Best layer stack strategy for a 6 layer PCB with mostly SMD components
Just a few comments....


Lots of vias into the GND plane is not a problem.
Number of vias drilled into a board does not have a huge impact on production cost. If it does find a different board fab shop.
You need to make your stackup symmetrical in terms of copper density (as mentioned already in comments) to avoid board warp.
It is not a good idea generally to try to avoid vias through the use of GND pours on the surface layers. GND pours are great but the should be stitched to the GND plane probably more than if you did not have them. Keep in mind that, on a board of any density with SMT components, a surface GND pour will not be accessible to many of the GND connections anyway and you thus still need vias at all those points into the inner GND plane.
If you provide lots of PWR to GND plane decoupling capacitors the PWR plane can be a reasonable reference plane to use for AC impedance of controlled impedance routing. See next why this can be important.
If you need four signal layers with controlled impedance for routing a dense board then use layers 1, 3, 4 and 6 for routing and put PWR and GND on layers 2 and 5.
If signal routing impedance is not that critical in your design for most traces then do your routing on layers 1, 2, 5 and 6 with PWR and GND on layers 3 and 4. For the few traces where controlled impedance is most important consider placing them on the inner signal layers 2 and 5 where they can be closer to the PWR and GND reference planes.
GND pours on any layer, surface or otherwise, can be very useful if you have sensitive areas of circuitry that need to have their own GND area that is then joined to the main GND plane via a single point often through a ferrite bead component.