Simulating a datum center plane 2

[semiond]

I need help in understanding this issue regarding simulating a center plane from a datum feature related to an external width dimension: let's say a width dimention is defined as a primary datum feature. When using a vise-like physical datum feature simulator with two almost parallel faces that close on the part, unless the tangent planes on both sides of the datum feature are perfectly parallel (and in the real world they're not), one of the vise faces will act similar to a primary datum plane - touching on 3 high points, and the opposite face will touch on only one point, similary to a tetriary datum plane. Now, depending on which side of the datum feature will make the more stable contact with the simulator, we might get a different separation width between the vise faces, and therefore the simulated datum plane will also be different. For example, if the measurement set up has the vise faces oriented horizontally, the side of the datum feature facing down will orient the part in the fixture, and if you flip the part upside down for a repeated measurement you might get different results on whatever control called out that datum. Now, I understand that there is only one "actual mating envelope" to the datum feature per ASME and only one of the sides facing down will produce the "minimum separation" condition per fig. 4-13, But that means that you have to mount the part twice in the fixtute and re-check your results, and I somehow doubt that this is the recommended practice... on the other hand, if the vise is oriented vertically, we will have no control over which side we stabilize better in the simulator - which is even worse. Everyone's insight will be much appreciated... Thank you!

 

[Belanger]

If the datum in question were secondary or tertiary, the answer would be pretty simple -- it wouldn't be permitted to vary or rock in the manner you describe. But since you say it is to be the primary datum, then I suppose there could be an unstable situation. The ASME Y14.5 standard says this in paragraph 4.11.2: "If irregularities on a datum feature are such that the part is unstable (that is, it rocks) when brought into contact with the corresponding datum feature simulator, the default stabilization procedure is per the candidate datum set as outlined in ASME Y14.5.1M."

So what you are asking about is what is called a set of candidate datums. I don't have a copy of 14.5.1 with me, so I'm not sure of your official answer right now, but I hope I've given some guidance to you dilemma.

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

 

[semiond]

Thank you very much for your input John. The paragraph you mentioned clarifies what should be done in many situations. My main concern though is with a situation where the part doesn't rock, but slightly different measurement practices may show different results. For example if you use a horizontal granite slab to inspect a part like the one in fig. 4-13 in ASME Y14.5, and close on it from above with some gage block that is kept parallel to the granite slab all the way until it touches the part on a high point, the set up might appear stable - the part wouldn't rock and so there will be no indication of a problem, but if you flip the part upside down and repeat the same practice you might get a different simulated center plane, and the central slot for example, might appear positioned and oriented differently to it. So the unaware inspector gets a 50/50 chance to simulate a wrong datum plane - which is not established in a condition of true "minimal separation" of the 2 parallel planes forming the datum feature simulator. I made a simple check in a CAD program: inspection of parallelism to a center plane datum where the faces forming the datum feature of width are not perfectly parallel. I saw that the more severe result appears when the datum is simulated in true "minimum separation". So in case of a wrong measurement, bad parts may pass. But how to prevent the wrong measurement? As a designer, i'm not very experienced in measurements, but i try not to define things in a drawing that i'm not sure in 100% myself how to measure at least on a theoretical level, and right now this issue is what stops me from defining a center plane as a primary datum in a part, where functionally it appears correct.

 

[3DDave]

In many instances there multiple solutions. To accept the part the inspector only needs to find one that meets the given requirements.

When installed, the part will also have the same options for location/orientation. If that is not acceptable then change the way the part is held in its next assembly and change the datum references to match.

If it is important that the acceptance orientation is the same as the installation orientation, then either have the inspector mark the part in a permanent way or have the part carry an orientation mark that is then shown in the assembly drawing.

