NX Modeling tolerance (Preferences) and the extrude results of bodies

Modeling tolerance (Preferences) and the result during extrude

Workaround to use only tolerance value by turning OFF Optimize Curve option.

Example:

Section loop is open or closed is depending on the chaining tolerance.

For extrude feature, chaining tolerance is 0.95 times of distance tolerance.

Extrude(2) is created with below modeling preference setting.

So distance tolerance = 0.01mm.

Optimize Curve ON, distance tolerance factor = 5.

But since Optimize Curve toggle is ON, and optimize factor for distance tolerance is 5.

So distance tolerance after applying optimize factor = 0.05 mm

Since chaining tolerance = 0.95* distance tolerance = 0.95 * 0.05 =  0.0475mm

For this case, if sketch expression value greater than 0.0475mm, section will be treated as open loop, otherwise closed loop.

If user wish to work with only distance tolerance (0.01 mm), user can turn OFF the optimize Curve toggle in Modeling tolerance or modify the optimize factor for distance tolerance as per requirement.

If user turn OFF the Optimize Curve toggle OFF, then distance tolerance = 0.01mm

Then chaining tolerance would be = 0.95 * 0.01 = 0.0095mm.

In this case, if sketch expression value greater than 0.0095mm, section will be treated as open loop, otherwise closed loop.

And for sketch expression values 0.04 and 0.05, extrude will create sheet body which is expected by user.

With above justifications the selection intent is working as designed. 

Workaround is: Use only tolerance value by turning OFF Optimize Curve option.