LMC and MMC callouts in FCF 1

[brandnew1]

Hi everyone,

i'm by far no expert on GD&T but i do have the basics.

If the LMC is used, does this work the opposite as that of the MMC...so in terms of bonus tolerance as the hole gets smaller the more the bonus tolerance?

How about situations that arise as such:
Dia. .37 +/-.0005 [tp]dia. .010 L / H / C (L)

R.300 [tp]dia..014 M / H / C (L)

i'm not quite sure how this works when LMC is used for a datum in the FCF or when both MMC / LMC. For the R.300, i believe i would get a bonus tolerance as the radius increases in size, but how does the LMC work? Do i get additional tolerance when datum C is cut smaller in size?

Attached is the same callouts as above but in the GD&T Symbol format.

thank you

 

[Belanger]

For the first part of the question, you are correct. If it's a hole, then the smaller the hole is made, the more out of position it may be ... I'm just rephrasing what you wrote.

For the second part of the question, we would need to clarify if it's an internal or external radius (and whether it is < or > than 180º), but basically the first "M" symbol works just like the "M" on a regular hole or pin: when the feature's size departs from the MMC, a bonus tolerance of the same increment is allowed.

For the use of "L" after a datum letter, we would need to know more about the datum feature being referenced. Is it a hole or pin? Does it have any geometric tolerance of its own? But the short answer is yes: variation on the actual datum feature C can make the position of this radius appear to be more out of position. GD&T folks don't call this bonus; it is usually called "shift tolerance" to help us distinguish it from "bonus tolerance." But we have to be careful ... shift tolerance doesn't really add on top of the .010. Instead of making the tolerance zone larger, it merely allows it to scoot around with respect to the datum feature.

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

 

[brandnew1]

Thank you John-Paul,

i don't think i'm allowed to show the drawing however i drew up one similar with those callouts. Forgive my drawing, i just used MS Paint.

So with this type of callout, when the part comes in to be inspected, how do i determine if this would be an acceptable part? Based on the given value of 1.100BSC, if i origin to Datum C and viewing the part where the radius is in the (X,Y) coordinate plane i calculate a value of X = .93, Y = .57 as being the location.

So generally, if the hole were to increase i could add the bonus tolerance to this .014. But how does Datum-C affect this when it’s with an LMC modifier.

Now as i look at the drawing, is this correct? How would an outer area be affected in terms of MMC? i thought it would be the hole itself?

thank you for the help

 

[brandnew1]

i apologize, that should be X = .78, Y = .78....

 

[MechNorth]

Substantial issue with putting a position on a radius feature that is not a feature of size. You can control the R.300 with a profile control instead. Also, you have no relationship between datum C and the higher-precedence datum-H.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[SeasonLee]

When the straightness applied to a FOS (datum feature C), its tolerance zone is a cylinder, the diameter symbol can’t be omitted.

SeasonLee

 

[Belanger]

It sounds like you're coming at it from the inspection side. But just in case you have any input on the design side, the other posts here do have valid points. (In fact, the notion of a radius being a "feature of size" has generated much debate on this forum!)

Taking what you have right now, the .3700 hole is given an initial position tolerance of Ø.010. So the actual location of .78 by .78 will be within the position tolerance no matter what size the hole and/or datum is. (Recall that the stated tolerance of .010 allows the actual axis to drift .005 in any direction.) But let's push the situation a little further...

If the hole's size is at .3705, then the tolerance stays at Ø .010 -- this is by definition the LMC of the hole. But if the hole's size is .3695, then the position tolerance actually swells to Ø .011, or a radial tolerance of .0055. Now the hole's axis could actually drift out to x=.7817 and y=.7817.

But there might actually be times when the axis could drift even further! This is where the other "L" symbol on the datum comes in. However, here's the tricky part: Does the straightness callout really hang under the dia. 1.200 dimension? If so, then it has to be factored into our discussion of "L" on the datum reference. (I wonder if the straightness is really applied to the surface elements, though).

In general, the idea is that if datum feature C is made at sizes smaller than its LMC, then yes, you can think of that extra variation as extra tolerance to be added into the position tolerance for the hole.

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

 

[MechNorth]

J-P, the straightness is applied to the toleranced size making it a derived median line control, not a direct surface control. I'd like to see how they'd propose simulating datum-C at LMC.
SeasonLee, good catch ... I sometimes see what I expect to see rather than what I really see.
Also have an issue with the callout for Datum-C; just not valid, but I'm accepting that the OP meant to do it with a proper symbol.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[Belanger]

Jim -- I would have thought the same thing, but I wanted to verify from his print. That's because circularity can't be applied to a FOS, so either the straightness is on the surface elements, or the circularity needs to be shown separately. Thus, I posed the question back to the OP. If he says it really is on the FOS, then we'll have to deal with the VC of the datum, even though most people think the "L" in the FCF means LMC size.

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

 

[MechNorth]

Actually, and unfortunately, you can put the circularity control with the fos dimension; see Fig. 6-9 in '04. I thoroughly dislike it, but it is allowed in the standard. I tell my students I'll rap them on the knuckles if I catch them doing it. I tell them that any control applied to the fos size dimension is a control of the axis, center plane, derived median line or derived median plane ... so people tend to confuse a circularity/cylindricity callout on a fos callout to be controlling the same; unfortunately you need a better understanding of those controls to know that they apply exclusively to the surface.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[Belanger]

I personally don't have a big problem with it, since by definition there's only one way to interpret circularity; it's akin to showing a runout tolerance under the size dim. Thankfully, the new standard doesn't show that practice anymore (except for the AVG diameter, but of course that's not a feature of size).

