Geometric Tolerance

[BlueChip]

Anyone have a good explanation for the term "true position" ... looking for a good & simple way to explain it. Thanks.

[HuFlungDung]

Hi Bluechip,

Are you referring to servo positioning?

[Paul_S]

True position tolerancing is used to help guarantee interchangeability between machined or manufactured components. It typically consists of a retangular block with a square block on the left with its geometric control symbol which is a "+" with a smaller circle at its center. This geometric control symbol designating True Position. To the right is a reganguar block with the an absolute tolerance value. And to the right of the tolerance value is a tolerance modifer, a "S," "M," or a "L" in
a circle. The "S" means the tolerance applies regardless of the part feature size. The "M" means the tolerance applies at maxium material condition. For example, it the feature is a .312
hole with a tolerance of -.001 +.004, the position tolerance applies to the maxium material condtion of the diameter at .311. So if the tolerance is, let's say, .002 at maximum materal condition would be a bull eye of .002 in diameter that the center of the .311 hole can be located. But if the hole is .316 then the tolerance bull eye becomes .007 in diameter. So taking this example farther, if the hole is .312 and out side the .003 bull eye for its location by, let's say, .002. If the hole is opened up to the maxium of .316, it is no longer out of tolerance. It would then just be in tolerance of .007 true position.

The dimension blocks are box values with have an absolute value and no tolerance at all. These are called Basic Dimensions. The True Position block is the tolerance block.

Regarding the "L" in the circle "Least Material" condition. Where the tolerance applies to the large hole or smaller shaft, for example. And it is not as commonly used. But it is used.

There are a number of books which will cover this. Y14.5 is the standard which governs True Position, along with all the other standard geometric dimensioning. Y14.5 is the ANSI standard. There is also an ISO standard.

I hope this is of some help.

[BlueChip]

Thanks Paul ... it was a thing of beauty.

[CAMmando]

Just a couple od additional points to add to Pauls excellent reply.

99% of the time true position is given for round features with the Ø symbol preceding the tolerance. This means that the tolerance zone (the area that the centerline of the feature may legally be located) is circular.

This is a natural and inherently good way to define the tolerance zone for round features that must fit together. The old bilateral X/Y location tolerance method resulted in a rectangular tolerance zone. This does not really lend itself to round features.

You can use a worse case scenario conversion to get an “equivalent” plus/minus X/Y location tolerance. If you picture a square tolerance zone inscribed inside of the round tolerance zone, you will see that the corner of the square would be given by:

d/2*sin45°

So in the worst case scenario, a true position tolerance of Ø.010 RFS would be “equivalent” to ±.0035 in the X and Y axis.

[timf]

i took a class once and we designed gages to check parts that were various geometerical tolerances and conditions and it was all so clear after that class.
all that was started above is right and very well explained but it never really sunk in for me till we made the fixtures that that checked the parts for maximum defect but still functional.

[E-Stop]

An additional comment on CAMmando's reply. The .0035 tolerance in the X an Y is correct at it's maximum for both axis. But as one axis is closer to nominal the other axis is given more tolerance. So in the drawing shown, if the X axis is dead nuts, the Y axis can be out .005

[timf]

i was also once told to take the box number and divide by 3 then use that as my max tolerance for both axis.

.010 true position /3= +/-.0033 in x and y

it seems to always be safe for basic positional tolerancing and it was the easiest way to understand when first starting to deal with it.
this method cheats you out of the extra tolerance so your part is not scrap if you miss the target, depending on the other axis.
the closer it is the more bonus you get on the other as stated by E-stop.

[CAMmando]

Thats pretty close.

You can also multiply the radius by .707

.005*.707=.0035

[E-Stop]

My rule of thumb is to multiply the true position tolerance by .3535 to get the X,Y tolerance zone.

.025 TP * .3535 = .0088 X & Y tolerance

And as mentioned before, the closer one axis is to nominal the more the other axis can be out.