Why Place MMC in Reference Datum when tolerance is in RFS? 3

[dingy2]

I see this so often and I wonder the purpose of placing a reference datum at MMC when the tolerance is shown in RFS.

Let's say, as an example, we have a profile of a surface tolerance of 0.2 mm referencing primary datum A, secondary datum B (RMB) and tertiary datum C (in MMB). What is the purpose of having a datum in MMB when one must actually measure the profile tolerance on a CMM? I know that it is legal (nothing in the standard stating otherwise) but what is the value or purpose?

I can see when one has a profile of a surface tolerance of 3 mm and the secondary and tertiary datums are at MMB, one can utilize a checking fixture with the outer and inner profile tolerance boundaries shown on a checking fixture but a tolerance of 0.2 mm??

In another situation, one has a positional tolerance of a diametrical tolerance zone of 0.3 in RFS while the secondary and tertiary datums are at MMB. Shouldn't the positional tolerance also be reflected at MMC or should both the positional and reference datums be reflected at RFS/RMB?

I have always been blown away with the application of MMB on the reference datums while the tolerance is in RFS but this may have something to do with my background in measuring rather than designing.

Maybe some of the Designers here could help me out on this one.


Dave D.

http://www.qmsi.ca

 

[fsincox]

Dave,
It really depends on where the bonus come from, the first exapmle that comes to mind is calling out a tapped hole pattern to clearance holes. The general traditional definition of tapped holes says they do not work MMC so. I know people do not like it but if we go by function and not gaging, we would default to RFS. I believe gaging is not done on the majority of manufactured parts.
Frank

 

[dingy2]

Frank:

When you are talking about tapped holes, I believe that you are thinking about positional tolerances at MMC. If your drawing called out a pattern of tapped holes in RFS and then referenced the secondary and tertiary datums at MMB, now there is a problem.

If the holes are in RFS and datum were also in RMB, no problem. We could measure the tapped hole location (using a checking plug in each hole) simulating the pitch diameter.

Dave D.

http://www.qmsi.ca

 

[fsincox]

Dave,
Thanks, Yes, I was and I was not aware of this as a "real" problem. I admit I have never had to measure these, thought. I have never seen anyone advocate blind MMC on threads, though it is pretty clear the shop wants them. There are always caveats, to engineers that means to be safe use RFS.
Frank

 

[MechNorth]

Interesting question, Dave.
On the profile control, I completely agree. I always tell my trainees that "It's legal, it's just not useful, so put your profiles at RMB". When asked if it's ok if they put MMB with a MMC on the profile, I explain that MMC isn't legal ... it's like saying "check where the actual surface is by running the indicator (cmm, etc.) at the MMC" ... you just get air for the most part.

As for position of a threaded featurea at RFS with MMB, I see it all the time. It's almost like they're saying "get the SPC data", then let it shift around. Typically, RFS isn't needed for these, though as Frank said, "to engineers, that means to be safe use RFS." As for gaging (gauging) threads, I don't advocate the use of pitch cylinder; in any case other than one or two holes, the cost of the plugs and the usage time is prohibitive for cost. I strongly urge people to look at using major diameter for male threads and minor diameter for female threads. Several international studies have now concluded that there is no significant nor reproducible differences in the results and it's a lot faster & cheaper. For reference, Sandia Nat'l Lats did some studies in the '90s, and DIN (I think it was DIN, or the German National Standards Institute) around the same time frame. I've heard of at least one other study more recently, but I can't recall the source. Pretty much the same results from each.

The larger problem is that designers typically don't know enough about manufacturing and inspection to make good choices about modifiers, and typically manufacturing and inspection don't know enough about the design and function to understand the design intent and why the specific controls and modifiers were selected. As a result, I see too much "fiddling" and selective interpretation. Design "previews" with cross-functional teams is the answer but most companies don't understand this, and only get the groups together in the "review" stage, when it's too late.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dingy2]

Thanks Jim:

I see both all the time and although it is legal, it is not practical and, to me, reflects that the Designer does not understand its meaning.

So, to sum it up, on all profiles, the datums should be in RMB. One cannot measure a surface that is allowed to move. The part should be stationary.

As far as positional tolerances, if the tolerance has a MMC modifier, then the datums may also, but not necessarily, be in MMB. The datums could be in RMB and one could still measure or gauge the part. If the positional tolerance is in RFS, then the datums should also be in RMB. Having the datums in RMB just doesn't make sense since we are in a measuring method only.

