×
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

TWO HOLE DATUM FOR ATTRIBUTE GAGE

TWO HOLE DATUM FOR ATTRIBUTE GAGE

TWO HOLE DATUM FOR ATTRIBUTE GAGE

(OP)
We're building an attribute gage for production and incoming inspection.  Two holes on the part are selected as a datum. There is both tolerance on the hole sizes and positional tolerance on the two holes.  Should the gage  pins for these two holes be sized only for variation in the hole size or a combination of hole size tolerance AND positional tolerance.  ... if another feature control frames references this datum, is the positional tolerance for these two datum holes to be taken into account?

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

That depends on how you are referencing the datums. If the position tolerance for the holse is at MMC and that all the feature controls be gaged reference the holes at MMC then your pins would be the minimum hole dia - the position tolerance at MMC. If the condition is RFS then you need to use pins that center on the holes.

Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services
www.infotechpr.net

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

Wicsteve,

   I assume your two holes are selected as secondary and tertiary datums.

   There is no positional tolerance on a hole used as a secondary datum.  You define the hole as being in the right place.  Perhaps the outside edge of your part is in the wrong place!

   There is a positional error in your second hole, but this is one dimensional.  There can be no rotation error around your secondary datum, because your tertiary datum is defined as being in the right place.  Again, your part's outline could be wrong.

   If your second datum hole is a slot, or your pin diamond shaped, you do not need to worry about the positional error of your hole and pin.  

   If hole and pin are round, you need to locate both to ±C/2, where C is the clearance between your pin and hole.  The standard position tolerance works too, but you should leave out the diameter symbol.  Your error is one dimensional.  The positional tolerance is C.  Slots or diamond pins are a much better idea.   

               JHG

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

drawoh, it could be that the two holes taken together are a single datum...

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

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

Wicsteve - what are the drawings tolerances/datum scheme/dimensioning scheme  that you are trying to check to with this gauge?

When you say "Two holes on the part are selected as a datum" do you actually meant the 'pattern' is the datum per ASME Y14.5M-1994 4.5.8 & figure 4-22?

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

(OP)
This is a secondary datum and is created from a pattern of two holes. The part is a two hole flange with attached tube (welded and bent). The tube end, away form the flange, is the feature who's position is to be controlled with reference to these flange holes. The tube end's feature conrol frame calls out the positional tolerance with reference to this datum at datum's maximum material conditions. The intent is that in assemblying the part, both holes are mounted over studs at the same time and as long as the tube end can be manuvered in place within the tolerance zone, then it is acceptable for the application.


 

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

Quote (Belanger):


drawoh, it could be that the two holes taken together are a single datum...  

    A pattern of more than two holes would change my reasoning.  I think my analysis is still valid if you have two holes.  

               JHG

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

Belanger,

   On second thought, it does matter.  If I have a secondary and a tertiary datum, it is clear which one controls rotation, and should be slotted or diamond pinned.  The holes and pins can be very accurate, and in most cases, I would not care about MMC.

   If the two pins are a single datum, the oversized hole and the ± tolerance between the holes cause locating slop.  Is MMC a meaningful concept here?

   Making two round holes fit over a stud is easy.  The ± tolerance between the holes and between the studs is half the clearance.  The overwhelming probability is that the assembled piece will move in X and Y, and it will rotate.  From the OP's description, it is possbile that the lineary translation due to rotation, is magnified at the tube end.  Mathematically, this sounds nasty, although it could be a good assembly strategy.

               JHG

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

Wicsteve,

   Okay, your two holes are your locating datum.  You are trying to locate the tube end close enough for assembly.  Your test fixture must simulate your mounting studs.  

   Your two pins are very, very accurately located at nominal position.  Their diameter is the stud diameter plus the stud's positional tolerance.  You may want to CNC mill this all out of steel billet to get the best possible accuracy.

   If your part goes over these pins, it will go over any conforming set of studs.  You can now test your tube to see if it can be moved to its assembly position.  If it can, your part will work with any conforming set of studs.   