 

[semiond]

Thank you Dave for your help. But what if we are dealing with a part that should have a symmetrical design and is clamped in it's functional assembly from both sides between spacers without priority to one side over the other? (as far as I understand, that's what center plane datums are for in the first place). And even though there might be a situation where the clamping force on the part in it's practical application will stabilize it repeatably, we don't want the same force applied in the inspection fixture on the newly manufactured part to avoid damaging the surface finish. Shouldn't there be a more "standardized" solution to this, that doesn't require changing the design of the part geometry and function?

 

[Belanger]

3DDave -- I know that in 1994 there was a paragraph about "adjusting to optimal" when a datum feature is unstable (the old paragraph 4.5.1), but that was dropped in 2009.
Maybe that was just for surface datums, not FOS?

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

 

[SwinnyGG]

But what if we are dealing with a part that should have a symmetrical design and is clamped in it's functional assembly from both sides between spacers without priority to one side over the other?

The case you're describing sounds like one where the part actually needs to be checked in both orientations, since you cannot control orientation at assembly.

The alternative to this would be that you address of the lack of orientation priority at assembly, using an orientation identification feature as others have stated.

 

[drawoh]

semiond,

I strongly prefer a feature-of-size datum to be accurate. If it is very much more precise than the features controlled by your tolerances, your life is way simpler. My next choice would be to call up the datum feature at MMC/B. Again, this keeps the tooling simple.

If the feature is sloppy enough that we are not sure where the centre is, I would dimension and measure from an edge or corner.

--
JHG

 

[3DDave]

If the manufactured FOS has nearly opposing peaks on both sides, there can be many orientations that are stable.

This can radically relocate features intended to be dimensioned relative to the centerplane.

 

[semiond]

Belanger, I checked paragraph 4.5.1 in the 94' standard and it does seem to talk about planar datum features "not subject to size variations" and "adjusting to optimal" seems like the practice required in case of a slightly convex surface (intended to be flat) rocking on the fixture surface that acts as a plane simulator. It's a different scenario from what I'm talking about.

But that paragraph also points in the end to 4.3.3 that talks generally about the need to control the accuracy of datum features, since "Measurements made from a datum reference frame do not take into account any variations of the datum features." This is related to what drawoh suggested - that a datum feature of size should be very accurate. If that datum feature of size is used as primary datum in the part's datum reference frame, I suppose that the way to make it accurate is tightening the dimensional tolerance on the width, and this in combination with rule no. 1 will indirectly tighten the parallelism between the tangent planes of the 2 opposing surfaces of the FOS. But this also means that I have to tighten a tolerance of size much beyond the functional requirement, just to make other measurements more repeatable. This might increase costs and doesn't sit well with the agenda behind the use of GD&T.

 

[semiond]

jgKRI, you said:
"The case you're describing sounds like one where the part actually needs to be checked in both orientations, since you cannot control orientation at assembly."

I think that if I use each side of the FOS separately as the orienting plane, I might end up with two different datum reference frames for the part, and a need to double all the geometrical controls. And I would still remain with a need to center or locate features in relation to a correct datum center plane (which is difficult to simulate)

I suppose I could "force" one of the sides to be a planar datum and replace the center plane with it for other controls, defining basic dimensions from it to features that were supposed to be understood as "centered" to the original datum center plane, etc. But that wouldn't describe the part functionality accurately (like datums should), and that approach disqualifies pretty much all cases where a center plane chosen as a primary datum, which is kind of weird...

 

[SwinnyGG]

Unless I'm missing something, yes- that's the consequence of your current scheme.

The easiest solution that I can see is to just control orientation. Mark the part and gage a specific orientation.

 

[pylfrm]

semiond,

If you are considering abandoning symmetry, you might want to look at customized datum reference frames per ASME Y14.5-2009. It would be possible to use one flat surface as the primary datum feature, but only allow it to constrain orientation. The feature of size involving both flat surfaces could then be used as the secondary datum feature, and it would only constrain translation. This gives you something like a feature center plane, except possibly with improved inspection repeatability. Irregularities on the primary datum feature can still cause issues though, so I'm not sure if this scheme is really much of an improvement.

