Equivalence of XY and compound true position tolerances 3

[imagitec]

The hole-to-edge toelrance in an XY tolerancing scheme is roughly equivalent to the pattern locating (1st) part of a compound true position tolerance. And the hole-to-hole tolerance is roughly equivalent to the pattern (2nd) part of a compound true position tolerance.

Assume the hole-to-hole and hole-to-edge tolerances locating a pattern are +/-.005" and +/-.02", respectively. The equivalent pattern tolerance zone would be .007" in diameter. What should the diameter of the pattern locating tolerance zone be? Most manuals I've seen say .03", and I think that's wrong.

In the pattern tolerance, two holes are involved, each with a .007" diameter tolerance zone about its true position. If the axes are located at opposite extremes of their tolerance zones, the distance between them will be plus or minus .007" from nominal.

In the pattern locating tolerance, only one hole with a .03" diameter tolerance zone about its true position is involved. This implies that distance from either locating edge to the actual position of the hole can be at most .015" from nominal. That is tighter than the Cartesian tolerance. To correct this, the diameter of the tolerance zone should be .057".

Am I correct?

Thanks,
Rob

Rob Campbell, PE
Finite Monkeys -

http://www.livejournal.com/users/robcampbell

 

[drawoh]

rjcjr9,

ASME Y14.5M-1994 has tolerance formulae worked out in their appendix. You might want to look at this. I sat down a few years ago and work a lot of this stuff out myself. I needed a reference, and I could not find one at the time.

http://home.eol.ca/~hgibson/tolerances.pdf

In summary, your tolerances are affected by whether your fasteners are floating or fixed (ASME terminology), and by the number of fasteners in the pattern. If you have only two fasteners, the tolerance relationship is one dimensional, not two.

The maximum geometric tolerance for a two dimensional floating fastener pattern is the minimum hole clearance. The maximum geometric tolerance for a fixed fastener is half the minimim hole clearance.

You did not mention any of this, but you should take it into account.

Geometric positioning tolerances generate a circular tolerance zone instead of the square or rectangular tolerance zone of linear tolerances. The two systems are not really equivalent.

I do not think the composite tolerances in your example are equivalent either. In your example, you located hole A to +/-.02" in two dimensions. You located hole B and possibly C and D from hole A to +/-.007" in two dimensions. My interpretation as per ASME Y14.5M-1994 is that your pattern and its tolerances are orthogonal. The maximum rotation is 2x.007"/length.

Both elements of the composite positional tolerance apply to each hole in your pattern. This allows your pattern to be out of position by .015", and rotated by 2x.15"/length.

The .03" positional tolerance is not equivalent to a +/-.02" linear tolcrance. In a strict mathematical sense, the requirements of a .03" positional tolerance will be met by a 2D linear tolerance of +/-.01", approximately. By this, I mean that an error of .01" in two orthogonal directions will remain just within the .03" circle defined by the positional tolerance.

JHG

 

[imagitec]

I unnecessarily complicated the problem by referring to a hole pattern and a composite tolerance. A better example:

Today, your company does not use GD&T. Tomorrow, your company will start using GD&T. You must convert all the drawings to use true position tolerancing. You are redlining a drawing in which a single hole is located relative to two edges. The edge-to-hole tolerance is +/-.02", and +/-.02" is the most correct tolerance using the current system. What true position tolerance would you assign? According to the figures on pages 113 and 115 of Modern Geometric Dimensioning and Tolerancing, 2nd ed[/] by Lowell Foster, you would assign 0.03. As I explained in my original post, I think this is incorrect.

Rob


Rob Campbell, PE
Finite Monkeys -

http://www.livejournal.com/users/robcampbell

 

[diamondjim]

I am with JHG. You have to
know the hole size and bolt
or fastener size to determine
the true position required on
the holes regardless of what
you have used in the past.
What clearance hole is defined
on page 113 and 115. It must
be a consideration.

