×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Bonus Tolerance Question, MMC on a Datum
4

Bonus Tolerance Question, MMC on a Datum

Bonus Tolerance Question, MMC on a Datum

(OP)
I have looked through ASME Y14.5-2009 and maybe I am blind, but I can't find what I'm looking for.  Attached is an example drawing.

How is the true position of the .056 hole affected by the MMC on datum B?  The hole has a .001 tolerance zone at MMC, so I can get a little bonus tolerance if I make the hole larger than MMC (to .056), correct?  If the hole ends up outside of the bonus tolerance, does the MMC on datum B give me more bonus to keep the hole in tolerance?

RE: Bonus Tolerance Question, MMC on a Datum

Yes, and since the tolerance on datum B is larger, this has the most bonus.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.
 

RE: Bonus Tolerance Question, MMC on a Datum

This would be covered in paragraphs 4.11.5 through 4.11.9 in the 2009 standard.  It can sometimes be rather tricky. You already have a handle on the bonus from the hole that's being positioned (as you say, making it at .056 will gain the full bonus there).

But because of the M modifier (properly called MMB, since it's slightly different than MMC), there may be even more position tolerance available.  You have to look at ALL of the variation on datum feature B, not just its size.  The total variation on B could be .016 (.006 size tolerance and .01 perpendicularity).  The standard calls this extra .016 datum shift.   They do that to distinguish it from "bonus," which is technically only the fudge factor on the small hole (the .002).

The bonus tolerance makes the position tolerance grow.  The datum shift doesn't really make it grow, but allows it to shift or "play" as if you had the part on a gage fixture and it jiggled a little.  But in this case it's safe to add bonus and shift to the given position tolerance and treat it as if it were one grand total.

 

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Bonus Tolerance Question, MMC on a Datum

Look at fig. 7-18. I belive this is something you are looking for.

RE: Bonus Tolerance Question, MMC on a Datum

(OP)
So the .056 hole doesn't shift relative to the shifted datum B?  With that scenario, the .056 hole still has a .001 position tolerance with .002 bonus tolerance.

RE: Bonus Tolerance Question, MMC on a Datum

Well, your last post might be correct but we have to clarify the terms.  The .056 hole can move within a .003 position tolerance relative to the perfect datum B (I get this from the .001 stated tol + .002 bonus tol).  But the extra "M" after the B says that the real, actual datum hole (which we call datum "feature" B) could shift within a .016 zone from the perfect datum B, if the real hole were at .114 and perfectly perpendicular.

That might sound weird, because I'm saying that the hole we call datum B might deviate from the actual, true datum B.  There's the rub. (Think of a physical gage fixture that we drop this part onto. A gage pin of .104 would be used to simulate the true datum, which we call MMB.)

Now put it all together: if the .056 hole moves within .003 relative to the perfect datum, and the actual hole that the datum is derived from moves within .016 from the perfect datum, it's like saying the distance between the two actual holes could be within a total range of .019 (translate: max = .1675 and min = .1485 axis to axis).  Again, these numbers are only true if both holes are made at their smallest size and are exactly 90º to A.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Bonus Tolerance Question, MMC on a Datum

Correction to my last sentence:  these numbers are only true if both holes are made at the biggest size and are exactly perpendicular to A.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Bonus Tolerance Question, MMC on a Datum

I was about to make a comment here until I reviewed the perpendicularity tolerance on datum B. Is it really .010 or is there an error and the tolerance should be .001? Something is not correct especially since the perpendicularity tolernace is in 2 decimal places while all the other tolerances are in 3 decimal.  

Dave D.
www.qmsi.ca

RE: Bonus Tolerance Question, MMC on a Datum

(OP)
The drawing is "correct" with the .010 perpendicularity tolerance.  The folks who created this drawing are known for their GD&T funny business.

RE: Bonus Tolerance Question, MMC on a Datum

cfordyce05,

I hope the explanations given by the others are clear for you, because I would like to add that presence of (M) modifier following datum B within positional FCF's would have no impact on any relationship between .056 hole and other features which are controlled by positional tolerance with relation to the same datum reference frame A|B(M).  

