GD&T MMC versus Tolerance

[gregfox]

I understand the difference between the position of a feature and its size. I would like to know why GD&T MMC (or LMC) is use for a hole and pin rather than just making the dimension of the hole and pin such that they will always fit if in tolerance.

I'm really not getting this "bonus" thing, aside from the fact that it looks like what would be there if you gave the necessary tolerance in the first place.

Please use plain English. I really sick of reading "wkikiease"etc

Fox Manufacturing Group (Machining and Molding)[

http://tjmain.com/foxmfggroup.com/Home.html

]

 

[KENAT]

Simplistically:

When you are trying to put a pin, screw or similar through a hole, as the size of the hole increases, how accurately it is placed becomes less important.

If the hole is .010" over size then it can move .005" in any direction and the screw/pin will still fit through.

The concept of MMC is to take advantage of this, saying that as the hole diameter increases the tolerance on it's location can be relaxed correspondingly.

Make sense?

You're basically squeeze all the tolerance out that you can so you ensure all parts work without scrapping

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[dingy2]

If you have a diametrical tolerance zone of .010, it means that there is a radial tolerance of .005 (1/2 the diametrical tolerance zone) about the theoretical center. It doesn't matter about the size, it is a radial tolerance of .005" for the hole center.

If you see a diametrical tolerance zone of .010 at MMC, it is dependent upon the size. Let's say you have a hole with a diameter of .250 with a tolerance of +/- .005. The MMC (maximum material condition) will be its smallest allowable diameter - in this case .245. I would always think of the requirement as a diametrical tolerance zone of .010 beyond its MMC (.245) and the would equal a boundary of .235. Subtract the actual size of the hole from this dimension (.235) and you now have the calculated positional tolerance.

Let's say the actual size is .251. The calculated positional tolerance would be .251 - .235 = .016 or radially .008. As the size of the hole changes, so does the calculated positional tolerance.

Rational - If a Designer calculated the tolerance of a hole at its smallest allowable size and the hole ends up bigger, we take that extra size difference (bonus) and add it to our position tolerance. To me, it is practical.

Hope this helps.

Dave D.

http://www.qmsi.ca

 

[PeterStock]

The size of the pin and hole are sized so they allways fit together. The location tolerance of the hole and pin is where the bonus tolerances show up. Consider a hole at its MMC and max position error. It could just touch the pin at its MMC and max position error. If the the hole increases in size the location error can increase and still just touch the pin. Allowing this bonus tolerance (and datum shift if one of the datums if a feature of size) means a part that has larger but still within tolerance holes, but the position is a bit off from the postion tolerance at MMC can be accepted if it still can be assembled.

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services

http://www.infotechpr.net

 

[dgallup]

Another big benefit of GD&T & MMC is functional gauging. It allows you to make a hard go/no-go gauge that takes into account both size and position. The part is good or bad in one quick, low cost check without expensive measuring devices.

 

[PeterStock]

The opposite to MMC is LMC, least material condition. This is used where what is important is not the location but how close the feature is to other features. As an example you would use it to control a minimum wall thickness.

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services

http://www.infotechpr.net

 

[PaulJackson]

Please use plain English. I really sick of reading "wkikiease"etc

Here is a wikiease response.

paul

 

[drawoh]

I understand the difference between the position of a feature and its size. I would like to know why GD&T MMC (or LMC) is use for a hole and pin rather than just making the dimension of the hole and pin such that they will always fit if in tolerance.

Take the case that you are specifying a clearance hole for a fastener.

The fastener has a size and a location. From this information, you can determine what space may potentially be occupied by the fastener.

Your clearance hole must be outside this space. For a given sized hole, you can work out the positional tolerance required to keep your fastener inside your hole. The bigger your hole is, the sloppier your positional tolerance can be.

The positional tolerances of clearance holes often are called up at MMC. This indicates that the positional tolerance applies at the small diameter (MMC), and that it can be loosened as the hole gets bigger.

How is that?

JHG

 

[BiPolarMoment]

This seems like a good place to ask as any and seems relevant... I find the concept of a zero positional tolerance at MMC for a clearance hole much more understandable than including a separate tolerance for both the diameter and positional tolerance. Are there specific advantages/disadvantages to doing it either way?

 

[PaulJackson]

Zero at MMC

Advantages:

Fully proportional location/orientation tolerance (as long as the sizes meet their boundaries and the MMB is not breeched the feature satisfies the specification).

