NX Revolve produced incorrect surface type due to Optimize Curve preference

The sketch has two sketch curves that are lines; these lines are nearly parallel to each other (they're 2 degrees apart).

Concern#1:
Using the default Revolve tolerance of 0.01mm, the Revolve feature creates only one face from these two sketch lines.
Solution: Change the Revolve tolerance to 0.001mm, this will allow 2 faces to be created from revolve feature.

Concern#2:
Although two faces were created from revolve feature as expected, these two faces are of type "Revolve" instead of "Conical". This can cause issue when data is processed down to Drafting views, as drafting will show them as spline instead of line, thus unable to dimension between splines.

Revolve surface type - spline type in Drafting (no good)
Conical surface type - line type in Drafting (good)

What is the solution to Concern#2?

The problem where Revolve produces incorrect surface\edge types can be due to a Modeling Preferences option called "Optimize Curve" (Menu->Preferences->Modeling->General->Optimize Curve).

When 'Optimize Curve" is ON and with an Angle Factor of 5. Combine this with the 0.5 angle tolerance also in Modeling Preferences, NX will combine the two lines into a spline in an effort to optimize the part as the threshold is greater than the 2 degree difference between the lines.

If the line optimization is not desired, "Optimize Curve" can be turned OFF, OR the Angle Factor can be reduced below 5.