I do agree with both Frank and the assessment on threaded features.

As GD&T trainers, we should not reflect drawings that are not practical but I have seen them.

Does this makes sense to you?

Dave D.

http://www.qmsi.ca

 

[Belanger]

I don't think it's at all impractical to have MMB with a profile tolerance. What if it's a cosmetic cover plate for some sort of instrument panel? Suppose there are 4 corner holes that are attachment points; this is where the MMB comes in. And then a cutout in the middle of the plate might fit over something; this is where the profile tolerance is applied.

On reading your OP, Dave, I think you agree that this is OK. Your question is particularly about the tertiary datum being MMB, right?

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

 

[pmarc]

Dave,

So, to sum it up, on all profiles, the datums should be in RMB. One cannot measure a surface that is allowed to move. The part should be stationary.

I have to respectfully disagree with this statement. There are also other methods of verifying profile than probing the surface by CMM. You can for instance scan the part without touching it, so the part will not move during inspection. You can use optical comparators too. Having datum references at MMB enables to adjust the part (best-fit alignment) to fit into boundaries defined by profile tolerance zone. Of course I agree that using MMB concept should be done based on functional requirements, but I would not arbitrarily say that this is poor practice in case of profile tolerances.

As for positional tolerance I can even imagine situations when specifying tolerance value at LMC with datum features at MMB makes practical sense. So again I would be careful with such statements.

 

[dingy2]

J-P:

Thanks for your input since this has bothered me for quite a while. I do agree that you are simulating assembly by having the 4 holes as a datum at MMB. If the actual profile of a surface tolerance is large, say 3 mm, then I can see having a checking fixture with the outer/inner boundaries scribed. We can move the part for the best visual fit.

Now, let's say we have a tolerance of 0.2 mm, we would not have a checking fixture here. I know that if one took it to the CMM room, the datums would be set up in RMB.

As far as a secondary reflected at RMB and the tertiary in MMB, wow, that is a problem.

I think that I would take back my original conclusion and say that there may be times when a profile of a surface could reflect the secondary and tertiary datums at MMB. Most of the time, it is not practical. Any Designer applying MMB on datums when we have a profile tolerance should be able to justify it in some manner.

Thanks again.



Dave D.

http://www.qmsi.ca

 

[dingy2]

pmarc:

You stated "I have to respectfully disagree with this statement. There are also other methods of verifying profile than probing the surface by CMM. You can for instance scan the part without touching it, so the part will not move during inspection. You can use optical comparators too. Having datum references at MMB enables to adjust the part (best-fit alignment) to fit into boundaries defined by profile tolerance zone. Of course I agree that using MMB concept should be done based on functional requirements, but I would not arbitrarily say that this is poor practice in case of profile tolerances.

As for positional tolerance I can even imagine situations when specifying tolerance value at LMC with datum features at MMB makes practical sense. So again I would be careful with such statements."

Yes, I have used optical comparitors in my past but only on very small parts since we explode the view 20X. Yes, we could make templates too with the inner and outer boundaries shown. If the secondary and tertiary datums were holes, one could scribe in the MMB in, say, the 4 holes and jockey the part around to get the best fit. This is the use of a checking fixture rather than actualy measuring the feature though. I do agree with you here but this is a special case.

If the part is large or reasonable in size, then we do have a problem with datums at MMB. The part must be stationary to actually measure the feature.

As far as positional at LMC and the datums at MMB, I can see that. Having the positional tolerance in RFS and the datums at MMB, is not practical. We want to check the actual centre of the features and the datums can float at MMB?? The datums would be taken at RMB and then the centre of the features confirmed.

I take back my blanket statement but Designers should be able to justify why a datum is reflected at MMB while the feature is measured at RFS.


Dave D.

http://www.qmsi.ca

 

[pmarc]

Dave,

Maybe the Tec-Ease tip will somehow help:

http://www.tec-ease.com/gdt-tips-view.php?q=135

 

[dingy2]

pmarc:

Yes, the Tec-Ease Tip confirms what I had stated. We could use MMB on datums with profile of a surface if it is to be confirmed on an Optical Comparitor sometimes known as a shadowgraft. It is also stated that it cannot be confirmed (very difficult) using a CMM or most other measuring equipment.

