In theory oit should be easy with the pattern feature but from the simple example I tried it looks like Inv has a problem with following the tangency of the path when it goes around the ends.
You can also try an Emboss function. Make a sketch with your profile and Emboss this on your track.
Have also a look at the standard Inventor Belt Design tool. In a Synchronous Belt inventor uses a pattern similar to your track.
Even if you want to pattern it around, it will not fit curved surface. So maybe you should pattern only sketch, and then project sketch on surved surface, then extrude it. If i'll have time, i'll try to do it later today.
It doesnt need to fit the curved surface, just model them over sizes and then use a surface to trim down to the height needed.
I dont think you can use a sketch pattern as sketch pattern wont follow a curve, just a straight line - I think.
You might be able to model the belt profile in the sheet metal environment as a contour flange. Then use the Rip and Unfold commands to flatten it, sketch the tread patern, extrude it with the Face command, and Refold. The extruded face will stretch itself to follow the contour of the sheet metal part.
I made this simple track with the emboss feature. First created a sketch with a pattern of the profile, dimensions linked to the geometry of the basic track to match the right size. Then emboss the sketch first on the straight part, then reused the sketch and emboss this on the curved part of the track with wrap to face option on. Last step, circular pattern the 2 embosses to the other sides. Check the attached ipt (2012) to see how i did it.
An other option is to use the "Bend Part"option hidden under the Model Tab, section Modify. Create the Track as a flat with profile. Then place a sketch where you define the bend distances, and then 'Bend Part'. Make sure that you don't get interference by adjusting the sketch and pattern. See my ipt for more info.