Datum MMC as bonus. Newbie Alert 13

[marvalgames]

Hi all. Brand new and so much to learn. Anyway I have a drawing with a True Position with MMC. It also uses Datum A and C marked as MMC (or is it MMB). From what I understand this is not added as bonus tolerance? However in some cases possible? Not sure because my co-worker and trainer is saying to add the Bonus from Datum B the slot? Pretty confused. Please see attachment.
Thanks for any feedback

 

[drawoh]

marvalgames,

I am trying to make sense of your drawing. I cannot find the feature for datum[ ]A. I assume it is a diameter with a tolerance. Also, I think your drawing standard is ANSI Y14.5M-1982, which makes the term MMC. MMB is for ASME 14.5-2009.

Datum feature[ ]B is the end of your part. It is not a feature of size (FOS), and MMC has no meaning. Datum feature[ ]C appears to be a slot. This is an FOS, and there can be a bonus tolerance if this is called up at MMC (or LMC!).

Think of your datums as the fixturing features required to immobilize your part. You should generally call them up in the same order.

Calling up FOS datum features at MMC makes it easier to build inspection tooling. This is important if your datum features are not accurate. If your FOS datum features are accurate, the bonus tolerance is not worth documenting.

--
JHG

 

[mkcski]

marvalgames:

Let me add to drawohs' statment:

[/Think of your datums as the fixturing features required to immobilize your part. You should generally call them up in the same order.
quote]

While datums do contol motion, their selection and their sequence (order of precedence) are usually driven by the function and fit-up requirements of the part.

Certified Sr. GD&T Professional

 

[powerhound]

And to add more to the story, an MMB/MMC modifier applied to a datum reference does not increase the size of the tolerance zone in the tolerance portion of the feature control frame, it only allows the tolerance zone to move. This is definitely a tough subject for a newbie to tackle.

John Acosta, GDTP Senior Level
Manufacturing Engineering Tech

 

[marvalgames]

Thanks everyone. I am starting to wrap my head around this and understand it better. In the meantime allow me to be more specific to the current problem at hand.
I am trying to calculate the True Position of the .165 +/- .005 Hole Diameter (near Datum B on attachment)
Tolerance .010 M / Datum A M / Datum C M.
I know I can add the M for the Hole itself. So if the hole is the .170 max I am now allowed up to .020.
I am still unclear if I can add the Bonus for Datum A and C in this specific case.
Datum C is the slot (.060 +/- .005)
Datum A is the ID of the Tube (.445 +/- .002)

I was told to add to my True Position tolerance the Datum C Bonus. So if if the slot is the .065 max my new tolerance for the True Position is now up to .030. (Started at .010. In my example the Diameter is .170 and the slot is .065)

I am still trying to make sense of how Datum C slot could possibly be added as a bonus to my .165 Diameter True Position.
(Especially when considering above post "MMB/MMC modifier applied to a datum reference does not increase the size of the tolerance zone in the tolerance portion of the feature control frame, it only allows the tolerance zone to move")

Thanks again.

 

[3DDave]

Stop listening to whoever told you that hole position and datum shift could be added.

 

[semiond]

An advice from a newbie to a newbie (If i'm wrong i count on the non-newbies to correct me) imagine the mating part of the part you're dimensioning as the inspection fixture. The datums tell you information about the features of the mating part. Concluding from the way it was toleranced, that sleeve in your drawing sits on a shaft (datum A) with a certain radial clearance to it's internal dia. The sleeve is supported on it's end face (and thus oriented in space) by datum B. A tab (datum C) protruding from the shaft enters the slot, also with some clearance, and limits the rotation around the axis to some level. Now let's say a screw should enter through the hole you toleranced to the 3 datums into a threaded hole in the shaft, and a larger tab should enter through the larger slot into a pocket in the shaft. When assembling, you can take advatage of the clearances i was talking about to move the sleeve back and forth a little bit and spin it a little bit until everything fits. If all parts fit - the part passes the dimensional inspection ☺ This is what the modifiers on the referenced datums (mmb per asme y14.5 09') are saying, usually the maximum material boundary on those datums means that the shaft and the datum C tab on the mating part that serves as your inpection fixture should be produced in their largest allowable size (which are related to the smallest sizes of inner dia. And slot width on your part, respectively). Does this mean that you get a larger toletance zone in production for the controlled features? I think not. It's hard for me to analyze it in this case, but i know that in some cases it may lead to a tolerance stack up that will make assembly impossible. In any way, the mmb doesn't make the tolerance zone larger, but it tells that there is some space for "play" in assembly - it simulates functional assembly in the dimentional inspection.