RE: Bonus Tolerance Question, MMC on a Datum

(OP)
It is clear now.  Thank you all.

RE: Bonus Tolerance Question, MMC on a Datum

I would rather talk further more about the MMC on a datum than to create a new thread.

As you can see on the OP, there is a material condition modifier (MMC) on the secondary reference datum B, all above are talking about the datum shift and its calculation, but no one asked "why" and "when" a MMC is needed on the FCF.

Quoted from a GD&T book: When a cylinder, hole (or FOS) is used as a datum feature, any FCF that reference the datum feature must include the material condition MMC or LMC,...

I just want to know "why" and "when" MMC is needed on the FCF. Thanks for the forum provided this learning environment.

SeasonLee
 

RE: Bonus Tolerance Question, MMC on a Datum

SeasonLee, the book is wrong.  If it said that M or L is required for a datum created by a pattern, then I might buy it; even that isn't an absolute requirement.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Bonus Tolerance Question, MMC on a Datum

If its an older book to the pre-1994 standard could they mean that it had to have M,L, or S? If that's the case then I guess technically it's true because the S is implied if no modifier is shown.

If it's a newer book than it's wrong.

Dan

Han primo incensus

RE: Bonus Tolerance Question, MMC on a Datum

Wow, that is poorly worded!

The book is trying to say that since the datum feature isn't a surface, then it must be simulated correctly -- not just setting the part onto a surface plate or gage table.   So it must be one of three things: MMC, LMC, or RFS (or in today's parlance MMB, LMB, or RMB).

That paragraph does allude to Rule #2 ("assume RFS"), so I guess all is OK.  But that one sentence isn't right, no matter how you slice it, because of the parentheses.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Bonus Tolerance Question, MMC on a Datum

John: Sorry for the misleading, I should quote exactly from the book.

From that figure, you can see the MMC on the referenced datum A, I am still interesting to learn "why" and "when" MMC is needed on the referenced datum.

SEasonLee

RE: Bonus Tolerance Question, MMC on a Datum

No apologies needed.  That sentence is flat-out wrong.   It would be correct if it were:

"When a cylinder...is used as a datum feature, any feature control frames that reference the datum feature must include the material condition (MMC, LMC, or RFS) under which the datum feature simulator is to be constructed."


At any rate, one of those three is needed because a FOS can, of course, change in size from part to part.  So the designer needs to tell the inspector if he wants a fixed or variable hold upon that datum feature. RFS means that the inspector must hole the datum feature firmly, regardless of its actual size (and any GD&T).  But the M or L modifiers on the datum reference would imply that a constant-size gage is adequate, even if the part is loose.  (I'm simplifying it by explaining it in terms of physical gaging, because that's not practical with L.  But the general idea should make sense.)

When to use?   In its function, if the datum feature is a clearance fit, and a little looseness or play is acceptable, then the M modifier should follow that datum letter when referenced.  If the function dictates that the datum feature will be firmly held, like a press-fit dowel/hole, then the RFS condition is the way to go.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Bonus Tolerance Question, MMC on a Datum

I completely agree with J-P on this one.  That one sentence in the book is incorrect, and could easily lead the reader to an incorrect conclusion if they did not look into what Rule #2 states.  The idea is that a datum feature of size must be referenced at a certain material boundary condition - either explicitly with (M) or (L), or implicitly with implied RMB.

As far as why MMB or any other material boundary modifier would be referenced on a particular datum feature, fit and function of the datum feature would primarily drive this.  If the datum feature interfaces with a mating feature with a clearance fit (e.g. fixed size mating feature or fixture element), then an MMB reference usually makes sense.  If the datum feature interfaces with a mating feature with a self-centering fit (e.g. press fit, threads, adjustable or tapered fixture element), then an RMB reference usually makes sense.  If the datum feature will have material removed and must align the workpiece with a cutter path, then an LMB reference usually makes sense.  It all comes down to how the workpiece will be constrained to a datum reference frame (coordinate system) using contact with the datum feature surface.  If the datum feature is not functional and was chosen arbitrarily, then I would usually go with RFS as it will be the simplest and most repeatable (no issues with datum feature shift).