The application is quite limited. If you can somehow make a checking fixture on either an optical comparitor or checking fixture, then it can be used. Otherwise, it does not apply.

Thanks for the info.

Dave D.

http://www.qmsi.ca

 

[MechNorth]

Again, as Don points out, it's practical on paper gauging, vision systems, optical comparators. Most software packages for CMMs do NOT address datum shift adequately in general and for profile specifically (the last time I looked was about 2 years ago, I think though it could be longer).

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dingy2]

So, to sum it up again with your input:

Positional tolerances in RFS should be referenced in RMB and not MMB. We cannot measure the centre of a hole that is not restrained. We will obtain an actual position of the feature using measuring equipment such as a CMM.

Positional tolerances in MMB can be referenced in either RMB or MMB. In both cases, a checking fixture is best to confirm this requirement. When we have the reference datum at MMB, then a cylindrical pin would go into the feature of size or inside the boundary. If the reference datum is RMB, then a tapered spring loaded cone would locate in the feature of size or enclosure. A translation symbol (revision 2009) should be placed on the tertiary datum as applicable.

Using a CMM to measure the above is not recommended since, as Jim stated, most CMM software does not address datums at MMB. This method is OK when the datums are shown in RMB but not MMB. Usually, the CMM Operator would simply transfer a RMB to the datums which isn't quite correct.

Back to Profile of a Surface since this created the most controversy.

If one had a requirement of Profile of a Surface 0.2 which defaults to a +/- 0.1 about the true profile. If we actually measured this surface, we could get an actual reading of, say, +0.06 and - 0.09 which is not outside the requirements. It appears that we have satisfied the Profile of a Surface requirement.

We can only use MMB on a datum in conjunction with Profile of a Surface when one is confirming the requirement using a checking fixture. The checking fixture or template could be used in conjunction with an optical comparitor (Shadow Graph) on small parts or other optical measuring equipment. If the Profile of a Surface tolerance is large enough (say 3 mm), we could make a visual checking fixture with the outer and inner boundaries scribed on the surface. The part can jockey on the datums shown at MMB until we get the best fit. The only result would be OK or NOT OK since checking fixtures are attribute gauges. We will not obtain actual measurements.

Checking Fixtures used in Profiles - Usually Profile of a Surface is 3 dimensional with the primary datum as the mounting surface and in our case, the secondary and tertiary datums are features of size (per 2009, can be a surface also). The checking fixtures described above are visual and are only 2 dimensional. The fixture does NOT confirm surface perpendicularity to the primary datum. It is possible to have the Profile of a Surface requirement deemed OK with the visual checking fixture but the surface is not perpendicular and could actually be out of tolerance. This checking fixture does NOT address all the requirements of Profile of a Surface. Should we use a checking method that does not address all the requirements of Profile of a Surface? If not, Profile of a Surface should be referenced in RMB only.

Thanks guys for your help on this.



Dave D.

http://www.qmsi.ca

 

[MechNorth]

Not sure what you mean by "We cannot measure a hole that is not restrained."
With the comment I made re CMM software not recognizing/addressing MMB/LMB, it doesn't make it inappropriate necessarily, but it does mean that paper plots must be done manually to address the datum shift. It's another step that most users don't recognize needs to be done.
Where you have "defaults", I'm thinking that you mean "roughly equates to".
Re datum modifiers on a profile control, I think that the paper plots mentioned above may still be applicable, though I haven't done this yet. I will keep that in mind for future consideration as time allows.
Your comment that Profile is a 3-D control maybe comes up short. Most Geometric controls are 3-D, with the exception of straightness, circularity, profile of a line and circular runout on a nominally cylindrical surface offset from the axis.
Your observation re projection method inspection is dead on, and should only be used for shallow depths otherwise you get ghosting (parallax?) and other issues.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[dingy2]

Morning Jim:

Whenever we actually measure a feature, it must be held in some fashion or restrained. Whenever we have a datum shift coming from the datum referenced at MMB, the shift is manually performed using a checking fixture, template or some other attribute gauge. If we use a CMM, as an example, we still would set up on the datum as if it were in a RMB (restrained) and then the size of the datum feature is "somehow" accrued into the tolerance of the feature. Most CMM software that I have experienced does not have this capability and the few that do have it, I wonder about how the programme was developed and how appropriate the results are.

I mentioned "default" in the Profile of a Surface since the tolerance defaults to a range of of a bi-lateral tolerance, half above and half below the true profile.