 

[drawoh]

marvalgames,

I am trying to make sense of your datums. Datum feature[ ]A defines a centre-line. Datum feature[ ]B locates your part left to right. You have not specified this for your hole, but you need it. Datum feature[ ]C controls the rotation of your part. Note how you should always be calling your datums in the same order.

If your two FOS datum features are at LMC, you have that room to wiggle your part around to pick up your Ø.165[ ]hole. All of this movement is up and down.

--
JHG

 

[CheckerHater]

I was told to add to my True Position tolerance the Datum C Bonus.

Stop listening to whoever told you that hole position and datum shift could be added.

I made a simple (maybe oversimplified) example to illustrate two important things:
1. Yes, datum shift is real and under some circumstances may give you extra positional tolerance.
2. No, you cannot simply add the datum shift to the value in Feature Control Frame.

As real life parts are usually far more complicated than the one I used, several experts agree that it is safer to simply ignore the datum shift.

(In my example I use zero at MMC tolerance to simplify calculations, but it's not critical)

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[semiond]

Just to add to what drawoh said, it is usually important to call out the datums in the same order in your controls, because the order of the datums represents the role of each datum feature in the interface of your part to the mating part, and similary to the fixturing device at inspection. The primary datum should be where the mounting forces are the greatest and usually where the contact face is the largest. On this datum feature the part should make contact with the fixture on at least 3 points and it constrains the most degrees of freedom, including at least two rotations (unless the datum is a sphere). The next datum to constrain degrees of freedom is the secondary and then the tetriary constrains the rest (if needed). So usually the datums will appear in the same order on each feature control frame, unless perhaps where there are two different possible interfaces to the same part... in your case, i think that datum B is has too little surface area to be primary, so i guess it should be A then B then C for both the hole and the large slot.

 

[pmarc]

What I am going to say may sound like a nit-picking, so sorry for that, but I believe it is worth to say it:

And to add more to the story, an MMB/MMC modifier applied to a datum reference does not increase the size of the tolerance zone in the tolerance portion of the feature control frame, it only allows the tolerance zone to move

I have found that to some people a different intepretation is useful. An MMB/MMC modifier applied to a datum reference does not allow the tolerance zone to move - as long as there is a loose between actual as-produced surface of datum feature referenced at MMB/MMC and its simulator, the modifier allows the considered part to move relative to the fixed datum feature simulator and fixed tolerance zone(s).

1. Yes, datum shift is real and under some circumstances may give you extra positional tolerance.

Datum shift loosens relationship between datum feature referenced at MMC/MMB and the toleranced feature but never gives extra position tolerance in a sense that the position tolerance zones gets bigger. The size of tolerance zone does not depend on what happens with the datum feature. If it were, then the size of the gage pin(s) in both "Bonus condition" pictures would have to vary depending on the size of RAME (Related Actual Mating Envelope) of datum feature B.

 

[chez311]

CH - so I don't want to derail the discussion too far out of the realm that it is useful to OP, however I reviewed your example and it really helped me put the the whole MMB/LMB concept into perspective for me. I should probably leave it at "MMB/LMB is more complicated than simply adding it to position tolerance in most cases and does not behave as a bonus tolerance" however I can't help but dig a little deeper...

