GDT on machined extruded part 1

[rkrz]

We are making parts out of extruded stock and trying to redo the prints with GDT.
The part is machined all around and we want to use 2 holes as the secondary and tertiary datums.
However it is not a flat plate as usually shown in the ASME standard, and the hole (datum) needs to be controlled to the extruded 'step' to be in the right (y direction), with everything else being called back to it.
Attached is an example.
Would it make sense to instead just give a start +- on the 28.75 reference dimension to the 25mm hole and then use positions/profiles from there?
Just want to learn how to tackle this.

Thanks.

 

[Wuzhee]

You should absolutely not define tolerances on reference dimensions.
Be aware also that "stock" owerwrites ASME Rule #1.

I'd make the large hole Datum B and the small middle hole Datum C then profile the contour and position the holes to it.

 

[rkrz]

In that case how is the position of the large hole controlled. If it was a flat plate, it makes sense, but it needs to be in a certain position relative to the step down. Hence my thought of changing the ref dim to a toleranced dimension to the step.

The stock is just a reference, I agree its not part of the standard, and I don't want to take the B datum off the stock. I am just trying to figure out the best way to define the part.

 

[Wuzhee]

Not knowing your manufacturing processes one would suggest define several functional datums for manufacturing steps.
Is it steel, alloy, plastic, what?

Datum B would be machined away right at the start. So it's more like a functional datum to create a flat plane on which you can orient your part (I guess datum A is done by face milling).
To this Datum B you can call out the large hole, then the rest. This is what's on the drawing right now.
But to answer your question -

In that case how is the position of the large hole controlled.

if the large hole is Datum B then you drill wherever you want the large hole then drill the second smaller hole and you can locate your part with a flat plane and two pins for the rest. You locate FROM the large hole. Manufacturing wise I'd choose this option, but not knowing the function of the part there's several possible solutions to choose from

 

[Burunduk]

Datum B is from a feature that is gone by the time the drawn part is ready for inspection? Probably you try to make it comfy for the machinist but that probably shouldn't be your main concern if you try to define a part to make it work.

It's not recommended to try to capture a specific multistep manufacturing process in the dimensioning and tolerancing of a final product. Take into consideration how this part is being used and derive the datum definition and tolerancing scheme from there.

 

[rkrz]

The raw material is a 5m long aluminum extrusion that we put through an extrusion milling center, about 100 of these pieces come out of 1 piece of raw material. The front and back faces are extruded material and not machined, the outer profile and holes are all that is machined.

The significant features are the large hole and the bottom half circle profile.

The only thing I am having trouble figuring out how to tolerance is the large hole. If it should be datum B, where is it located in reference to the step that is there in the raw material, which we do not touch. Maybe make the step a datum? at least temporary before defining the holes as datums.

If i machined that step I could just put a profile to the step back to A and the large hole (datum B in that case). With The datum B circle being only called back perpendicular to A. Would it make sense to do this if it is not machined?

In summary, how do I define the position of the large hole?

 

[ctopher]

I agree with others.
Try to think about how will this part be inspected.
Datum B will not be there, so can't inspect it's features.

Chris, CSWP
SolidWorks
ctophers home

 

[DGN1975]

it doesn't matter if a feature is machined or not to use it as a datum or dimension to it. the example you gave I don't see the holes toleranced to the step at all as the 28.75 is just a reference.
I would just add a tolerance to the 28.75 step to the large hole or you could add a surface profile to the right view to control where the step is to the large hole. The current datum B needs to be removed.
Use the Current ACD as DRF.

 

[ewh]

I agree the above regarding phantom datums. Wuzhee's first suggestion, with the addition of [edit] removing the reference from and [/edit] making the 28.75 a toleranced dimension (whatever tolerance you determine necessary) seems the simplest course of action.

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV

 

[Burunduk]

The best way to define position for the large hole depends on how the part is used. Weather to define position for it at all or control it for orientation only and define the position of other features relative to it also depends on it.

Edit: the question I answered here was deleted by the time I submitted the post (like datum feature B was removed by the time the part being toleranced to it is finished).

 

[Belanger]

You should absolutely not define tolerances on reference dimensions.

An interesting side note about this... the Y14.5 standard doesn't say that it's absolutely not allowed. From paragraph 3.28: A reference dimension is "dimensional information, usually without a tolerance."

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

 

[Burunduk]

Belanger,
I would say that it only makes sense to specify a reference dimension in the following cases:
1. The variation permissible for that dimension is a stack of other tolerances specified on the drawing,
2. The tolerance for that dimension already appears in another view on the same drawing.
3. The tolerance is in a referenced document (such as the drawing of the casting the part is made of) - and I personally don't like that scheme.

 

[Belanger]

I didn't editorialize whether it's good or bad.
I just clarified that it's not "absolutely" true that ref dims shall not have a tolerance.

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

 

[jassco]

Hi, Belanger:

Could you give an example to show application of reference dimension with tolerances? I am yet to see such a thing.

Best regards,

Alex

 

[Belanger]

Hi Alex -- see the attached graphic.
I must emphasize that I am not in any way championing a toleranced basic dimension. I merely pointed out that the standard includes the word "usually" and there is presumably a reason for that word.
In my impromptu example, 11.3 ± 0.2 is shown in parentheses. Perhaps that distance across the panel was achieved in an earlier operation, and now the brackets are cut to length and formed into shape. Maybe they include the reference dim so that we know the approximate distance, but it's not a pass/fail criteria for this drawing.
(And yes, I know we shouldn't use ± tolerancing for location, etc. etc... but it's just an example to address the question at hand.)

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

 

[Belanger]

This post should contain the graphic -- not sure why it didn't work on the previous post.

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

 

[jassco]

Hi, Belanger:

Where did you get this screenshot from? It makes no sense to me.

Best regards,

Alex

 

[Belanger]

Alex, let me know what in particular is bothering you about the example. Are you referring to the drawing in general (I have no idea what the part is)?
Or are you referring to the reference dimension?

Perhaps I'll turn it around toward you: Is the example I gave violating Y14.5 by using that style of reference dimension?

I'll say it once again -- I am not endorsing toleranced reference dimensions. I am only showing one pictorial interpretation of the word "usually" that we see in paragraph 3.28 of the standard.


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

 

[jassco]

Hi, Belanger:

I respect you a lot. But for this one, I have to disagree with you. This dimension (11.3+/-0.2) bothers me in these two areas:

1. A reference dimension with tolerance;
2. A positional tolerance associated with a reference dimension.

I was aware of Section 3.28 ("Dimension, Reference" - ASMY Y14.5-2018). I also saw the same statement in ASME Y14.5-2009. I think this is a mistake.

Reference dimension is used for REFERENCE PURPOSES ONLY! In another word, removing reference dimensions from a print shall not affect definition of the product. Using the same ASME Y14.5 language, a reference dimension does not govern production or inspection.

Best regards,

Alex

 

[Belanger]

Hi Alex,
First of all, that position tolerance only relates the two holes to themselves and to datum A. The ref dim has nothing to do with the position callout.
Second, you take issue with a reference dimension having a tolerance. But the standard clearly says that a ref dim is usually without tolerance. That leaves wiggle room for a ref dim to have a tolerance. You can call it a mistake, but there's nothing intrinsically wrong because the parentheses essentially nullify any tolerance inside them.
Related to that, yes I agree that a ref dim is for reference purposes only. With that in mind, a ref dim can have extraneous information attached to it (such as a tolerance) but since it's all for reference purposes only, it has no bearing on the drawing we're looking at. The ref dimension could indeed be removed from this drawing and it has no effect on the product nor its inspection (see my point #1 about the position FCF).


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