Circularity tolerance (out of round condition)

[bryjarmoc]

If there is not a "circularity" requirement on the the drawing then is there an "assumed" circularity tolerance on any given diameter. I.E. a percentage of the nominal size?

 

[KENAT]

The entire surface has to fall between the upper and lower diameter tolerance.

So if your tolerance on diameter is +-.001 you have reasonable circularity.

If +- .010 not so good.

Nothing based on % as far as I know.

KENAT, probably the least qualified checker you'll ever meet...

 

[dingy2]

I agree with Kinat that the entire feature must not fall outside the tolerance zone. Again, this is differences in diameter and not circularity which is a surface condition.

There is no assume percentage for circularity.


Dave D.

http://www.qmsi.ca

 

[Standing]

With the Y14.5M-1994 note on a drawing the part must be perfect form at MMC.

Bradley
SolidWorks Premim 2007 x64 SP4.0
PDM Works, Dell XPS Intel(R) Pentium(R) D CPU
3.00 GHz, 5 GB RAM, Virtual memory 12577 MB, nVidia 3400

 

[ctopher]

If nothing is noted on the dwg, the machinst can do as he/she pleases, but machine it round as the dwg indicates.

Chris
SolidWorks 07 4.0/PDMWorks 07
AutoCAD 06
ctopher's home (updated 04-21-07)

 

[axym]

Further to Bradley's reply, perfect form is required at MMC. This is a consequence of Rule #1 (otherwise known as the Envelope Rule) in which a size tolerance requires that the feature not violate an imaginary boundary of perfect form at MMC. For example, if a hole has a size tolerance of 1.000 +/- .010, its surface must not violate a perfect cylinder of diameter .990 (represented by a .990 gage pin being able to pass completely through). Thus if the hole's cross-sectional diameter is .990, its form characteristics (circularity, surface line straightness, derived median straightness, cylindricity) must be perfect in order for the gage pin to pass through. If the hole's cross-sectional diameter is larger than .990 (say .995), its form characteristics can be out by as much as .005. At the LMC diameter of 1.010, the form characteristics can be out by as much as .020 (the size tolerance).

Back to the original question, a diameter tolerance gives an equal control over circularity. A diameter tolerance of +/- .010 would limit the circularity error to .020 at worst. There is no assumed relationship between circularity and the nominal diameter.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

 

[drawoh]

bryjarmoc,

A +/- tolerance on a diameter creates limits which must contain whatever form gets fabricated. If the diameter is 50+/-0.1mm, the as-fabricated form must be contained within two concentric circles of 49.9mm and 50.1mm. You also need a location tolerance to set the position of the centre of the round feature.

See ASME Y14.5M-1994, section 2.7.1. This is Rule #1, as noted above.

JHG

 

[ALOBrazil]

Further to Drawoh's reply, the circularity error is the radial distance between two concentric circles. That takes to a interesting fact: if your part was fabricated with an oval shape, then the maximum circularity error is half of the diameter tolerance !!!

For another shapes is possible a circularity error until the diameter tolerance, as explained in the following link:

http://www.tec-ease.com/tips/november-04.htm

Ademir

 

[bryjarmoc]

Thank you for everyone's input. I assumed there was not a circular requirement (if not called out). Our inspection department will measure a diameter and even though the min/max of the circle size is with in the diameter tolerance they will state there is a "out of round condition". Before I voiced my opinion, I wanted to ensure I was not missing something.

Thanks AGain.

 

[powerhound]

I'm curious as to why your inspection department would state an out of round condition on an inspection report if circularity is not even specified. If the diameter of a feature of size is 1.000 +/-.005 then the diameter can vary from .995 to 1.005 and be good. If the part does in fact vary that much, so what? What is the purpose of going out of the way to state that the part is out of round when it isn't specified on the print? What if the part measured 1.000 to 1.0001; would they state that it was out of round then? According to their policy, they should. What is the threshold before they decide that something is either round or out of round?

Powerhound
Production Supervisor
Inventor 2008
Mastercam X2
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II