Is it always possible to reduce the number of layers on a PCB by making the board larger
Ah the horror of trying to make DDR work in two layers :)  The long answer is of course to learn about signal integrity and try to understand exactly what you are doing.  I have seen this done before, and even pass EMI but with many caveats.  First there was only a single DDR part. Second the controller was carefully designed to route out onto all signals in the first two rows of widely spaced balls such that all signals routed with no vias on the top layer to the DDR part.  Then the bottom was used for a GND plane, even though it was 60 mils away.  Routes were matched, but kept "extremely" short.  Finally the part was run as slow as possible, basically the minimum frequency allowed by the DDR part.  Oh and we had a spread spectrum clock for EMI.

I would say as a general rule that this is not a good idea and you should stick to four layers and cut cost elsewhere.  If you are going to do it don't even expect to get to near full speed, and if you're trying to route multiple parts like a DIMM or clamshell.  I would say it's not even worth trying.

Cost depends on so many factors from where you're doing it to how much, it's a much smaller issue at very high volumes than it is at low proto volumes.  The headaches you will face trying to debug a two layer design are almost surely never worth it.  The increased time to market you will face trying to get it to work is alone worth the cost of a 4 layer in many cases.

You mention volume of 100 like it is high, but it is not at all once you start moving into the thousands, hundreds of thousands there's a steep drop in price from a few hundred pieces.  Same if you move off shore somewhere.  Just as an example I can think of my US price on 10K units of a 10 layer board is around $50, but my offshore of the same is $25.  Your price will also depend on how efficiently you use the panel ( your pcb house makes boards in standard sheet sizes.)  If you only fit two per panel and have a lot of waste your cost will go up just as if you only order 2 and leave room for 20 on the panel.  Incidentally that's how places that pool together pcb orders work.

Why does it cost more?  Well it's a lot ore work, involves double the material and requires a bit more precision or skill.  A two layer is just a piece of FR4 copper clad on both sides, just drill some holes, mask, etch away and post process.  For a four layer board mask and etch the two layer, then laminate two more outer layers on either side mask and etch again being very careful that they line up properly, then drill and post process.  That's just an example but the point is the process has more steps, more labor, more material and more cost.

It might be worth mentioning that there are chips for the mobile industry that take things like LPDDR4 mounted directly on top of them for an all in one solution.  Still I would want a four layer board for proper power distribution, decoupling, and routing of other signals but it's an interrsting angle to consider.