If you stick with a symmetrical tolerance scheme, increasing datum feature accuracy is about all you can do. Form accuracy is what matters, so you don't necessarily have to tighten the size tolerance.


pylfrm

 

[semiond]

pylfrm, thank you for that tip, customized datum reference frame seems like something that could work as a solution in some cases.

What I have in mind though is a part similar to fig. 4-15 in ASME 14.5Y-2009, only with two bosses protruding from the opposite sides around the central bore. In it's practical application, the part is clamped from both sides on the faces of the bosses, and spins on a shaft on which it sits with a sliding fit. I want to choose the datum reference frame according to the functional surfaces, So in my part the width between the faces of the bosses is the feature of size datum that replaces primary datum A in that figure. In addition, I need to center the body width in the section closer to the periphery to A by a positional tolerance. I also need datums B (secondary) and C (tetriary) for locating the holes, so in case that I apply the customized datum reference frame concept and choose one boss face as a primary and the center plane as secondary datums I may end up with a datum reference frame of 4 datums to lock all degrees of freedom...?

If I stick with center plane as the primary datum, i think that in order to "qualify" the datum feature, I need to control the orientation (parallelism) between the tangent planes from both sides of the FOS. because even if the form (flatness) of each side is very good, if the tangent planes are not parallel enough, it may cause the problem I was talking about.

 

[pylfrm]

semiond,

Keep in mind that tangent planes have the same potential for instability as planar primary datum features.

Compared to the tolerances you want to apply, how large is the worst-case shift allowed by datum feature inaccuracy? It's hard to guess at this without knowing a lot more about your part's geometry.


pylfrm

 

[semiond]

pylfrm, i added a sketch with some dimensions in milimeters related to the subject. I didn't tell earlier but a parallelism check like shown in the sketch is also needed. In the 2 measuring methods shown it is checked on the same face (I guess i should have done a small chamfer there to differentiate it from the other faces). The worse result is the correct one, but how many inspectors will actually do the double check?

Also note how each time one of the faces of the datum feature of size is playing the role of a planar primary datum feature, while the other has no meaning other than indication of the simulator's separation distance (AME size, that is only correct at the second option).

 

[pmarc]

semiond,
Asuming that in your sketch inspector is not able to bring two parallel planes of datum feature simulator closer than 4.71 apart, inspection method #2 should be used.

Fig. 4-13 and para. 4.11.4b in ASME Y14.5-2009 explain that two parallel planes of datum feature simulator must be at minimum separation. So this means the inspection #1 does not meet this requirement.

 

[3DDave]

The purpose of inspection is to find an orientation and/or location that allows the part to pass, not to exclude the infinite number of conditions where it does not pass.

For example, the car wheel on a hub. I can set the wheel so the primary contacting surfaces are parallel and so the hub guide shoulder is perfectly aligned to the hole in the rim, but there are an infinite number of orientations that the studs won't align with the holes in the rim. I only need to find one where they will line up to install the wheel.

Your example is what I mentioned earlier. The part needs to be designed so the assembler can install the part in a compliant way; that way the inspector can also install the part in the orientation required to match what the assembler will do. If that is not the case you will need to add instructions for the inspector to move the part and have the tolerances checked through the entire range of allowable orientations.

 

[semiond]

3DDave, if i understand you correctly, then it is fair to say that if a center plane of a feature of size (external width) is defined as the primary datum feature in a datum reference frame, and no additional specific information is given in the drawing regarding assembly and inspection technique - in the form of notes, markings, or assembly views depicted in a part drawing, then the following is true:

1. The part drawing is not complete: the orientation and exact theoretical location of all or some of the tolerance zones related to the defined controls is ambiguous.

2. the part in the exaple can be considered in tolerance after checking it like shown by "inspection method #1".

Is that correct?

 

[3DDave]

1) The part drawing is complete and not ambiguous. It simply accepts parts you don't want. If it doesn't get the result you want then you need to make different choices.
2) It would be acceptable unless the inspector was lazy an rejected on the one orientation.