It is certainly OK to use positive planes instead of negative planes to get the result you are looking for. Negative planes are driven using the anti-pad definition inside of your Via padstacks while positive planes clearances are driven the DRC Clearance to the copper pad by default but you have the option to use the anti-pad to drive positive planes as well.
It most but not all cases the fabrication vendor would like a larger clearance on plane layers to prevent possible plane shorts. This could occur on planes where you have a large mass of copper that tends to shift during processing and also on plated thru hole location which need to be drilled larger to meet the hole size requirements once the holes are plated. I would confirm with the fabrication vendors that you use on what minimum clearance (anti-pad) is required on plane layers and adjust the anti-pad in you padstacks and/or the DRC Clearance to shapes accordingly to avoid any fabrication issues.
You could use positive planes and then add traces to connect all the islands, which would take a lot of your time, but as I said previously it may be in your best interest to consult with your fabrication vendor that your company uses in the hopes that they are OK with reducing the clearance so copper planes can flow the BGA pin fields without being broken up.
Here is a couple images of a small BGA with a slightly modified pin escape to allow the planes to flow to the inner power and ground vias. This can also be a solution to your plane break-up problem you are seeing. It is best to plan ahead during the beginning stages in the design on how you are going to get multiple powers planes connected up. I highlighted GND green and the 4 Powers different colors to illustrate what I have done.
Originally posted in cdnusers.org by mcatramb91