Unilateral composite profile problem

[sendithard]

Can

 

[sendithard]

Dear lord what happened to the forums......

I got this callout recently....the problem I see is the top segment locates and sizes the feature within .100.
Then the lower segment asks for the feature to be oriented to A, then further refines the size/form to a .05 tol zone.

If the part falls in the PLTZF that is great....but remember bc if it one-sided the PLTZF is in one direction from the basic dimension. So when we try to conform to the FRTZF, how is that size component calculated? It should be calculated from the middle of the road surface. But I'm getting odd results.

 

[sendithard]

The bottom line is I think the tolerance zones in the callout conflict....you have one at .100 and another at ,05 but they are in one direction so the center of the tolerance zones are not the same.

 

[pmarc]

Have you taken into account the fact that the smaller tolerance zone does not have to fully lie inside the larger tolerance zone, and that what needs to lie within both is the actual feature?

 

[SeasonLee]

I think composite profile tolerance can only be applied to an irregular feature of size or pattern of features, the round hole in this example is just a regular FOS, and that’s why I think composite profile tolerance is not a proper callout here.



Season

 

[pmarc]

SeasonLee,

I am not sure I see a problem with a composite profile applied to such a simple feature. In fact, I see some benefits in doing so (such as that no one will then need to worry if size of the feature is inspected properly).

There is definitely nothing in the standard that would prohibit doing this.

 

[sendithard]

The callout can be applied to a regular feature like this. pmarc, it took me a second to understand what you were saying, but yes I agree the feature must rest within both, but you could have a tol zone break thru the boundary of the larger zone...as long as the part is inside both you are good...but that isn't what I'm concerned about here.

The problem with this callout is that because it is a one sided tolerance the tolerance band origin is pushed away from the part surface .05 on the top segment and then the origin of the tolerance band for the bottom callout is pushed only .025 from the surfaces. We know that the bottom tolerance on a composite restricts the size of the feature to be more accurately made to the basics, but it shouldn't change the nominal of what the size of the part should be made at. In this callout, the top segment says, 'hey make this diameter at 20.1mm' and then the bottom callout say 'hey make this diameter at 20.05mm.

How this should be done in my opinion is make the basic at 20.05mm and use a normal composite callout with .1 tol on the top and .05 tol on the bottom and everyone knows to make this feature at 20.05mm in diameter. Unfortunately, with one sided composite, you wouldn't get a 0 measured value for the top tolerance when you make the part properly at 20.05mm dia.

 

[jassco]

Hi, Sendithard:

This statement below is false as this feature does not have a specification for its size which is indirectly controlled by the profile tolerances.

"but it shouldn't change the nominal of what the size of the part should be made at."

Your part is good as long as both of the profile tolerances are met.

Happy Thanksgiving!

Alex

 

[SeasonLee]

pmarc

I cannot find any example of composite profile callout applied on a single round hole from the standard, all examples with composite profile tolerance callout are irregular FOS or pattern features.

We can see this word “PLTZE” very often from standard, which means the top segment controls the location of the pattern and is referred to as the Pattern-Locating Tolerance Zone.

The single hole is not a pattern of features, and so I do not think composite profile is a right callout here.

Season

 

[sendithard]

Season,

This is just an example, but it doesn't matter if there is one hole or 10 holes. The problem remains the top tol zone prefers a diameter of 20.1 and the bottom tol zone prefers a diameter of 20.05. I'm of the opinion this should never happen. If you make the part at a perfect size when you report a measurement for both feature callouts you should get a 0 value if the location and size is perfect. In this case if you make the feature at 20.05 the bottom callout would measure 0 and the top callout will have a measurement value error of some amount. Since it is looking for 20.1 and the part is made at 20.05, that would mean the surface is radially out by .025 so the measurement value on the top segment would be recorded at .05. The problem with this is you just lost 50% of your tolerance if it was stated at .100 and that is the problem I am dealing with. You shouldn't ever lose tolerance if you make the part at a perfect size and location.

 

[jassco]

Profiles are supposed to be attached to surfaces. Attaching profiles to a size dimension is probably invalid, and thus is not advised by ASME Y14.5.

The upper segment is to locate the pattern with .1 while the bottom one is to refine it to 0.05 in reference to datum A only.

Best regards,

Alex

 

[pmarc]

SeasonLee,
Please take a look at para. 11.6.1 in Y14.5-2018 to see that composite profile does not require a pattern. They even have terms for the larger and smaller tolerance zones.

