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?
Eng-Tips is the largest engineering community on the Internet
Intelligent Work Forums for Engineering Professionals
-
Congratulations waross on being selected by the Tek-Tips community for having the most helpful posts in the forums last week. Way to Go!
TWO HOLE DATUM FOR ATTRIBUTE GAGE
- Thread starter Wicsteve
- Start date
PeterStock
Mechanical
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
Peter Stockhausen
Senior Design Analyst (Checker)
Infotech Aerospace Services
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
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.
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?
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 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
- Thread starter
- #6
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.
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
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.
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
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.
- Thread starter
- #10
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.
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.
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.
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 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
thread1103-239885 thread1103-236974 thread1103-220967
I think one of them might have it in.
I think one of them might have it in.
Posting guidelines faq731-376 (probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484
What is Engineering anyway: faq1088-1484
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
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
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.
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.
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.
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.
- Thread starter
- #16
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.
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.
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.
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.
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
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
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.
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.
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]](/data/assets/smilies/smile.gif "[smile] [smile]")
There must be some way to account for this in the software.
John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
Now would you say that they are inspecting the part correctly?
There must be some way to account for this in the software.
John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems
- Status
Similar threads
- Locked
- Question
- Locked
- Question