 

[drawoh]

Rob,

I am being somewhat pedantic when I insist that 2D linear tolerances and GD&T positional tolerances are not equivalent. We can assume that we are solving a standard assembly problem like making fasteners fit.

Let us take the case that your design is intended to make a nut and bolt pass through a hole located in a 2D pattern from two orthognoal edges. Assume that your holes are 1/16" larger than your bolts.

Your 2D linear tolerance is +/-.022". This defines a .044" square centred on your nominal position that the hole must be located within.

Your positinal tolerance is .062". This defines a .062" diameter circle centred on your nominal position. The circle contacts the corners of the square defined above.

ASME Y14.5M-1994 is a dimensioning and tolerancing standard, and as such, it defines whatever tolerances you apply to your drawing. In addition to GD&T, it explains the meaning of your original linear tolerances. Conversion to GD&T might be nothing more than adding a note that your drawing is to be interpreted as per ASME Y14.5M-1994.

The positional tolerance defines a larger area for the hole to fall within. If your inspectors are rejecting a lot of parts because holes are not located properly, then the GD&T positional tolerance could be a cost saver.

If you are not having problems meeting specification or assembling parts, then it is probably not worth converthing everything.

I convert a linear tolerance of +/-.02" to a positional tolerance of .06" diameter. I do not have the textbook you are refering to, so I do not know how they got to .03", or just what the .03" is. Converting from a +/- error in one direction to a geometric diameter tolerance is confusing.

If you are doing the conversion, perhaps the best thing to do is work everything out from first principles.

JHG

 

[imagitec]

I understand the method for calculating the maximum permissable tolerance for a pair of mating hole patterns. That doesn't apply in my second example* - we have a single hole located relative to two edges. The correct, functional tolerance on each linear dimension is +/-.02". That's a given - it's part of the problem statement. Let's say the nominal x- and y-dimension are both 1 inch. So the tolerancing permits the hole's axis to fall within a 0.04" X 0.04" box with opposite corners at (0.98, 0.98) and (1.02, 1.02).

One of the limitations of Cartesian tolerances is that they define rectangular tolerance zones (it's even worse if you use, for example, a bolt circle and angles to locate holes). If (1.02,1.02) and (0.98,0.98) are both good points, and they're both .03" away from the nominal position, why aren't (0.97, 1.0) and (1.0, 1.03) also good points? Hence, the circular tolerance zone used in true position tolerancing.

Based on the above discussion, any point within a .03" radius of the true position should be considered good. That would be a 0.06" true position tolerance, since it is specified as a diamater. Yet _EVERY_ reference on GD&T I've seen specifies a 0.03" true position tolerance. Either the writers are sloppy being sloppy or I am wrong in my understanding.

Based on his last reply, I think JHG would agree that the references - at least the few I have that cover the subject - are wrong. Maybe his and yours are too, but uou haven't noticed. This is a real problem.

Many applications do not justify a thorough tolerance analysis. Typically, a reasonable tolerance that is a straight-forward conversion of cartesian tolerances is applied. Every GD&T resource I've seen has worked examples for hole-to-hole tolerances. None have explicit examples dealing with hole-to-edge tolerances. The only information is in the form of before-and-after figures of the same part dimensioned using cartesian and true position tolerancing - and they're always wrong. An engineer or designer who follows this example will apply tighter than intended tolerances.

A side note: the method of calculating permissable tolerances traditionally given in GD&T manuals is of little practical in all but the most trivial examples.

Thanks,
Rob

* This discussion is valid for my first example, too, because I was referring to the pattern locating tolerance. But referring to a composite tolerance only seemed to confuse the issue.