I'm a little confused how you can say that its "safer to simply ignore datum shift" while presenting an example in your attachment that both instances (single and multiple holes) are examples of conditions that would not be possible without MMB/datum shift. If the tolerance was applied at the RMB condition the min/max distance for all the holes would be 19/21 respectively, however since you have applied MMB positions outside these bounds are possible. It seems to me that with datum shift applied to multiple features the allowable min/max deviation for each individual feature is dependent on the material condition/location of all the features in the pattern. That means with all the holes at LMC as you have shown the min/max distance is now 18/22 for each hole, however that condition CANNOT exist simultaneously for both holes (ie: both at 18 or both at 22 is not allowed) - one may be at 18 while the other is at 22. Basically as the holes depart from the position tolerance allowed by the MMC bonus (previously stated 19/21) they must "shift" together (hence the name - lightbulb moment!!) as the movement of one limits the movement of another - every departure from this MMC bonus position by one hole limits the maximum position of the other by a proportional amount (ie: one hole at 18 limits the other to 20-22, and one hole at 22 limits the other to 18-20).

I'm sure I've confused the issue with putting numbers in there without figures but its the best I could do without making a ton of sketches. Basically what I'm trying to say is that I don't think its enough to say "ignore datum shift" as that wouldn't allow you to calculate the min/max conditions allowed by MMB/LMB datum shift which are different than those calculated without datum shift. Wouldn't it be better to go ahead and calculate your min/max conditions and treat it in a stackup in a similar fashion as bonus tolerance, with the knowledge that the min/max condition cannot exist for all features of that pattern simultaneously?

 

[powerhound]

pmarc,

Yeah, I thought some might have a problem with that explanation but that's the one I've used in the past that has caused the light to start coming on regarding datum feature shift. Further explanation brings it home to match what you said.

John Acosta, GDTP Senior Level
Manufacturing Engineering Tech

 

[powerhound]

pmarc,

I think what CH is saying is that if you have a tube with a positional tolerance that locates the ID at MMC with respect to the OD at MMB, this will appear to have increased your positional tolerance even though it really didn't.

John Acosta, GDTP Senior Level
Manufacturing Engineering Tech

 

[mkcski]

CHEZ311:

For consideration: when I teach MMC and/or MMB concepts I usually sketch what I call "cartoon" gages. I then "place" parts with varying controlled feature and datum feature sizes "onto" the gage. It doesn't take long for students to gasp fixed simulation (datum shift),variable simulation (largest/smallest inscribed/circumscribed) as well as related and unrelated actual mating envelopes. This might help the understanding.

Certified Sr. GD&T Professional

 

[chez311]

mkcski - i think i understand pretty well the effects of MMB vs MMC, in fact i was just stating that CH's example just helped solidify that understanding. the line dividing MMB datum shift vs MMC bonus tolerance had always been a little fuzzy for me but as i said his diagrams showed me in a similar way to your "cartoon" gauges, which was very helpful.

The main thing i was questioning was CH's statement below, i didn't understand why he said that as it seems to me that MMB/LMB datum shift can lead to min/max conditions not possible under RMB. I may be mistaken, but I didn't think "simply ignoring" it made sense, even in his example of multiple features. Maybe he meant something else and I'm not understanding correctly but I wanted to ask the question.

As real life parts are usually far more complicated than the one I used, several experts agree that it is safer to simply ignore the datum shift.

 

[CheckerHater]

When ignoring the datum shift (pretending datum is at RFS) you risk rejecting good parts (in theory) but not accepting bad parts.

CMM systems are having hard time dealing with datum(s) that move anyway. And that's how I would check 200 holes.
By the way, functional gauges are checking for datum shift automatically - you are safe there.

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[pmarc]

Pmark suggests calculating min and max of every hole for datum shift situations.

Where did I say that?

 

[pmarc]

That was not my quote but chez311's.

 

[CheckerHater]

OK, adjusted. Too much scrolling today

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future