profile and MMC 5

[dho]

[.005][(B) mmc] applied to inside wall of the rectangular shaped can (cover). B is a hole at the can bottom. the hole has +.002/-.000 on its diameter. how can i apply MMC to this bilateral profile? bump .005 to .007 or else?
thanks.

 

[Belanger]

The key is that the MMC is not applied to the profile tolerance, but to the datum feature. FYI -- the latest edition of the Y14.5 standard calls this M modifier MMB, maximum material boundary, which is slightly different than pure MMC, which is the name of the modifier if it were to appear after a tolerance number.

That said, there is sort of a back-door effect onto the profile tolerance, and it depends on the actual size that the hole at the bottom is made. BTW, does the hole at the bottom have any GD&T applied to it?

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

http://www.gdtseminars.com

 

[MechNorth]

I'm not sure what you're really looking for. Unilateral profile tolerance? If that's the case, then '09 has the Circle-U modifier available. For '94, you need to use offset chain lines to show which side the tolerance zone applies wrt the basic geometry.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[pmarc]

dho,
Does the profile callout control inside rectangle all around?

 

[dho]

yes all around.

 

[dho]

the (datum) B hole is subjected to position tolerance to datum A. .002 dia mmc.
the profile tolerance is specified BILATERAL.
what M does to the profile tolerance? MMC, or MMB, bilateral becomes uneven bilateral? which side get the "benefit"? will the other side lose the "benefit"?
thanks to all helping me.

 

[dho]

let's say the nominal inside dim minus .0025 fits tight with the mating part. any "benefit" to the inside profile tolerance will cause problem. and "benefit" to the outside profile tolerance makes no sense.

 

[dho]

please see attached.

 

[pmarc]

In that case you shall not add this .002 to profile tolerance value, otherwise you may end up with accepting a part that does not meet profile requirement.

You may think of it in following way [let's say the basic rectangle (defined by basic dimensions) is 5" long and 2.5" wide and the datum feature hole is 1" +.002/-.000)]:

Imagine a wireframe containing following elemets:
1. Circle of dia. 1" simulating datum feature hole at MMB
2. Two rectangles - 5.05"x2.55" and 4.95"x2.45" simulating profile tolerance zone. The rectangles are perfectly centered to each other and to the circle defined in point 1.

Now, take your part and try to fit it - by rotating and sliding - inside the wireframe, so that the surface of datum feature hole does not violate circle from point 1 and the outline of the rectangle fully fits inside a space between two rectangles from point 2. If you weren't able to fit it, the part is out-of-spec.

So what is the benefit of (M) modifier in profile FCF? It is hidden behind a type of movement you did when trying to fit the part inside the wireframe. If you were able to slide and rotate the part that means the diameter of datum feature hole was bigger than 1.000 and smaller than 1.002. If you were only able to rotate the part, the diameter of datum feature hole was exactly 1.000. Rotation would be also only type of movement available if the profile FCF was [.005].

Having said all of that, notice that (M) modifier does not enlarge profile tolerance zone - it is always 0.005 wide. Instead of it you gain a possibiliy of shifting the part to fit it inside profile tolerance zone, if datum feature hole is not at its MMB = 1.000.

I hope you picture what I tried to say.

 

[pmarc]

dho,
If you attach something, make it .pdf, .jpeg, .png, .doc or something similar. Thanks.

 

[dho]

thanks.
in pdf

 

[pmarc]

dho,
My explanation about interpretation of profile FCF applies to this drawing too. The geometry is slightly more complicated, but you will still have a possibility of shifting the part to fit the inner contour inside profile tolerance zone if the datum feature hole is not at MMB = 1.000.

Positional tolerance applied to that hole has no impact on what I said, since profile FCF does not use A as datum reference. If A was referenced in profile FCF, you would have more shift available, because circle described by me in point 1 would be. dia. .188, and not .190.

Side note: I assume the true profile of inner contour is described somewhere by basic dimensions - in CAD file for example.

 

[MechNorth]

The MMC modifier (not MMB because this is a pre '94 drawing based on the datum feature identifier symbols used) on the Datum-B reference in the profile control is of no value here. Profile is a surface control. While the standard doesn't say that the MMC modifier is illegal in this case, it does not give any support on how it is affected either. In practice, inspectors ignore the datum modifier(s) when dealing with surface profiles. I don't know if Y14.5.1 (the mathematical definition of Y14.5) is working on a definition for this, but I suspect not. CMMs do not account for datum shift on a profile control either.

Jim Sykes, P.Eng, GDTP-S
Profile Services

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dho]

my fault. acad14 has only OLD symbol. the customer dwg has new. see corrected pdf.
thanks.

 

[pmarc]

Jim,
Did I understand your response correct? Are you saying that profile FCF's with and without (M) result in the same geometrcial requirements?

 

[Belanger]

I second that, Jim. Datum shift can certainly play a role with profile of a surface at times.

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

http://www.gdtseminars.com

 

[pmarc]

In case if someone, besides Jim, thinks that (M) "is of no value" for profile callout, I am attaching short pdf to explain that there is significant difference between having and not having datum reference modified by (M). I hope it is clear enough.

http://files.engineering.com/getfil...d-46e3-8158-ef9e0634917c&file=profile_MMB.pdf

 

[dho]

so, the profile only gets outside "benefit"? or say resulting unequal bilateral tolerance?
thanks.
see attached.

 

[Belanger]

Good stuff, pmarc. That's why I seconded you, but I didn't have such a graphic handy to explain it in detail.

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

http://www.gdtseminars.com

 

[pmarc]

No, the profile tolerance does not get any benefit. It is always .5 (in my example) or .005 (in your case) wide. It is the rectangular outline that gets certain locational benefit depending on actual size of datum feature.

Here is what would happen if tolerance zone was enlarged:
You added .1 (half of maximum datum feature shift available) to profile tolerance and made it +.35/-.25 all around. But notice, that by doing it you changed the requirement for maximum height and width of rectangle. Using your logic maximum actual size of outline could be 2.70 x 3.70. My example is showing the rectangle that cannot be bigger than 2.50 x 3.50.