Arriving Flatness and Parallelism tolerances

[Babups]

HI,

From the attached picture, Drawing from design team.

1. From my understanding the applied flatness and Parallelism tolerance can be Max upto size tolerance
applied(As per Rule 1).
Say for example : Size tolerance is within X + 0 /- 0.025
Flatness + parallelism can be within Max 0.025

Received drawing has got the flatness tolerance of 0.02 and parallelism tolerance of 0.013, Put to gether it comes to 0.033.

Please share your thought, Kindly let know if i am missing something.

 

[Burunduk]

No issue with the drawing.
Flatness and parallelism, each one separately shouldn't be greater than the size tolerance, when rule #1 applies, beacuse rule #1 will limit the variation each of them controls to the amount of the size tolerance.
Do not add them. The sum of them doesn't provide you any useful information.

 

[Babups]

okie,

In the Worst case scenario : If my actual part comes with flatness by 0.02 and parallelism by 0.013, In that case it makes my cross section (W +0 /-0.025) to go below the stated spec, It makes the part to be rejected right?

can you share your thoughts?

 

[Burunduk]

Not necessarily.
Let's look at an example:
For simplicity assume that the allowed parallelism in your drawing was also within 0.02 rather than 0.013.

Flatness on the left surface in your drawing within 0.02 means the surface needs to be between two planes 0.02 apart.
Imagine it was produced concave within 0.02.

Parallelism within 0.02 on the right surface in your drawing means it needs to be between 2 parallel planes 0.02 apart that are parallel to datum A (the tangent plane that touches the high points of the left surface). Imagine it was produced convex within 0.02 - this is allowed by the parallelism tolerance zone.

Would you say that in this condition the size must be non-conforming? Well, that is not true.
The "actual local size" could be well within tolerance between every two opposing points on the two surfaces.


This image shows what actual local size means in a feature that has a similar shape as I described.

 

[CheckerHater]

We forgot to ask the ultimate question: ASME or ISO?

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[Burunduk]

I assumed ASME because the OP mentioned Rule #1 (and there is no circled E so it's probably not ISO's Envelope principal that he considers).

 

[powerhound]

Since he said "to go below the stated spec" he's assuming both surfaces are concave, in which case that would result in a rejected part.

John Acosta, GDTP Senior Level
Manufacturing Engineering Tech

 

[Babups]

Sorry for the delayed response,

1. It's as per ASME

2. If the both are produced with the concavity, then it will result in non conformance to spec limit.

In this case, How one should approach to correct the drawing ? Pls share your views

 

[Burunduk]

There is no need to correct the drawing. It is valid as is.
Even if the part's variation utilizes both geometric tolerances fully, you cannot predict if the part is rejected or not. Yes, it will be rejected if both are concave to the maximum allowance, but if one surface is produced concave and the other convex, that can be a good part. As long as the rule#1 envelope is not violated and all actual local sizes are within tolerance, it shouldn't be rejected.

If one of the geometric tolerances - parallelism or flatness, was greater than the size tolerance, then some of that geometric tolerance would become redundant as the variation is already controlled to the amount of the size tolerance by rule #1. That is when the drawing would need correction.