Rob Campbell, PE
Finite Monkeys -

http://www.livejournal.com/users/robcampbell

 

[imagitec]

JHG wrote:
--- quote ---
I convert a linear tolerance of +/-.02" to a positional tolerance of .06" diameter. I do not have the textbook you are refering to, so I do not know how they got to .03", or just what the .03" is. Converting from a +/- error in one direction to a geometric diameter tolerance is confusing.
--- end quote ---

That would be correct if it is a pattern locating tolerance or the position tolerance on a single hole relative to datums, as described in my earlier post. It would be twice as loose as you intended if it is used as the pattern tolerance for a hole pattern - the second part of a composite true position tolerance:

Given a rectangular hole pattern, imagine a rectangle, rectangle A, with sides equal to the nominal dimensions. At each corner is a circle of diameter equal to the pattern tolerance. Imagine the axes of the holes as gas molecules, allowed to float anywhere within those circles. When two axes on the same edge are as far apart as those circles allow, they will be nominal + tolerance zone apart. When they are as close as the circles permit, they will be nominal - tolerance zone apart. So applying a true position tolerance of .06 translates to a cartesian tolerance roughly equivalent to +/-0.04, not +/-0.02.

Now imagine another rectangle, rectangle B, with corners at the nominal (basic) hole positions. At each corner is a circle of diameter equal to the pattern locating tolerance. Rectangle A - maintaining perfect form - may float anywhere so long as the smaller circles attached to its corners do not go outside of the larger circles attached to the stationary rectangle B.

Any set of holes that satisfy that requirement satisfies the composite true position tolerance.

Rob

Rob Campbell, PE
Finite Monkeys -

http://www.livejournal.com/users/robcampbell

 

[CanEngJohn]

For simple but effective conversion make areas equivalent on edge to hole locations. So a bilateral tolerance of [±].02 would work out to a Diametral tolerance of .045. For hole to Hole locations I would make your [±].02 a .04 diameter and develop a MMC bonus into the spec based on clearances.

Be careful when reading your GD&T texts. Many read a tolerance of .02 converts to .03. A tolerance of .02 to them is equal to [±].01. Wheras in your example your [±].02 is a .04 tolerance to them. This is a common mistake because in the linear to GD&T thought transfer we forget that GD&T is about tolerance zones (both sides combined) instead of [±].

 

[drawoh]

CanEngJohn,

In other words, it is the .02" tolerance I do not understand. Modern Geometric Dimensioning and Tolerancing sounds like a good book to not read. Why can't they work with the numbers that people actually put on drawings?

JHG

 

[drawoh]

Rob,

ASME Y14.5M-1994 is quite readable. If you are determined to implement it, I cannot see why you would read anything else. The standard uses something like nineteen pages to explain composite tolerances, and I think it answers your question. There is no substitute for all the graphics they use.

When I took my GD&T course, the instructor had a set of tolerance tables in which the MMC tolerances were set to zero. This confused the hell out of us, but it allowed the instructor to make a point. I cannot remember what it was. I have not used these tables since. The ones in the Machinery's Handbook are much more practical.

Perhaps these textbooks are structured as part of a course you did not take.

I have my GD&T classroom notes on my shelf, but if I have a question, I pull out my copy of the standard. You might as well go straight to the source.

JHG

 

[CanEngJohn]

drawoh writes

Why can't they work with the numbers that people actually put on drawings?

That is actually the point. They are changing what people put on drawings. The change is to move to "True Position" instead of "[±]". It is a different way of defining a good part.

The problem is when you have to go back and forth between the two. They are not equal and cannot be translated from one to the other. They can only approximate each other.

It is actually easier to start from scratch and figure out what you need in the new system than trying to convert from one to the other.

 

[drawoh]

CanEngJohn,

There is a case for +/- tolerances for holes. You have a note that assigns a +/- tolerance to a given number of decimal places. This standard tolerance is accurate enough to ensure assembly of your part. Your fabricator can easily work to this tolerance, and your quantities are small. Your drafting time is a significant part of your cost. Why waste time applying fancy tolerances?

JHG

 

[CanEngJohn]

Because they may not make a good part.

One of the major problems with bilateral tolerancing is it is common to create aggregate errors which cause complex systems to not line up. Ask Pratt and Whitney. They ran into this hard about 20 years ago when my dad was working there.

