Datum feature in line

[dodge78]

Please see attached. When the datum feature symbol is in line with a toleranced feature, does the bonus apply to positional when mmc is tagged

 

[powerhound]

You have to be careful in your perception of datum shift (if that's what you meant). In the case shown, you would get datum shift based on the size of the datum feature but keep in mind that your tolerance zone is not getting larger, it is only moving in a favorable direction. This gives the appearance of a larger tolerance zone but it's not. Note that I am only talking about the case you have presented.

When the circle M is in the datum portion of the feature control frame, it's not called bonus tolerance, it's called datum shift. Your question mentions bonus but the drawing shows the M in the datum portion.

Powerhound, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[dodge78]

I will try to be more specific, I have a callout of a T.P. of .012 to A @ MMC. Since the datum feature symbol is inline with the dimension, the "A" datum is the center of the 1.500 regardless of its size. Now that the 1.500 has a +/-.005 tolerance, if its actually 1.500, .005 under the O.D. max of 1.505, do I now have a positional tolerance of .017 since the 1.500 is .005 under MMC. (the M was meant to be penciled inside with the A, in the tolerance block)

 

[Belanger]

Looking at the left-hand picture only (in your original post), datum A is intended to be the center plane. But... we cannot say that it's the center "regardless of size." To really define datum A, we need to look at how it's used. So the feature control frame on the right explains how datum A is to be used: You've placed the "M" modifier there, so the true datum A is the centerplane of the block as if it were at 1.505. If the actual part is at 1.500, then yes there is an extra .005 that will somehow factor into the positional measurement.
It is permissible to say that the effective positional error between the two actual center planes will appear to have a .017 variation, but as Powerhound stated the position tolerance zone itself has not grown. Rather, the tolerance zone is still .012 but it's now allowed to shift around (because the item it's trying to position to has a slop of .005).

So again, your logic is on track, but in GD&T terminology we just have to be careful about how we say it.

It should also be noted that the logic presented here only works in simple cases where there's a single datum feature and it's acting in the same direction as the toleranced feature. If the notch were perpendicular to datum A, then the extra "datum shift" of .005 that we're talking about is not linearly additive.

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

http://www.gdtseminars.com

 

[powerhound]

I feel that I must reinforce JPs last paragraph that states that this "additive" tolerance only works in very simple cases such as you have presented. That's also why it's important to know that the tolerance zone is shifting, not growing.

To clear up one of your statements:

"the "A" datum is the center of the 1.500 regardless of its size."

No, since you added the MMC modifier, datum A is the center of a 1.505 wide boundary since the MMC of datum feature A is 1.505. Had you not added the modifier then your statement would be true.

Powerhound, GDTP S-0731
Engineering Technician
Inventor 2013
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[dingy2]

I just don't see the logic in using MMC on the datum and not in the positional tolerance. It is legal but try and find a logical application?? Usually, one had both the positional and the datum at MMC. That makes sense to me and one can also see both the positional in RFS and datum in RMB which also makes sense.

I think that we have had this discussion before though.

Dave D.

http://www.qmsi.ca

 

[Belanger]

Dave, I suppose the OP was just trying to understand the concept of "M" on the datum, so he isolated that one only.

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

http://www.gdtseminars.com

 

[pmarc]

I prefer to think about such situations in following way:

1. What is datum A?
As it was already mentioned, presence of (M) modifier after datum letter A in positional feature control frame causes that datum A is the center plane of 1.505 wide boundary.

2. What is size of positional tolerance zone and how is the zone located/oriented to datum A?
The tolerance zone is two parallel planes spaced 0.12 apart and perfectly centered on datum center plane. The size of the tolerance zone does not change (it is always 0.12), the tolerance zone cannot move or shift relative to datum A.

3. So what is actually allowed to shift?
It is the datum feature A (and in consequence the feature being positionally controlled) that can shift. If the size of datum feature is smaller than 1.505 (but greater than or equal to 1.495), and some initial results of positional callout check show that .500+/-.005 feature is out of its allowable position, the part can be adjusted (shifted) inside 1.505 boundary in order to make .500+/-.005 feature better fitting inside the positional tolerance zone. Example: if the size of datum feature A is 1.498, the part can be shifted up to .007 (1.505-1.498) to bring the toleranced feature back inside its positional tolerance zone.

As for logical application of this callout, imagine that OP's part must assemble with a slot of 1.505-1.515 width, and the .500+/-.005 groove must be centered to the slot and not to the width of OP's part. Wouldn't the callout be a way to go?