               JHG

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

(OP)
Part of our problem is that our QC staff measured the part on a CMM. They randomly selected one of the two holes, rotated the part to aligned the other hole, then made measurements to the tube end from the center of the first hole (and by the way declared the part to be out of tolerance). In my way of thinking they changed the datum declaration to fit their CMM measuring scheme. Further, their result may have been different if they had selected the other hole first.

I believe they should have located the origin for their measurements, from a point half way between the two holes (measuring the distance between the two holes, then calculating their midpoint).  This I think would have the same result as if the fixture's locating pin diameters accounted for both hole size tolerance AND distance tolerance between the two datum holes.  Our QC staff believes that tube end which references the MMC of the two hole datum, only allows for the hole size variation (bonus tolerance) and does not include any allowance for positional tolerance between the two datum holes. That doesn't make sense to me because if we made those flange holes larger to fit loosely over the studs on the application we should be allowed even more real tolerance for the tube end.

So the big question... For a datum created from a pattern of two (or 3, 4, 5 etc) holes, is the distance tolerance (positional tolerance) between the datum holes part of the datum's definition or not?   Implication - In the past I've often redistributed positional tolerance allotment between the datum holes (pattern of holes) and a subsequent feature, usually giving more allowance to the more difficult dimension to hold. If our QC people are correct, I should not have done this since the datum and feature positional tolerance are completely independent of one another (except for hole size tolerance).

Please forgive me if I ramble. Drawing is enclosed.
 

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

I'm pretty sure the case of a hole pattern as a datum has been discussed in great length before.

I think Paul Jackson went into detail on what inspection jigs he might use.  I think he used some kind of roll pins or spring pins to have some give so the inspection fixture centered on the hole pattern.

You may be able to find it, it was a while back and got pretty long.

Posting guidelines FAQ731-376: Eng-Tips.com Forum Policies http://eng-tips.com/market.cfm? (probably not aimed specifically at you)
What is Engineering anyway: FAQ1088-1484: In layman terms, what is "engineering"?

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

Having the picture sure helps!  For your original question: a functional gage can be designed and the two pins would each be dia. 8.51. This is the smallest size minus the allowable position tolerance.  (I'm assuming perfect gage pins of 8.51 -- any tolerance on the gage is a whole separate discussion).

When measuring the position of the tube, any looseness around those two gage pins can be used to your advantage: you can shift the part around the pins (while always maintaining primary contact on datum feature A) until the tube appears in the right place. So the tolerance on the two holes does have an effect on the position tolerance of the tube, but it's not directly added in as "bonus" tolerance would be; it's an indirect effect that is sometimes called "shift" tolerance.

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

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

Wic steve,

I have a couple of questions relating to the part and your definition of it.  What version of Y14.5 is applied on the drawing.  How is the attachment of the tube end made in the next assembly.  This information would be of value in determining the proper definition and attribute gages.

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

WICsteve:

Datum B is qualified by having 2 holes in position at MMC to each other and perpendicular to datum A. The virtual condition size in this situation would be a diameter of 8.51 mm. That virtual condition diameter is not only the diameter of the pins that will be used to check for the positional tolerance of the 2 holes but ALSO will be the pins for datum B when one is making a gauge for the tube position as per ASME Y14.5M-94. ASME Y14.5 - 2009 is a bit different in requirements at MMC but in your situation, it would be the same virtual condition size of 8.51 mm. One will gain tolerances from the datum holes depending upon the hole sizes.

Using a CMM, one cannot duplicate the requirement of having both holes as a datum or checking both holes to themselves in MMC. As a matter of fact, just checking the hole to hole position requires that the CMM Operator would use one hole as a datum and then check the other hole to the first hole. One will also have a discrepancy checking the tube position relative to the 2 holes at MMC. A CMM is just not an appropriate measuring method here.

If the CMM finds holes out of position and the gauge (properly made) accepts the holes, the gauge supersedes the CMM. I would suggest purchasing ASME Y14.3-2003 for tolerance applications for attribute gauges. It is absolutely great and it really clears up the muddy area of attribute gauges and related tolerances.

Hope this helps.

