Why is the MMC modifier used so much more often than the LMC modifier?

[jeballes]

I work for an aerospace company that seems to add the MMC modifier to almost every tolerance and datum reference possible, but I never see the LMC modifier used. Is there a reason the LMC modifier is used less often? Is it related to the inspection requirements for the part?

I understand that inspecting a feature toleranced with an MMC modifier can be inspected easily with a go/no-go gage, and I guess that would not be applicable to the LMC modifier, but does it make a difference if the part is being inspected by a CMM?

Along the same lines, does it make sense to use the MMC modifier on tolerances for features that are not part of the interface with another part vs. just using a larger tolerance?

Any help is appreciated.

 

[mkcski]

MMC is typically applied when assembly concerns are paramount to the design and interchangability is needed. A study of Virtual Condition concepts will lead you to the details. I.E, Holes never go inside a boundary and fasteners never outside, guaranteing assembly at all sizes and locations if part is made to drawing requirements.

LMC is usually applied when sturctural concerns are driving the design. Like: the wall thickness of thin-wall tubing is at its worst when ID and OD are at LMC size. Tube sheets in heat exchanges are another example - the materal ligament between tube-holes is the smallest when the hoels are at biggest size - LMC.

Certified Sr. GD&T Professional

 

[drawoh]

jeballes,

Think through the problem you are trying to solve. If you are putting a screw or bolt through a hole that is oversize, you can open up tolerances a bit. You specify MMC/B. Don't just mindless apply tolerances. Solve a problem. I have used LMC/B twice.

The first time was a casting with two accurately bored holes in it. I had to ensure that the as-cast holes provided material to be bored out.

The second time I did it, I was ensuring there was adequate material thickness between two holes. I don't run into this problem very much.

--
JHG

 

[dgallup]

MMC gives you bonus tolerance, that means more parts are in spec, that means lower cost. Cost drives about 99% of all manufacturing decisions. As drawoh said, there are very few cases where LMC does anything useful. I too have used it only a handful of times, concentric cylinders are one.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

 

[jeballes]

But wouldn't using the LMC also give bonus tolerance to the feature? For example, a cooling hole pattern where you want to maintain the wall thickness between the holes. LMC on a position tolerance allows the position to vary more greatly when the holes are made smaller, so more parts would be in spec than if the position tolerance was RFS.

I find that I actually frequently encounter cases where I think LMC is the best way to go, so what I want to know is if there is some reason why it is not being used.

I have a hypothetical question: if you have a 1 +/- .010 hole which cannot violate a 1.040 diameter boundary. Would there be any benefit to using a position tolerance of .010 with an MMC modifier vs. just a .030 position tolerance RFS?
I see situations like this a lot and the only rationale I can imagine is something related to the inspection process.

 

[pylfrm]

I have a hypothetical question: if you have a 1 +/- .010 hole which cannot violate a 1.040 diameter boundary. Would there be any benefit to using a position tolerance of .010 with an MMC modifier vs. just a .030 position tolerance RFS?

One benefit of the first option is that it actually achieves your goal, while the second option only prevents the hole from violating a boundary of diameter 1.060 centered at true position. Keep in mind that the hole doesn't have to be perfectly cylindrical.


LMC position tolerances can indeed be used to ensure sufficient material exists for a subsequent machining operation, but I think profile tolerances often make more sense in these cases. If you can tolerate a certain amount of extra material on one side of a hole, you can probably tolerate that same amount all around.

LMC position tolerances can also be used to ensure adequate material thickness between between features, but I think directly tolerancing the minimum wall thickness often makes more sense in these cases. Providing fixed boundaries that must not be violated is probably more restrictive than necessary.

I don't mean to imply that LMC position tolerances never make sense, but I do think some of the more commonly discussed applications are rather questionable.


pylfrm

 

[CheckerHater]

Agree with pylfrm.

MMC modifier is beneficial (bonus tolerance and everything) in almost any situation of two parts fitting together, including fasteners to hold them.
And since nearly every machine consists of parts assembled with the fasteners, you see MMC modifier everywhere.
Also, conditions of mating parts (like Virtual Condition) have simple practical meaning - they give you sizes for your functional gauge(s).

LMC on the other hand is trickier. The LMC virtual condition is buried inside the material. it cannot be measured or checked with the gauge.
You need complicated techniques like CMM or scanning to establish where your boundaries should be located and how far away your part is from those boundaries. (Or you can check wall thickness with the caliper )

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

 

[mkcski]

I also agree wiht pyfrm with using profile to control (provide) extra stock (material) for future processing (grinding, machining) operations. Yes the inspection of LMC can really onle be done via calculation.

Sidebar: My spell checker quite working. Anyone know how to get it going?

Certified Sr. GD&T Professional

 

[Belanger]

Here's a simple thought experiment (along the lines of what's already been mentioned):
You have an assembly where a pin needs to fit into a hole. You know that both size and location need to be controlled -- and for now let's just think about designing the hole.

Option 1) As the hole's size gets bigger, we can let its position scoot around a little more

Option 2) As the hole's size gets smaller, we can let its position scoot around a little more


Which of those two options seems to make sense in order to allow for the mating pin?
(BTW, Option 1 is what MMC does, and Option 2 is what LMC does.)

 

[SDETERS]

For LMC we use this callout for Die casting Raw Material Bores that get machined.

 

[drawoh]

jeballes,

Here is the problem most of us solve most of the time...

The bigger the hole is, the more positional error can be tolerated. MMC/B provides a bonus here.

--
JHG

 

[mkcski]

There is also a case to consider zero positional toleance at MMC. This allows the MMC sizes to be the same and clearnce between the hole and fasteners is dependent on the actual sizes moving towards LMC (biggest hole, smallest pin). Just a thought.

Certified Sr. GD&T Professional

 

[SwinnyGG]

When you machine parts, you are removing material, not adding it. As tools wear, you remove less and less material with each operation (approaching MMC) until MMC is reached and parts start to fail.

See the examples above by other posters, where LMC controls are used on feature created mostly by additive methods (casting, etc).

As usual, this is a generality, and all of the detailed analysis of GD&T in the above posts is equally applicable to the question.

 

[Belanger]

I think Sdeters is saying that machined parts still need to have a minimum machine stock in order to grind off. So LMC ensures that minimum stock material (kind of like wall thickness).

 

[SwinnyGG]

Right.. that's what I said. LMC ensures the bores on his parts have sufficient material that they can be properly machined.

That machining callout probably uses an MMC modifier, because in that step material is being removed.

 

[Tunalover]

When it comes to in-plane features like holes and slots, I like to use LMC and LMB when the feature is close to an edge and you need to prevent feature breakout.

H. Bruce Jackson
ElectroMechanical Product Development
UMD 1984
UCF 1993

 

[greenimi]

Also, in simple cases like OD to ID direct relationship (one of the feature being datum feature and the other being controlled feature) the minimum and maximum distance/wall thickness between features IS the same regardless which modifiers are used (MMC/MMB or RFS/RMB). Therefore, if these worst case distances (max/min) are the same, why not use MMC to capitalize on bonus tolerance or datum shift, as applicable, make inspection easier/functional gaging and maybe drive the overall cost of the product down.

The above statement is not true if LMC and RFS modifiers are used interchangeably in simple cases as described (min/max distances/wall thickness between the features is NOT the same if LMC modifier is used versus RFS). Likewise, the results are NOT the same if LMC and MMC modifiers are intermixed or swapped with one another.

That could be, one of the multiple reasons, on why MMC is more “popular” than LMC: stackups

 

[marshell]

MMC can also allow for rework of a part that may have position errors. Holes, or datum features (depending on where MMC is applied and error occurring) can be machined towards their LMC limit allowing max positional tolerance, that may bring a part back into spec. A part defined cannot be reworked as the adding of material would be needed. Either way the design and function of the part is the critical determining factor on MMB vs LMB.