Imagine a 20 million dollar Jet Engine which is being built. You get to the last few pieces and they are not quite going together. There is supposed to be clearance on two of these pieces but they are binding.

What do you do?

They started to rip the engine apart looking for the part that was out of spec. Weeks later everything has been ripped apart and measured repeatedly. Every single part was found to be in spec.

What happened was a bunch of bilateral tolerances lined up in extreme corners between mating parts. Round parts fitting into round holes with square tolerance zones. They stacked up in such a way that they could not put the engine together. They experienced what is known as Aggregate Errror.

Since then they have moved to circular tolerance zones on many of those parts (True Position) to eliminate the corners which caused the problem Round hole, round post, round tolerance zone. When I originally heard about this from my dad I immediately asked "Why use a square for a round hole with a round post?"

In GD&T there are methods to define square zones. This is done primarily using datum selection. Also GD&T still allows bilateral tolerances on its prints. In essence you have added flexibility to your system. You can keep your note with specified decimal tolerances. Too often have I had a toolmaker forget to check those tolerances. The result is a habit of putting it in front of his nose if it is remotely important.

 

[drawoh]

CanEngJohn,

You are describing a situation where the specified tolerances were not accurate enough. It sounds like it was hard to fabricate to them anyway, and I do not know how much of the cost of a jet engine is eaten up by drafting time. Most of the conditions I mentioned above are not being met here.

If my drawings are going to result in a twenty million dollar engine, I am going to work out my tolerances very carefully, and I am going to by very nervous around any design that accumulates tolerances.

JHG

 

[CanEngJohn]

What I am driving at is that there is solid justifcation to use GD&T for some applications. The only way to make a good part is to apply the right specification in the best language. One of the interesting points from the above story is that they eliminated the problem by changing the system and not by tightening up the specifications. (They did not change their accuracy but they changed their precision.) While I did use a dramatic example this concept has worked well for me in many daily applications.

Quite often I don't use GD&T in my prints on the basis that it isn't the best way to describe what is being made. But if I need a bolt circle to be concentric to a rotating shaft you can bet I will take the extra 2 minutes to make sure I have the correct GD&T on the print. Those [±] dimensions are not going to cut it more often than not.

 

[ccw]

The geo positional tolerance is a circle of xx DIAMETER, the center of the hole is allowed to float around in it. Since most holes/fasteners are round or circular, this is a more liberal representation of hole center location tolerancing. Now, back to the orthogonal to GD&T redimensioning problem posed.

The +/- .02 edge to hole tolerancing would generate a square zone .04 x .04 for the hole center to float around in. In this case, assuming the orthogonal tolerancing scheme allowed for a workable fit in the extreme and knowing nothing else, to assure that the intended assembly will still work, one should be conservative and INSCRIBE the circle in the square, so the geo-pos. tolerance diameter would be computed as .04. However, if one determines that this tolerance was specifically for round fasteners or pins, and round holes, then the liberal interpretation of CIRCUMSCRIBED circle outside the square would be applicable and the geo-pos. tolerance diameter would be .0566.

 

[drawoh]

ccw,

The shape of the GD&T tolerance zone has nothing whatsoever to do with the shape of the feature being located. It exists because you can tolerate a maximum linear error in any direction. This defines a circle.

There is no theoretical reason why you cannot apply a positional tolerance on a square feature or some other polygon with an obvious centre. The only practical problem I can see is that the GD&T profile tolerances probably are more appropriate.

Let us look at the case where, for some reason, I want to broach square holes in a part into which I will press-fit square locating pins. The broached holes must be controlled for position. The GD&T position tolerance is absolutely appropriate for this. You do need to control rotation as well, somehow.

Here is another thought. The GD&T positional tolerance explicitly calls up a circle. I can see no theoretical reason why I cannot substitute some other piece of geometry, such as a square. The truly quick and dirty conversion for rjcjr9 would be a .04" square.

This was not noted anywhere in ASME Y14.5M-1004, and I cannot think of an intelligent reason to do it.

JHG