NX Extrude fails with "A solid body cannot be created from the section. The section may have gaps".

When you attempt to extrude a  sketch and receive an alert that "A solid body cannot be created from the section. The section may have gaps", then you end up getting sheet body, what do you have to do to resolve this problem?

One might think this is a sketch issue, but it is not since there are no gaps in the sketch.

The real problem in this case is that some of the curves in the sketch are very small (about 0.03 mm) while the chaining tolerance used by the section is 0.0475 when Optimize Curve is turned on and at the default tolerance factor of 5. So, in that case the small curves are found to be degenerate (zero-length).

Note: In this case when "Optimize Curve" is on, the chaining tolerance value 0.0475 is calculated internally and comes from 0.01 * 0.95 * 5, where 0.01 is the distance tolerance multiplied with 0.95, as the default chaining tolerance is 95% of the distance tolerance, and the 5 is the Optimize Curve Distance Tolerance Factor.

This kind of issue is made aware of in the documentation with a warning about using Optimize Curve with small edges here:

https://docs.sw.siemens.com/en-US/doc/209349590/PL20220512394070742.modeling/xid1318332?audience=external

The above linked documentation also has a recommendation below to resolve this issue:

Recommendations:

A general recommended workflow is to leave the Optimize Curve preference, set to on. If you encounter a tolerance issue with a feature, tighten the Distance Tolerance or the Angle Tolerance to address the specific occurrence.

Consider clearing the Optimize Curve  preference check box for extremely high precision cases, but try tightening distance and angle tolerances first.