cut too small to show 2

[PROCON]

I need to make a cut for a vent of .0005 deep but pro-e will not show the cut less than .0012. Can the settings be changed to allow this to show up.

 

[Hora]

Change the part accuracy from .0012 (default) to a smaller value (.0001). In 2001 is under SETUP menu. Should be similar for Wildfire.

-Hora

 

[texaspete]

Can anyone tell me which is better. Would "absolute tolerance" or "relative tolerance" be better. If Absolute tells the cad operater that the smallest feature or edge is .0012 (default). Is this true? I design sheetmetal office furniture and by default the OEM start model is .0012 relative tolerance. When the part is 6 ft tall and the thickness of the part is 18 gauge - some times very small features (say a punch has small radii), Pro/E will complain or warn of small geometry.
Which is better "absolute or relative" tolerance.
Texaspete

 

[TheTick]

Relative tolerance automatically adjusts the size of the modeling tolerance with respect to the size of features in the model. Absolute tolerance forces the modeling "engine" to apply the same tolerance to all features, regardless of feature size.

The benefit of relative to;erance is that it doesn't force the modeling engine to highly refine edges defined by faces that are very large. This would take up more memory.

The downside is sometimes relative tolerance seems to miscalculate what tolerance is necessary to generate the solid model. I have seen this problem on large parts that have small features (one example: a large plastic molded shell with a small reveal and tiny snap features). Switching to absolute accuracy can resolve the problem.

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