There may be other reasons to reference a datum feature at a certain material condition, that go beyond this simple analysis.  These usually relate to tolerance stackup considerations and limiting tolerance accumulation in assemblies.  For example, a datum feature that mates with a clearance fit might still be referenced RFS (or possibly even LMC) to limit tolerance accumulation in the assembly.

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

RE: Bonus Tolerance Question, MMC on a Datum

Can I say MMC modifier on the referenced datum will create a repeatable datum axis since it has a constant size gage?

SeasonLee

RE: Bonus Tolerance Question, MMC on a Datum

On each manufactured part, the datum feature might have an axis which deviates from the true datum. But yes, the datum repeatable because it is the axis of the worst-case cylinder, which is represented by the constant-size gage.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Bonus Tolerance Question, MMC on a Datum

From the fit and function will direct us the use of modifier, this is what I know on the feature modifier, but it's the first time I know this will also apply to the datum modifier selection. Thanks John and Evan.

SeasonLee

RE: Bonus Tolerance Question, MMC on a Datum

SeasonLee,

No, the constant-size gage element does not result in a repeatable datum axis.  It's the opposite.  Let me clarify what I mean.

The datum axis is defined in the gage element (datum feature simulator).  For MMB (and LMB) datum feature references, the size of the gage element is constant.  This means that there will generally be some clearance between the surface of the datum feature and the surface of the gage element.  There can be movement between the two(commonly known as datum shift).  The datum feature (and therefore the part) can have different relationships to the datum (and therefore the coordinate system).  There is not a stable or easily repeatable relationship.  

For RMB datum feature references, the size of the gage element is adjustable and shrinks/expands to achieve stable contact with the extremities of the datum feature.  There is no datum shift.  The relationship between the datum feature and the datum is stable and repeatable.

This is what I mean by the statement that the constant-size gage element does not result in a repeatable datum axis.  The relationship between the part and the datum axis is not repeatable.

Evan Janeshewski

Axymetrix Quality Engineering Inc.
www.axymetrix.ca

RE: Bonus Tolerance Question, MMC on a Datum

I thought of that too, Evan.  It all depends on what he means by repeatable.  Does it mean an axis we can find each and every time?  Surely a fixed gage does that, even if the part itself slops around. On the other hand, an RMB gage (or even a CMM scan) has many more variables that enter the picture.  So it's more stable, but it has more chance for something to go wrong.
But I do agree with everything you wrote.  

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

RE: Bonus Tolerance Question, MMC on a Datum

A MMC modifier will have a fixed gage, and the part can be measured repeatedly, is that correct?

Also, I noticed that when a hole pattern is used as a datum feature, it is almost always referenced at MMC, why?

SeasonLee

RE: Bonus Tolerance Question, MMC on a Datum

Well, the notion of repeatability is tricky.  Yes, a fixed gage can be repeatable in the sense of ease of measurement -- jiggle the part around and you'll be more likely to "repeat" a measurement.   But if you wish to quantify repeatability in terms of statistics, then Evan's take is probably more accurate.

As for the pattern datum, I'll again use the illustration of fixed vs. variable gaging.  If a group of holes is identified as a datum feature and then referenced at MMC/MMB, then a fixed gage is used.  Even if one the holes is not perfectly positioned itself, the notion of datum shift will still allow for the part to fit onto the gage.

But if we omit the M modifier, and the datum is referenced RFS/RMB, then recall the a variable gage is required -- we must have a gage that self-centers on each of the holes making up the datum.  Well the only way this is practical is if each hole in the datum pattern is perfectly positioned!  If just one of the holes of the pattern is off by a hair, then the gage isn't really finding the true center; it will bind up on one side of the hole first.

So it's mainly for a practical reason.  (Sorry I don't have time to create some sketches right now.)

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
http://www.gdtseminars.com

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources