Ordinate 0,0 NOT at a datum? 3

[pinsNpads]

This is not how I would prefer to detail a part, but there is a specific motivation I won't go into.

What I have is a large part with many features. I have 3 datums selected (a plane, and two bores). The part is round and neither of the bore datums has axis at the center. Now, for a few reasons, people would like to see ordinate dimensions with 0,0 at the center of the part even though the positional tolerances reference A, B, and C which are unrelated (except by basic dims) to the center. Is this OK? I'd rather put 0,0 at my Datum B, but that causes other logistical problems. Any help is appreciated

 

[TheTick]

Is there an actual feature at the center to dimension from, or is it the theoretical center?

 

[pinsNpads]

It's a round part with a round bore in the middle (approx 24" bore). The issue is that the round bore is just clearance and is not critical to part function and so I'd like to not have it be datum. The other (smaller ~ .5") bores are not at center but ARE critical to part function and serve as alignment features. People like 0,0 at center to easily be able to confirm location of critical features relative to other parts in design reviews (among other reasons).

 

[ctopher]

Take it to inspection an the machine shop and ask them if they can locate and measure 0,0 at center, with dims located basic to the center.

Chris
SolidWorks/PDMWorks 08 2.0
AutoCAD 06
ctopher's home (updated 10-07-07)
ctopher's blog

 

[TheTick]

As long as the GD&T places the features w.r.t. the correct references, the 0,0 location shouldn't really matter. I do get bugged when 0,0 is "in space", in the center but not on a feature.

 

[PaulJackson]

I agree with TheTick. An (0,0 basic linear dimensional reference) ... does not a datum make. The coordinate system that is constructed using datum features A|B|C would put a 0,0 reference point where the axis of B's AME (actual mating envelope) intersects with A... oriented for rotation relative to C. The 0,0 reference must then be translated to what appears to be the center of the part using datum feature B's basic dimensions and all diameters that are shown coaxial with the (0,0 basic linear dimensional reference) will then have X and Y displacement error from 0,0.

 

[TheTick]

editorial comment...

It does seem a bit senseless, however, to not have 0,0 correspond w/ primary datums.

 

[ctopher]

pinsNpads,
I was curious what your inspection and machine shops would say.

Chris
SolidWorks/PDMWorks 08 2.0
AutoCAD 06
ctopher's home (updated 10-07-07)
ctopher's blog

 

[Xplicator]

This is always hard when I don't know the whole story and I may be wrong, but here is something to chew on.

It seems to me that the wrong functional primary DRF is being specified here since there is such a strong desire to have an origin separate from the current specified DRF. Additionally, maintaining an assembly clearance implies to me a functional requirement.

So I ask a question and suggest a possible solution. The question is whether you have considered adding an axial datum to the main bore feature defining the center of the part and utilize multiple DRF's or not? If not please see, Para 4.5.11 and 4.5.11.1 in the standard.

Last but not least, combining methods will surely lead to problems. I suggest pick one or the other, never both. My preference is GD&T.

 

[axym]

I agree with TheTick's first response, and with PaulJackson, that the XYZ coordinate system origin in the model or drawing can be put anywhere. The origin doesn't have to correspond directly with the datum features, and it often can't. With many datum feature configurations, patterns in particular, there is no unique "logical" location for the (0,0) origin. It's arbitrary.

The reasons for requesting the XYZ origin at a certain place often have nothing to do with part function - they are usually something to do with convenience for NC programming, fixture reference, or something like that. But that's not a problem - put the XYZ origin wherever they want it. That's the beauty of GD&T and basic dimensions - you can lay them out in whatever coordinate system you want, and it's all equivalent.

Having said that, all of this only works if the distinction between datum features and features at the (0,0,0) origin is understood properly by all concerned. If the inspection report shows a hole that is nominally (0,0) with actuals of(0.003, -0.005), this can be counter-intuitive if you're expecting datum features to always be at the origin (as some machine shops might).

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[pinsNpads]

Thanks for the responses. I think this confirms my thought which was that I could have 0,0 wherever it "needs" to be even if that is not a datum which will be used to locate critical features. I think this introduces the possibility for confusion by vendors, but my alternatives are worse in this case!

 

[drawoh]

pinsNpads,

One of the functions of your datum is to provide fixturing for manufacturing and inspection. If you use a sloppy feature as a datum, you make fixturing difficult.

Definitely, you should use your bores as datums.

JHG

 

[PaulJackson]

If |B| and |C| were both dowels...aligning and locatiing one part part to another... and if the dowel hole and dowel pin sizes (clearances) were identical for both... then both dowels could be designated |B| with a 2X size, and pattern position to |A| (controlling the spread and perpendicularity to |A|).

Also if the center of the dowel hole pattern then was symetrical with the other coaxial diameters (although it does not need to be) then the origin 0,0 produced from the dowels (midpoint between the spread) would not need to be translated and may more functionally reflect the assembly location and orientation between the structures.

This is how many powertrain component dowel interfaces are specified.

Paul

 

[Xplicator]

Again with out the whole story everything is merely speculation.

pinsNpads I really don't believe your alternatives are worse, I know if I had more information that this could be easily defined unambiguously using GD&T. I am wondering if this DRF that you speak of (a plane and 2 bores) observe the mutual perpendicular plane requirement. If it does, possibly use of PaulJackson speculation of your situation having a pattern, to use as a datum feature could be utilized by you.

drawoh, be aware the variable size used to simulate the datum on jigs/fixtures/gages comes from the actual FOS relating to the datum feature, not the size of the mating component. Unless MMC/LMC is used in which case a fixed datum feature simulator is used; if it fits it's functional, end of story.

 

[pinsNpads]

I'm not really trying to withhold information, it just seemed more interesting to discuss it without getting bogged down in the specific details of my example. The two bores which I'm going to call B and C are not the same size. They are sized to press fit off-the-shelf round and slotted bushings. I could have an additional set of datums, but to my knowledge that would add possible variation to the features I care about (at least any way I can think of it) in that variations in the datum reference features would affect the location of B and thus any features referenced off of B.

There seems to be a LOT of confusion propagated here. I'm NOT avoiding using GD&T. I am, in fact, using it. If I had my choice, I'd have 0,0 at Datum B and move on with life. Several people where I work don't want this as it make checking drawings for basic fit and "checklist" reviews more difficult. The unfortunate result of this thinking is drawings with datums chosen really really poorly. Datums which have NO functional importance whatsoever.

 

[pinsNpads]

here's (assuming this works) a pic of an approximated version of the part we're discussing. I've simplified and modified things a bit. The dims I've put on here are just for the sake of conversation.

 

[KENAT]

My suggestion/vote: pick your datums based on function with a nod to inspection and without unnecessarily making it difficult for manufacturing but without pandering either.

I've been having similar headaches and at the moment I've pretty much given up trying to make people happy and am instead leaning toward standards compliance, technical veracity etc.

May not make you popular though.

If you do this it's even more important that you're technically correct, so don't make a mistake like I did on the part in my thread the other day thread1103-207146

KENAT, probably the least qualified checker you'll ever meet...

 

[Xplicator]

I believe I now realize your dilemma since the dowel pin holes are not the same size, you believe that you cannot apply the pattern datum. As I examine your simplified example, I must presume the difference in size is a preventive measure to ensure correct orientation (clocking) of the other features in assembly process and making them equal is not an option.

The following is then my take on a potential solution. The way I see it, if the two (Dowels) are mating to locating holes and share equal function. I am not necessarily sure that you still can't use the pattern datum here; you would just need to be a bit creative with the GD&T language. To me the standard is very gray in this particular area. It does not say that the pattern of features must be the same size, therefore I would propose that:
• you leave the hole sizes and tolerances as they are
• that you create a position FCF, toleranced w.r.t. Primary "A"
• use two leaders from the FCF pointing one to each hole
• attach the “B” datum symbol to the FCF
• Make the "bolt circle" Dia a basic dim
• rotate the part so that the two holes are at 0 & 180 degrees respectfully as viewed

By doing this I can not find where the standard would be violated and you now have locked the component in six degrees of freedom with a DRF at the center. Additionally, use of the projected tolerance zone modifier is recommended here.

 

[PaulJackson]

Excellent advice Xplicator! With pinsNpads explanation of split press-fit bushings being installed in the holes the two holes most-likely serve as a dowel pattern where both holes constrain the three remaining degrees-of-freedom as a pattern RFS.

The one exception I have with your points is the comment on rotation of the view so that "the two holes are at 0 & 180 degrees respectfully as viewed." pinsNpads explained earlier that "Several people where I work don't want this as it make checking drawings for basic fit and "checklist" reviews more difficult" and Evan commented that the way the views are laid out and coordinates are detailed..."they are usually something to do with convenience for NC programming, fixture reference, or something like that", so I would not advise rotating the view if it is oriented to other details for ease of checking, manufacture, CMM programming, inspection, etc.

Paul