I stated that most Profile of a Surface is 3D and I think that is true. If we use profile of a surface on 3 planes that are co-planar similar to a flatness requirement, is that really 3D? I think that it is more 2D so I think my previous statement is correct.

Thanks for your comment.



Dave D.

http://www.qmsi.ca

 

[axym]

Dave,

This is a very interesting thread. I strongly disagree with some of your statements, but I know that there are many others who would share your position. You have brought up some very good points of discussion.

My main issue is the underlying theme of the inspection method driving the design. To me, your statement that "designers should be able to justify why a datum is reflected at MMB while the feature is measured at RFS" has the tail wagging the dog. If the fit and function of the part makes datum feature shift possible, then the designer should reference the datum features at MMB. Inspection always has the option of inspecting the part as if the datum features were referenced at RMB, and not making use of the datum feature shift.

I agree with the others that it is fine to have a profile tolerance with datum features referenced at MMB. Or the secondary at RMB and the tertiary at MMB. If that's how the part fits, that's what should be specified.

Dave, I definitely agree with you that specifications like these can cause us difficulties in inspection. There are a lot of things in Y14.5 that are gaging-friendly but measurement-unfriendly. It might be easy to get a pass/fail result with a gage, and very difficult to get a repeatable numerical value with some other method. This is especially true for datum features referenced at MMB. Most CMM software still does not handle this very well. Some softwares can do the required constrained optimization, or "virtual jockeying" if you will, but most cannot. Some softwares have limited functionality, in which they can best fit patterns of holes with Position tolerances or groups of surfaces with Profile tolerances, but not both at the same time.

All of this is assuming, of course, that our intent is to optimize the GD&T to maximize tolerances within functional requirements. If our intent is to optimize the GD&T for simplicity of inspection or to mesh with a given inspection method, then a lot of things will be different. What if we know that the parts will be made by a vendor that only has calipers and mic's available in their shop - should we just specify plus/minus tolerances in that case?

Should "they can't inspect that" be a valid reason for not specifying a particular functional requirement? This is definitely a can of worms.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[dingy2]

Hi Evan:

ASME Y14.5-2009 does not get into inspection methods or application in most cases except in the forward stating that GD&T should reflect the function and relationship of the features. Sometimes, the standard does try to reflect a practical point of view.

Here is an example.

Section 4.8 Datum Features (page 57 of 2009 edition) states "However, a datum feature should be accessible on the part and of sufficient size to permit its use. Datum features must be readily discernible on the part." This appears to state a practical perspective when utilizing features as datums.

I agree that GD&T should be driven by the Design or utilization of the product --- BUT --- it should be practical. Having Profile of a Surface with the secondary and tertiary datums at MMC is not practical unless it can be confirmed with a checking fixture or gauge of some sort. Even with that type of gauge, one does not confirm all the requirements.

I disagree that the person running a CMM has an option of applying or not applying the datum shift. There is nothing in the standard stating this option. We do it but it is wrong. It simply means that there is no way of fully confirming the requirement as it stands.

Many, many years ago, we used to call the people in design "Ivory Tower Boys" because some of the designs just were not practical. Over the years, Design personnel have integrated with Manufacturing and Quality to work together as a team to make a robust part at the least cost possible. If the design is not practical in a certain area or a design could be changed to facilitate assembly without compromising the design integrity, it was changed.

I was a Quality Consultant in the automotive sector and involved in Design Review. I always remember the philosophy at that time and it should be prevalent today. If the feature cannot be measured, it should not be on the drawing. That was a practical approach.



Dave D.

http://www.qmsi.ca

 

[MechNorth]

Dave,
There is a certain baseline element in your last statement. However, that's a blanket statement rather than a finite one; I have come across many parts which cannot be gauged and should not be gauged (aerospace, communications/electronics, others). The reality is it all depends upon the industry, and upon the individual component. Still, if western companies want to survive and hopefully thrive, they need specialists to come together on previews rather than reviews and get things right before ink meets paper.

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

http://www.profileservices.ca

TecEase, Inc.

http://www.tec-ease.com

 

[fsincox]

I was hoping someone whould raise an exception to this, no offence but, if it works MMB it is MMB wheither you can inspect it or not, IMHO. It really sends conflicting signals to all when we say this is the standard but don't use it like that!
Frank