GD&T Runout @ MMC?

[Matthew Hajicek - Singularity]

I'm out of practice on my GD&T.  I want to specify on a print that I'll accept .002" runout between two diameters of a hole at the maximum material condition (smallest holes), more if the holes are larger.  What would that look like?  Thanks!

[MattW]

Since no one has jumped in yet-  I've been told that position covers 80% of GD&T, so make sure you really need something else if you use something else.  In this case, it sounds like position is what you want.

According to this chart, runout is always applied RFS.

GD&T Color Chart.pdf

[Matthew Hajicek - Singularity]

OK, here's what I did so far.  You're saying I should use true position instead?  Turned part.

Thanks!

 

[Mr. M]

Yes, position with MMC is what you want.

[Matthew Hajicek - Singularity]

This look right?  Similar but different part with the same issue.

Edit: Forgot the MMC.

[MattW]

You are in bad shape if you are relying on me for GD&T help.

I think the datum A symbol needs to be attached to the extension line, not the dimension line, but I would have to check into that.

You probably want a diameter symbol in your .004 tolerance block.

You have your tolerance to A applied RFS.  That may be what you want, I'm just pointing it out in case you want to (or can) apply the tolerance at datum A MMC.

I like to draw out the limits of what I think the tolerance block allows in an attempt to see if I can make sense of it.

[Matthew Hajicek - Singularity]

Doesn't the "M" in the circle mean at MMC?

[MattW]

The circled M next to the .004 means the axis of a .195 hole is inside a .004 circle around the axis defined by datum A RFS.  a .197 hole is inside a .006 circle.  There can be no material inside a .191 cylinder on the axis defined by datum A.

If you determined the actual size of A by a gage pin, and then turned an end down to .191 on your perfect lathe, that end would fall through the .196 hole feature.

If the tolerance to datum A can be applied to A at MMC. a .233 gage pin with a .191 end goes through and position is verified.

 

 

 

[crazy^millman]

1 hour ago, Matthew Hajicek™ - Conventus said:

Doesn't the "M" in the circle mean at MMC?

Yes you are correct it does mean that. The bonus comes from the large size of the hole. The smaller the hole the less bonus they will gain.

[Matthew Hajicek - Singularity]

18 minutes ago, MattW said:

The circled M next to the .004 means the axis of a .195 hole is inside a .004 circle around the axis defined by datum A RFS.  a .197 hole is inside a .006 circle.  There can be no material inside a .191 cylinder on the axis defined by datum A.

If you determined the actual size of A by a gage pin, and then turned an end down to .191 on your perfect lathe, that end would fall through the .196 hole feature.

If the tolerance to datum A can be applied to A at MMC. a .233 gage pin with a .191 end goes through and position is verified.

OK, I get what you're saying now.  So if I want the latter how do I specify that?

[MattW]

a circled M next to A in your Feature control frame.  So you will have two circled M s, one next to your tolerance and one next to datum A.  Note that this effectively loosens the position tolerance, which may or may not be what you want.

[Prodoggg]

 If you would like to use MMC on both the feature the control frame is referencing and the A datum the correct way to do so is to have a circled 'M' after both the .004 and after the A datum callout. You should have a dia. symbol before the .004 in the feature control frame. This will give you a bonus on the .196 hole of one to one as the feature departs from its maximum material condition (at .197 you would get .002 dia. bonus). The way the additional bonus is gained, in this case, is also one to one as the datum A feature departs from its maximum material condition. The only other thing to consider is that the envelope rule applies so the cylinders are straight within the tolerance zone. So whatever fits in the holes will indeed fit. I hope this helps. 

[taperlength]

My book on geometric tolerancing says that if coaxiality is the prime consideration, then a Concentricity callout is preferable to a True Position.  The same MMC can be applied to both the feature and the datum.