No need for an MMC size boundary gage.

Disadvantages:

Confusion about what value to target size.

Disables the ability to statistically predict position conformance with continuous data... using typical formulas.

Paul

 

[Belanger]

Just to add to Paul's post...

Another advantage -- it reduces the inspection/gaging, because now the lower size limit for the hole is the same as the virtual condition which would be verified as the position tolerance. (IOW, if functional gaging methods are used, then the zero at MMC design eliminates a gage.)

Another disadvantage -- it might not be wanted if there is a minimum size of the hole that needs to be maintained for weight reasons. (It's not common, but a hole below that size might function fit-wise, but might add too much mass for the piece.)


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

 

[drawoh]

BiPolarMoment,

I have been specifying holes with zero positional tolerance at MMC for some time now. I have had one shop get back to me asking WTF I am doing. They accepted my explanation.

Consider the following...
[ul]
[li]When you specify something like a Ø5/4.2 hole, you are not getting Ø4.2. They must open up the hole to get some positional allowance. [/li]
[li]The minimum hole size should be the maximum space occupied by your fastener. In the case of a bolt, this is the maximum diameter of the bolt. For a screw, it is the maximum diameter, plus the positional tolerance of your tapped hole.[/li]
[li]The positional tolerance of your mating hole, whatever it is, controls the hole, not the space above the hole. You are interested in the space above the hole. Fudge your clearance hole out a bit. If your part is thick, consider using a projected tolerance zone on your hole underneath.[/li]
[li]Your maximum hole specification allows for drilling orpunching tolerances as well as positional tolerance. You need to be generous. Your maximum size should should be your minimum size plus a reasonable positional tolerance plus a reasonable total variation in your hole making process.[/li]
[/ul]

JHG

 

[drawoh]

Just to add to Paul's post...

...

Another disadvantage -- it might not be wanted if there is a minimum size of the hole that needs to be maintained for weight reasons. (It's not common, but a hole below that size might function fit-wise, but might add too much mass for the piece.)

Tolerances ought to be thought through, not just applied automatically. The zero positional tolerance is the most accurate and complete way to describe a hole that will be clear a fastener or other projected feature. If I have some different requirement, I should be specifying the hole differently.

JHG

 

[Belanger]

Well, not quite -- sometimes there are situations where you have to straddle several concurrent requirements.

I only mention this disadvantage because I experienced it in the aircraft industry, where even a half-ounce can be important. Yet it was still a through-hole for a screw.

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

 

[powerhound]

gregfox,

Your lack of acknowledgment to any of the answers to your question means either you haven't read them, you've lost interest, or you still don't get the whole bonus thing and are still waiting for a suitable response.

Let me take a stab at it. Imagine you have a part with two 1/4" dowel pins spaced 2" apart. For the sake of simplicity, we won't address the tolerance issues with this part. Let's assume the pins are EXACTLY .250 in diameter and EXACTLY 2.000" apart.

Now, let's say you are making a mating part that has 2 holes that the 2 pins of the existing part must fit into. Using the direct tolerancing method you are referring to, you COULD dimension the holes at .257 +/-.005 and give the 2.000" spacing a tolerance of +/-.002 and the parts would always mate up. The problem is that it doesn't take the size of the hole into consideration. If you produce the holes at .262 then why should you hold the tolerance of the spacing to +/-.002? Those holes could be spaced out to 2.012" and the part with the pins would still mate up.

Direct tolerancing sometimes induces tight tolerances where they are not necessary. Using GD&T, you would basically tell the manufacturer of the part. "If the holes are produced at .252 then their spacing tolerance cannot exceed +/-.002 but as the hole departs from MMC (gets bigger), you can add that amount to the tolerance."

So if the holes are produced at .257 they could be 2.007" apart and work, and if they were produced at .262 they could be 2.012" apart and still work.

Hopefully this makes the idea of bonus tolerance a little easier to grasp.

Powerhound, GDTP T-0419
Engineering Technician
Inventor 2010
Mastercam X4
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[gregfox]

Sorry for the delay, I have my forum emails come to a folder that for some reason suddenly filled. I had checked the this folder initially… I really do appreciate the responses!

And the best answer is “Direct tolerancing sometimes induces tight tolerances where they are not necessary” Now I get it.

Thanks!
Greg


Fox Manufacturing Group (Machining and Molding)[

http://tjmain.com/foxmfggroup.com/Home.html

]