An extruded feature could not go for circular pattern. Can anyone help?

Two things to try:

1. Redefine the extruded vane feature to be 'up to surface' (of the cone) and uncheck 'merge result'. This should leave the vane as a separate body. Then 'circular pattern' the vane body (not in the feature box, the box below called 'bodies') by itself. This should leave you with 24 vane 'bodies' and the conical base. Finally, fuse all of the bodies together with the 'combine' feature using the 'add' option.

If that doesn't work, the problem is probably where the tip of the vane touches the edge of the cone. Then I would try this:

2. Extend the ends of the cone (probably with 'move face' feature) so the same sized vane falls more thoroughly on the conical surface BEFORE creating and patterning the extruded vane feature and then trim or move face the cone edges back to the desired location, OR make the vane slightly smaller than the cone so it achieves the same condition, the vane connects fully inside the cone edges, not right on them.

If neither of these works then the problem is something else. I'd try it myself but your part is 'future version' to me. Ugh. It's happening more and more. I guess that means I need to update us again.

Not a SW man but here goes

It works fine for me (image attached).
It could be an issue that was fixed in a service pack.

I can't say this part is made in a wrong way, but it has been made in a rather odd way.
If you don't feel like remodeling the part, you can try this:
Edit Boss-Extrude1.
Enable the 2nd direction.
Set the values to Blind, and 1mm

This will help embed the vane into the body. Extruding a 3D sketch off of a conical surface is a perfect recipe for a tangent contact which is most likely giving the zero thickness error.

I did not need an analysis of your procedure to see at first glance that it was a very bad idea to merge your extrusion to repeat. I rarely have success when doing a circular repetition of functions. It is better to repeat bodies and then weld them. Here I started by doing an extrusion in a second direction to make sure that it will go beyond the face. I created an axis with the central segment and then repeated the body. Better to create a leave in the tips before the leave of the top, a shape in tip does NEVER give good results. Then he will comb the bodies but starting with only 1 with the base then in 2 other combinations I managed to combine everything. I even checked if I could leave at the base of the forms and there is also better to practice holidays on the edges in two or three times.
File is SW2018