Model accuracy

I switched from relative accuracy to absolute accuracy of .0001" back in '96 when I was new to Pro/ENGINEER (as it was called then) and had issues with small features on the end of a long wire failing on me.  I'd start out with the metric equivalent of that.  You'll find that sometimes for really tough geometry, that going to a tighter accuracy might make your latest feature work but causes some OTHER features to fail.  It's a balancing act sometimes, where you get some weird number that makes all your features happy.  Sometimes ya just gotta play with it.

I switched to absolute accuracy of 0.00001 a long time ago, predominantly because the default relative accuracy was causing me problems with machining operations (strange motions at surface-to-surface boundaries, etc.) It's a strange setting that can cause or fix regeneration issues depending on the combination of small/large features in models. The bad part is if I bring in an old model from the "before time" or something from a supplier or incautious colleague, often if I change the accuracy from relative to absolute it causes features to fail. Particularly if the model is based upon surface geometry provided by a customer.

For new stuff, if I keep the accuracy value nice and small, I find that my models are really stable and robust. That's probably due to the basis of the models being more accurate, and also 'cause I'm always looking for the troublemakers before they can cause problems (i.e. why have two surfaces defining a contour when I can get the customer to provide a single one that spans my part).

Ditto on Frank's explanation of finding the "Goldilocks" accuracy. I've had old models that needed to be tweaked to just the right value so everything works. Like 0.00001 doesn't work, but 0.00005 does, etc.

If you are using Creo models to bring geometry into your tool design then it is suggested by PTC that you match the accuracy of your tool design to that of the reference model. However since most users do not use absolute accuracy appropriately this may or may not be the best option.

In an ideal situation you will talk with the part designer to agree on an absolute accuracy setting that works for everyone before they design the parts. I always advise that the accuracy setting should be one order of magnitude smaller than the tightest tolerance that would be specified on a finished part. So if you have a +-0.1 mm tol then use 0.01mm absolute accuracy.

Starting with Creo 7.0, Creo Parametric uses absolute accuracy instead of relative accuracy. The default accuracy values are 0.00039 inches and .01 millimeters.