I am pretty sure you will find a corresponding paragraph in the 2009.

 

[pmarc]

Season,

This is just an example, but it doesn't matter if there is one hole or 10 holes. The problem remains the top tol zone prefers a diameter of 20.1 and the bottom tol zone prefers a diameter of 20.05. I'm of the opinion this should never happen. If you make the part at a perfect size when you report a measurement for both feature callouts you should get a 0 value if the location and size is perfect. In this case if you make the feature at 20.05 the bottom callout would measure 0 and the top callout will have a measurement value error of some amount. Since it is looking for 20.1 and the part is made at 20.05, that would mean the surface is radially out by .025 so the measurement value on the top segment would be recorded at .05. The problem with this is you just lost 50% of your tolerance if it was stated at .100 and that is the problem I am dealing with. You shouldn't ever lose tolerance if you make the part at a perfect size and location.

I am not sure I would look at this from the perspective of measured values.

What this combined callout tells you is that if the size of the hole (which is just a resultant thing here / not reportable directly) is 20.1 and the hole is perfectly perpendicular to A (which is another thing that you don't directly measure), the hole may still float a little as long as it does not violate the 20 and 20.2 boundaries. And this is the condition of the hole for which there is the maximum amount of the float. As the hole gets smaller or tilted relative to A, the amount of possible float will decrease.

 

[sendithard]

I feel similar to you on this as in the end all works out nicely, but the wrinkle here is that I have a machinist making the feature at 20.05 and obviously the hole has some deviation in X and Y location so the top profile callout they don't get the full .100mm of tolerance. They only get .050mm of tolerance with regards to location, bc they used up .050mm of tolerance due to size. I've handled this internally by creating a nominal sized feature in cad and using a normal zone instead of uni directional. I'm on the end where failed parts hit my desk and production will find these cracks rather quickly here. All of the software we are using spits out a bad result for the top callout due to the issues mentioned above.

 

[Burunduk]

sendithard,
I think you are missing something.
In this composite tolerance the bottom segment is what really controls the size. It refines size, form, and orientation to A. The top segment doesn't really tell you anything about the ideal size, it just defines the floating range.

 

[sendithard]

I agree in theory, but you have to extract a measured value from both callouts, otherwise you don't have a value to pass or fail a part.
The measured value of the top callout is based on a diameter of 20.1, so if you make the part correctly at 20.05 that measured value throws up a false flag. It isn't a problem if you make the basic diam at 20.05 and use a normal tol zone, but there is a flaw in using a composite with unilateral tol zone.

Do you agree you must extract a measured value from both segments for reporting and pass fail metrics? And do you agree that if the feature is made at 20.05 with perfect form and size that the top callout would report a measured value of .05mm?

 

[jassco]

Hi, sendithard:

Are you a designer or a quality engineer? If I were you, I would not advise your machinist on how he or she machines this part.

I assume you are not a quality engineer. Otherwise, you would not ask this question below:

"Do you agree you must extract a measured value from both segments for reporting and pass fail metrics?"

You have 2 specifications here.

Specification #1: .1 unilateral/unequal tolerance.

Specification #2: .05 also unilateral/unequal tolerance.

You measure this feature against these two specifications above.

Best regards,

Alex

 

[Burunduk]

sendithard,
I think I am sort of starting to understand what you are saying, but I would suggest you to post an illustration of the conflict to convince the others there is a problem. Once the problem is graphically clarified the efforts here for solution/conclusion will be more effective.

 

[pmarc]

sendithard,

Imagine the callout for the hole in question was changed to this:

Dia. 20.0-20.1
|POS|dia. 0.1 (L)|A|B|C|
|POS|dia. 0 (M)|A|B|C|
|PERP|dia. 0 (L)|A|

Would you see any fundamental problem with any of the 3 FCFs and with them living together (apart from that this definitely would not be a commonly seen combination)?

 

[sendithard]

Burunduk, I have a good graphic later to post, I just need to improve it for clarity.

pmarc,

Walking thru your example on paper:
Dia. 20.0-20.1
|POS|dia. 0.1 (L)|A|B|C| The hole at LMC is 20.1 and you get no bonus here. At 20.0 you get additional .1 bonus. Hole can be at most .1mm away from TP.

|POS|dia. 0 (M)|A|B|C| The hole at MMC is 20.0 and you get no bonus here. At 20.1 you get additional .1 bonus. Hole can be at most .05mm away from TP.
The only issue I see with both those is the LMC callout allows the feature to be farther from TP.