Here's a starting point - however you may have to do some surfacing rather than a solid. The point being to construct a "cutter" to cut away the shape of the teeth in some manner. This can be accomplished in a simple manner such as this or you can create surfaces and in place of the Subtract (included with the Extrude command) you would use Trim Body, making sure the surfaces extend through the solid completely.
Another approach would be to shorten the length of the Tube and rather than create a cutter, create a positive body to Unite with the top of the Tube to create the teeth.
Be careful adding Edge Blends to Patterns - Unsuppress Edge Blend(5) and watch the Pattern Feature fail miserably. You can get around this by modeling the Tube in a section and model a single tooth (or 2 half teeth) and one of the final steps being rather than use Pattern Feature or Pattern Face, use Instance Geometry.
IMO, the best thing you can do with copying something around in a circular manner if the part proves to be a bit complex - model a "pie section" of the part and use Instance Geometry with a final Unite at the end. This method removes any errors resulting from an Instance or Pattern misinterpreting which Edges to which they are supposed to be applied more often than not. I've had Pattern Face suggested as a workaround, but it too usually fails (with my examples, at least).
You will gain experience and be able to break things like this down quite easily the more you encounter them. I designed wheels for over 10 years and found myself frustrated more than once.
teeth_nx8.prt
Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB
