attatched. It's a compiled extract of ASME Y14.5, I hope I'm not massively breaking any copyright issues, if so administrator please delete the link or whatever works.
KENAT, probably the least qualified checker you'll ever meet...
RE: Question regarding Datum and tolerances on it as well as feature
The refinement of 0.02mm would be confirmed while setting on the 'high points' of datum -A-.
RE: Question regarding Datum and tolerances on it as well as feature
Hope this clears things up for you all! Additionally, I really have to question the .3mm form on a datum (foundation)when other features w.r.t. are specified to less than 10% of that. Seems like you could be asking for trouble. Upon performing a stack analysis on the assembly this may be also show up as a contributor.
I would advise evening them out a bit and if any thing make the Datum form tolerance tighter.
RE: Question regarding Datum and tolerances on it as well as feature
However weavedreamers last paragraph matches my understanding.
KENAT, probably the least qualified checker you'll ever meet...
RE: Question regarding Datum and tolerances on it as well as feature
RE: Question regarding Datum and tolerances on it as well as feature
Now that we have established datum A, is it practical to have parallelism (assumed) of another surface 0.02 to datum A? It depends on how large of an area that the other surface covers. It would not be practical to have the relatively tight tolerance if the other surface is the same size as datum A. If the other surface is rather small in comparison to datum A, then maybe 0.02 would be appropriate.
I might suggest that datum targets are placed on datum A to at least give some sort of consistency of measurement.
Dave D.
www.qmsi.ca
RE: Question regarding Datum and tolerances on it as well as feature
I re-thought my post just after I submitted it, but was called away to fight other fires, and wasn't able to re-address it until now.
I agree that the actual Datum A is a perfect plane established by the three highest points on the surface, and any feature referring to A is actually referring to that plane.
Believe it if you need it or leave it if you dare. - Robert Hunter
RE: Question regarding Datum and tolerances on it as well as feature
RE: Question regarding Datum and tolerances on it as well as feature
As a general statement, the feature tolerance does not become insignificant when the datum feature has a larger tolerance. If Datum Feature A has a flatness tolerance of 0.30, the considered feature can still have a parallelism tolerance of 0.02. There is not really any relationship between the two numbers.
As has been pointed out, the datum is a perfect plane that contacts the high points of the datum feature (i.e. the tangent plane, physically represented by a surface plate).
The form of the datum feature becomes significant when trying to establish the datum. If the datum feature is convex, the part will rock on the surface plate (have three-point contact in more than one way). There will be more than one tangent plane, and hence more than one possible datum (these are called "candidate datums" in ASME Y14.5.1). The parallelism tolerance zone is defined to be parallel to the datum, so its relationship to the considered feature changes as the part is rocked.
The form of the datum feature is often controlled in an effort to minimize the possible extent of rocking and datum instability. Alternatively, datum targets are specified. The part would rest on three pins or tooling balls instead of a surface plate. This allows a very stable and repeatable datum to be established from a very imperfect datum feature. So you could have a datum feature that was flat within 0.5" and machine a surface that was parallel to it within 0.0001".
Evan Janeshewski
Axymetrix Quality Engineering Inc.
www.axymetrix.ca
RE: Question regarding Datum and tolerances on it as well as feature
For the surface being controlled to the tighter tolerance I agree with others that parallelism wrt -A- is probably the way to go.
KENAT, probably the least qualified checker you'll ever meet...
RE: Question regarding Datum and tolerances on it as well as feature
Your primary plane datum is defined by ASME Y14.5M-1994 as the three points of your surface that make contact with a flat plane. I am not sure what happens if your face is convex.
Given the above definition, and a datum flatness of 0.3mm, you can apply a profile tolerance of 0.04mm (+/-0.02mm) to a surface, with respect to the datum. It makes sense to me, and it is inspectable.
Whether or not this is good design practise, is another matter. The geometry is a little weird, and it may not be what you think it is. What are you trying to accomplish?
JHG
RE: Question regarding Datum and tolerances on it as well as feature
I am not terribly picky about where my 3 pads are with regard to height. I am more concerned that they are all coplaner. The 3 gap setting islands on the other hand, I have to hold a very tight tolerance on since the dimension itself is 0.07mm. << hense the 0.02mm tolerance.
I'm not sure how "right" this is with regard to GD&T, but after speaking to a collegue about it, he understood what I wanted from the drawing. I am going to try to chat with the supplier to ensure they know what " I want..."
Thanks for all the answers >> a lot just confused me more, but most made sense.
The whole problem pretty much arrises because I do not want to put any tight tolerances where they are not necessarily needed. I would like to get away with no machining on a Cast part. Weather this works out or not...
RE: Question regarding Datum and tolerances on it as well as feature
Attatched a very simple sketch showing what I meant.
By the sounds of your last post too simple to be much help.
KENAT, probably the least qualified checker you'll ever meet...
RE: Question regarding Datum and tolerances on it as well as feature
Basically once the datum feature is created, the tolerance for other features are independant of the datum tolerance?
RE: Question regarding Datum and tolerances on it as well as feature
See the attatchment to my first post above which explain parallellism in this context.
Attatched is a corrected sketch.
KENAT, probably the least qualified checker you'll ever meet...