Dave D.
www.qmsi.ca

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

(OP)
First, thank everyone for their comments. They have been helpful.

ding2,  So, for the case of datums created from a pattern of holes, there really isn't anyway to correlate and make measurements on a CMM to parallel those of a go-no go attribute gage?  What do others do for ISIR submittals?

... and I'm glad you recommended buying ASME Y14.3 I really wanted to hear that before spending $90.  

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

WICsteve:

Customers usually will not accept an attribute gauge check for positional tolerances on an ISIR and insist on variable readings. Some even go so far as to ask for capability studies which is a bit of make believe.

If the CMM accepts the positional, no probs, just report it. If the CMM does not but the gauge does, big problems now. I would then report it as an attribute gauge and then wait and see.

Dave D.
www.qmsi.ca

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

I'm certainly not a CMM expert, but are you guys saying that the CMM software has no way of taking the measurement of the two holes and carrying that "shift" factor over to the position calculation of the tube?

I know it isn't a direct linear correlation, but I'd be real surprised if there isn't some algorithm to account for that.
 

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

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

J-P:

Hopefully on your next seminar you will have someone who is a CMM Operator such I have had some many times in the past. Just ask them how they approach the datum holes at MMC. You will find that they set up in a RFS condition on the holes so there is a datum shift gain and your CMM could reject the part while a properly made checking fixture could accept it.

I have had only one person in this forum who claims that there are programs out there that do, in fact, take the MMC condition of the datum holes in consideration but I have not had anyone in my seminars who have actually used a system like that.

   

Dave D.
www.qmsi.ca

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

Dave -- I am in the same situation. In 15 years of full-time GD&T training, I've met many CMM operators, and if I ask them, they say "Well we just ignore the M symbol on the datum." (I usually don't ask now, because it just displays that they never really understood the MMC concept.)

Now would you say that they are inspecting the part correctly? smile

There must be some way to account for this in the software.

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

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

Gentlemen,
A basic alignment and measurement by CMM would not be able to take into account a "shift" factor, how would it know which way to "shift"?

This is why Best-Fit was created, and, why most CMM software includes Best-fit. If not, Best-Fit can be an add-on package.

All the Best-Fit packages we have seen and used allow operator control on XYZ rotation & XYZ shift. Thus the MMC value can be input. This allows a CMM to be a "virtual floating check fixture", that will reject bad product and accept good product.
 

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

HGMorgan:

Yes the best fit packages allow the Operator to take many readings on a diameter and the CMM will come up with the best fit diameter discarding the largest and smallest readings. It can also calculate the tolerance using MMC on the feature BUT allowing a shift on a datum at MMC???

We could, in one case, have a datum shift tolerance between the actual size and its MMC size while the other datum feature could be between its actual and virtual condition size. If the software allows one to rotate and shift the part manually, I love to watch a CMM Operator explain how one shifts the datum to correspond with the requirement.

J-P

Using a CMM and having the datum holes at RFS while the drawing states MMC does not correspond to the requirement and the part is not inspected correctly.

Dave D.
www.qmsi.ca

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

dingy2:
The Best-Fit process is not taking several readings on one feature (Dia.) and then discarding largest and smallest readings. Best-Fit is taking readings on ALL the product features and then letting the software shift them to the closest average values from nonminal.

The Best-Fit process:
1. Align product per Datums
2. Survey (take points on) ALL features.
3. Run Best-Fit by setting the limits on XYZ rotation & XYZ shift per Eng Dwg tolerances. This creates "Soft-Gage" zones.

For this example:
XYZ Rotation: -A-(Z) would be allowed to rotate with-in the FLAT 0.4 zone. B (XY)would have free rotation, the two holes are going to lock in the angle.

XYZ Shift: -A-(Z) would be locked, B (XY) would be allowed to shift TP Dia. and any MMC bonus obtained from the survey of the actual hole diameter.

This is "how one shifts the datum to correspond with the requirement".

On our software, this would be set-up one time, and then ran on all the separate products without any intervention from operator.

A "Virtual Floating Check Fixture" that buys the good and rejects the bad. This does work, and the need for it is why Best-Fit was created.

