MMC for Datum Question

[T105]

Hi,

The question I would like to ask is about the determination of tolerance values when the datum is shown in Maximum Material Condition (MMC) or Least Material Condition (LMC).

From the sample drawing I assume that Datum A is the axis of the 414mm diameter cylinder (Is the assumption correct?).

The 406.4mm diameter cylindrical portion is positioned with the given GDT box. I would like to know how the MMC condition of the Datum A is evaluated.

best regards

 

[Belanger]

If you know how the first M symbol affects the position tolerance, then this second M symbol works in a very similar way. If the datum feature is at its maximum of 414.0, then there is no extra tolerance in the alignment of the two diamaters (of course you'll still have the 0.05 plus any "bonus" from the first M symbol).

But if the datum feature is made at a size less than maximum, then there is a corresponding increase in the allowable position tolerance. Here are some sample numbers:

If smaller dia = 406.425 and large dia = 414.0, then position tol = Ø0.05

If smaller dia = 406.390 and large dia = 414.0, then position tol = Ø0.085

If smaller dia = 406.425 and large dia = 413.925, then position tol = Ø0.125

If smaller dia = 406.390 and large dia = 413.925, then position tol = Ø0.16


FYI -- this effect of the second M symbol can be thought of as directly additive in this specific case only (because the two diameters act in the same direction). But just so you know, in other cases where the M symbol appears after the datum letter, it's not necessarily directly added. What really happens is that this second M symbol doesn't increase the tolerance zone, but rather allows it to shift around. But in your case, for simplicity, think of it as additive.

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

 

[SeasonLee]

When the large diameter is referenced as the primary datum A at MMC, the datum feature gage (or simulator) is fixed in size, the gage size is equal to the datum feature MMC at 414.

If the large diameter made less than MMC size, the part may have some movement (clearance or shift) in the gage, this movement is called “Datum Shift” in GD&T, it is an allowable movement between the part datum feature and the gage, datum shift is similar to bonus, it may result in additional tolerance for the part (for coaxial part only, like this example).

The amount of datum shift is equal to the amount the datum feature departs from MMC, so the max amount of datum shift is equal to the difference between the gage size and LMC of the datum feature. The max datum shift = = 414 – 413.925 = 0.075 (same as the difference of size limit)

For example : datum feature A size at Ø413.960
Tolerance feature size at Ø406.410
The total allowable tolerance = positional tolerance + bonus + datum shift
The total allowable tolerance = 0.05 + (406.425 – 406.410) + (414 – 413.960) = 0.105

SeasonLee

 

[T105]

Thank you very much for the detailed answers and explanations.

There is one point that I want to clarify. I assume that Datum A is the axis of the cylinder with diameter 414mm. Is that right?

If so, the datum is an axis which is somehow independent of the 414 diameter. So is it logical to add Max Material Cond on an axis?

 

[Belanger]

The true, theoretical datum is indeed an axis. But in the real world, we still need to physically touch something to derive an axis. This is where the "M" symbol comes in.

Without the "M" we would have to find the true axis regardless of size. That means wherever the large diameter is, we want to lock onto its actual axis.

But with the "M" symbol, the designer is saying that we really want to measure the small diameter against the axis of the large diameter as if it were at its biggest. That's quite different, because it implies that if the large diameter is less than MMC, then there can be a slight mismatch between the axis of the real part and the imaginary axis that we are really positioning around.

Perhaps it's easier to think of it the way SeasonLee mentioned: Just imagine a fixed-size gage hole of 414.00 that we drop the large diameter into. If it is a loose fit (i.e., the actual part is less than MMC), then the part can jiggle around inside that gage. Now we simply say, "Hey, it's OK that the part jiggles; we want to verify the position of the small diameter to the gage's axis, not the large diameter's actual axis.

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

 

[dtmbiz]

SeasonLee... think it should be LMC of dia 406.39

Maybe this would help if I am understanding your question.

The axis of the toleranced diameter is the center for a cylindrical tolerance zone located at the axis of Datum A in this dwg. The cylindrical tolerance zone would be a dia of 0.05 when the diameter is at MMC or 406.425 in this case. As the diameter gets smaller, the decreased size difference between the max condition (406.425) and the actual size hole (produced size) is added to the cylindrical tolerance zone. The additional tolerance is known as the “bonus tolerance”. E.g. if the actual diameter is 406.39 then the tolerance zone cylinder increases from dia 0.05 to dia 0.085. The actual diameter axis would need to lie within this dia .085. The cylindrical tolerance zone is positioned at the center of the datum simulator for Datum A axis and extends thru the depth of the located diameter. This is for the case of an external feature of size at MMC. The inverse would be true of an internal feature of size. The” M” referenced with Datum A allows “datum shift”. As Datum feature A deviates from it’s MMC size then the cylindrical tolerance zone is permitted to shift relative to the size difference between Datum feature A’s actual size and its size at MMC.

 

[SeasonLee]

dtmbiz

Let’s summarize all data :
The MMB of datum featutre A = 414
The LMB of datum featutre A = 413.925
The MMC of toleranced feature = 406.425
The LMC of toleranced feature = 406.390

If the toleranced feature size made at LMC 406.390, the bonus = 406.425 – 406.390 = 0.035. and the allowable position tolerance = position tolerance callout + bonus = 0.05 +0.035 = 0.085.

Since there is a M on datum feature A, so the total allowable position tolerance should include the “datum shift”.

SeasonLee

 

[dtmbiz]

SeasonLee...

In haste I thought that you used LMC in your example...
Summmaries are good... my bad..

Very goot for us simple folk...