NX Extrude of a helical-face, resulted in a "Convergent Solid Body". Subtract resulted in additional Extract Body feature.

Extrude of a helical-surface (using Face Edges) created a body. This body was used in a boolean operation (like the tool to subtract from a Block (as target).
The problem raises with the Subtract feature: 
- The Extrude doesn't subtract form the block; 
- an Extracted Body is created automatically;
- These Alert messages may appear: 

Selected Body used a tool of Subtract<xxx>. It may result in failure of Subtract<xxx>.


The output will be a facet body because input is analytic as well as facet. An Extract Body feature will be created automatically from the analytic input.

Facet as well as analytic bodies are selected. Targets must be either analytic or facet.

Solution

This behavior is because the extrude of the helical-face resulted in a "Convergent Solid Body".

The solution is to create a "regular" solid body:
 

1. Go to Menu >> Preferences >> Modeling..  >> tab Convergent 
2. UN-set "Treat Degree 1 Spline as Polyline"
3. Then recreate the extrude of the helical Face. 

This will result in a Solid body and subtract works as expected.


Remark:
Since NX 1947 customer default can be set:
 'File --> Utilities --> Customer Defaults --> Modeling --> General --> Convergent --> Treat Degree 1 Spline as Polyline'. 
The default is toggled OFF.

Notes and References

https://support.sw.siemens.com/knowledge-base/PL8014702

Hardware/Software Configuration

Platform: INTL64
OS: windows
OS Version: 1064
Product: NX
Application: DESIGN
Version: V1847
Function: FEATURE_MODEL

Ref: 001-10202678