 

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

Wicsteve,

It seems unlikely that you would want the positional tolerance of the send of the tube to apply for the entire straight portion.  Hence the question that I had posed earlier, with regards  

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

(OP)
RESTEDUP

Background (or more than you really want to know- Extra credit reading) -- The application is for a small engine assembly. The tube end passes into an extruded hole of an exhaust muffler. In reality, about 12 mm of the tube end actually is engaged, even though our print calls for checking 25.4 mm of length.

We had an issue in our customer's assembly plant because the manifold is first assembled to the engine and tightened down prior to final assembly of the muffler.  There appears to be too much allowable adjustment or swing in the manifold assembly due to the loose fitting flange holes and the assembly plant has difficulty in centering the tube. The customer doesn't have an attribute gage for this part but measured the part on their CMM using the upper flange hole as the origin. They declared the part out of tolerance even though it passed our attribute gage. We then got into a discussion with our QC people who checked the part on our CCM also using the upper flange hole as the origin for measurement. So went the discussion with multiple opinions as to which is correct, gage or CMM.  

This whole posting was started to resolve the question of part measurement and to understand the issues between CMM measurements (for ISIR, PPAP) and the attribute gages. We normally supply our customer and our factory with CMM data at the startup of a program but check production parts with an attribute gage. I'm afraid that engineering, manufacturing, and QC aren't sledding on the same hill in this regard. Also note that many of our manifold have two flanges (for twin cylinder engines).  Common practice is to use attribute gages to check (all four holes are used).  Yes, I know that only two holes should be used for a datum but the four hole method is sort of self-centering and more practical because "it's how the part sees the engine".

By the way, we probably will make the flange holes smaller to reduce the allowable swing. ... or the manifold  might need to be fixtured while being assembled to the engine.  The latter is more time consuming and harder to accomplish on our customer's assembly line. The assembly plant has resolved the issue in part, by re-centering the tube to the midpoint of allowable swing before assembling the muffler (usually by the means of a swift stoke with a hammer). We're still working out a solution with our customer.  
 
Finally, when this print was made we were attempting to comply with  ASME 14.5, 1994 standard.
 

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

Wicsteve,

Tightening the holes would not seem to help the problem.  I would think that to open them would aid the fit of the tube into the exhaust muffler.  The datum identifiers   with the dashes are not in compliance with 1994.

I would think it would help also to limit the extent of the gage for the tube end to cover the engaged portion only which can be done by limiting the length. (Chain Line comes to mind.)

To my knowledge not stated in any standard, but MMC works well with atribute gages whereas RFS is better suited for CMM.  

Dave moderately hit on this idea in his post.

 

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

As long as we're talking about the 1994 standard, it might be a good idea to use the "boundary" notation for the position tolerance on the tube.
 

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

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

J-P:

The tube end is round and "BOUNDARY" is not required using the 94 standard. This termed is used on non-round features of size when reflected in positional at MMC.  

Dave D.
www.qmsi.ca

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

Wicsteve,

- I am just curious - you said that your customer declaired part of out the tolerance, but which tolerance from the drawing was actually out of spec?

- If I understood you well, normally you are going to use hard gage simulators for specified datum features to fix the part during the inspection, am I right? If yes my question is how are you going to assure that the part will not wobble when put on planar datum A?

J-P, Dave,
I think a good example of dealing with such tubular elements is again shown on Tec-Ease site:
http://tec-ease.com/gdt-tips-view.php?q=128

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

(OP)
Getting off the subject
Small holes -- The problem at our customer's assembly line is that when the flange bolts are tightened with an air wrench,  the flange tends to rotate about the stud center (more or less).  Making the holes smaller would, to some degree, limit the the amount of rotational movement possible.  The manifold apparanently is not fixtured when assembled and can move.  I know that the operator does, by hand, position the tube to some extent but can't hold it from shifting about when the nuts are tightened.

Datum identifier -- You know, I'm still inserting dashes with the datum identifier. Never noticed that they aren't to be there. Thanks, as I'd have gone on for years without making the change.
 

RE: TWO HOLE DATUM FOR ATTRIBUTE GAGE

Right Dave -- thanks for the reminder! MMC equates to boundary to begin with.

 

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

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