So I'll go along... let's assume the straightness is meant to be on the FOS. It should then have the Ø symbol in front of the .010, and BrandNew, let us know if you want to see how the numbers are crunched for that last fudge factor called "shift tolerance."

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

 

[dingy2]

I am going to chip in on the original question and the subsequent drawing.

LMC is the opposite to MMC but the "bonus" tolerance is calculated the same method -the actual measured size of the feature from the virtual condition size.

In the first drawing, you placed a positional tolerance on a radius. As Jim stated, a radius is not a feature of size - 1.3.32.1 of 2009 standard. Profile of a surface or line is more appropriate.

You also have the reference datum at LMC. Although this might be theoretically correct, I have only seen it applied once in the 23 years that I have been involved in GD&T. It was applied on both IDs of a radiator hose. One would have to force the rubber hose onto a mandrel of LMC size (or virtual/LMB depending) in the checking fixture. The material was somewhat expandable and could expand over the mandrel with maybe a little assistance from some sort of lubricant. Other than that situation, I cannot see its practicality.

In the second drawing, the rad of .300 could be changed to a diameter of .600 and is a feature of size since one could measure across the diameter. One could still argue, in this situation, using a rad. could still constitute a feature of size since we can measure across it as per 1.3.32.1 of 2009 standard.

Straightness of the ID of the tube is not practical since I would love to see anyone measure it. Even a CMM would only be able to contact so far on each end but the centre?? - wouldn't happen. If you really needed to control the straightness of a long ID, use 0 at MMC and one would make a straight pin of 1.195 that must enter the tube and exit the tube with the force of one finger.

Roundess of an ID can be confirmed but not that well. One would take many points around the ID perpendicular to the axis.

Both straightness and roundness are best utilized on ODs rather than IDs since they can be confirmed with at least a 85% confidence level.

Straightness with a diametrical tolerance zone means the derived median line or axis (fig 5-2 page 92 of 2009)while without a diametrical tolerance zone (as your example) means each longitudinal element (fig. 5-1 also on page 92. Without a diametrical tolerance zone in the FCF, Rule 1 applies meaning that in your case the bend cannot be less than cylinder of ID 1.195. With a diametrical tolerance zone applied, Rule #1 does not apply.

Just my 2 cents worth.

Dave D.

http://www.qmsi.ca

 

[MechNorth]

Dave,
Interesting example of a somewhat valid use of an LMC-modified datum reference; I like it. Agree that it's pretty much useless elsewhere.

The tab doesn't look like it's a rull rad at the end (to me); it looks like it has a small flat/straight segment, which would eliminate it as an FOS. Even if the rad is full, it would only qualify as an FOS at the two opposed points which isn't actually locating the radius, just the tangency points wrt the axis. Technically legal at that one pair of opposed points, but useless in reality.

Also agree that the controls on the bore are rather useless beyond the first few inches at each end in this size of part; in that case, a limited zone of application should be indicated. On larger parts though, with a large enough bore, a CMM would perform just as it would for an external diameter. We all need to check our blanket statements for robustness; I guess that's part of the function of this forum too.


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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[MechNorth]

Also, re Fig. 5-1, read along with it Section 5.4.1.1; ..."The feature control frame is attached to a leader directed to the surface or extension line of the surface but not to the size dimension." That is what makes it a surface control, not whether or not a diameter symbol is present, though a diameter symbol on a surface straightness control would be incorrect for its own reasons.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dingy2]

You are correct, Jim, so the application of a straightness tolerance under the size of the feature without a diametrical tolerance zone is, basically, no man's land. It could be argued that there is a axis bend of no more than .010 in alignment (one direction only) with the top hole but is that what is required? I don't think so.

In most cases, I believe that Designers require a certain maximum axis straightness rather than longitudinal surface straightness. If one cannot contact the Designer for clarification, I would assume a diametrical tolerance zone. In this situation, it doesn't make any difference since the straightness of an ID such as shown cannot be confirmed with any degree of confidence. To control straightness of an ID with any length, reflect straightness at MMC.

Dave D.

http://www.qmsi.ca

 

[MechNorth]

Dave, I don't see it as legal to have the straightness of a derived median line for a cylindrical feature as being anything but diametral; there is no guidance in the standard on how to interpret it otherwise. Straightness of a derived median plane, however, would be legal only without the diameter symbol. I agree with your suggestion to shift to a 0(MMC) condition with accompanying size change. I warn my student's it's another knuckle-rapper if I catch them using straightness of a derived median line or derived median plane without having an MMC on it, and I also recommend they shift to a 0(MMC) condition which, as I remind them, is thus redundant as a the new size limits give the same control by Rule #1.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dingy2]

Jim - Fig. 5-2, page 92 reflects a diametrical tolerance zone for cylindrical features meaning axis or median line. It is an assumption that without a diametrical tolerance zone it would mean a median line. It could also be assumed a surface straightness but the FCF was not shown correctly. The drawing should either reflect fig. 5-1 or 5-2.

Do not expect that Rule #1 will be checked. It isn't. All dimensions are numbered by Quality and if there is no distinct dimension, no number will be issued and, thus, not checked. I did a private seminar recently and when I asked the CMM Operator how he approached Rule #1, he didn't know what I was talking about. Even after we went over Rule #1 (some find confusing), he said that if it isn't shown in a FCF, it is not checked. From a Design perspective, your butt is covered but that doesn't help your company, only one department.

MMC is conducive to a checking fixture and may not be appropriate when there is a production run of one. If the part has small long hole where straightness is mandatory, it cannot be checked unless it is MMC. Even on low production runs, MMC is the only way to go in this situation. I remember one company did not want me to discuss MMC at all - didn't do that seminar.



Dave D.

http://www.qmsi.ca