FYI, I've seen, on more than several occasions, users here insisting upon
(typical). However, there are relatively few applications where that insistence bears fruit. For almost all commercial designs,
(typical) is more than sufficient. It is, well... typical!
Don't worry about stitching the planes (at AC, i.e. by placing bypass caps (with vias) near signal vias): the fact that they are wide area and closely coupled has already solved this for you. A few bypasses scattered about will do the job; most likely you already have enough from local bypasses at chips.
If you need more routing area, there's always the option of a six-layer board. You can use the same VCC/GND (on Mid1 and Mid4 this time) and add two extra routing layers, or add planes if you prefer. (Or route within planes, assuming you have area for stitching vias.)
This general scheme (reserving about half of all layers as plane layers, while respecting symmetry*) applies to any number of layers, so you'll see PC motherboards made with, say, 8 layers, or server backplanes and other specialized stuff made with, heck, 32 or more layers, with about every other layer being a plane.
*Notice you can't** have three planes on a six-layer board while placing them symmetrically. Boards are laminated in layer or core pairs, so you want to use symmetrical dielectric and copper layers. So, you'd go for two or four planes in a six-layer board, as the preferred build.
**Well, shouldn't, really. Unbalanced copper density may lead to warpage (uneven shrinking as the freshly-bonded PCB cools to room temperature), making mechanical problems as well as poor soldering on dense SMT components. This mostly manifests over large boards (300mm+?), and egregious density mismatches (nearly empty layers vs. solid planes), I think? As long as you're making modest use of all layers, and the board isn't massive, don't worry about it, really.
When you need extraordinary performance (tight regulations say for mil/aerospace?), it may be worthwhile to sacrifice ease of layout, manufacture and debugging for a more internal-based design (outer pours plus many GND planes, routing power, or plane-ing power on additional layers as needed). Even so, it may happen that not enough advantage is had by such layout practices (e.g. RF that needs 80dB+ shielding, whereas the layout tricks might afford, say, 10-30dB?), and a shield can is required; or the shield can turns out cheaper anyway versus the extra board layers. At this point, it's merely options in the toolbox -- try them (project budget and time permitting, as always!) and see what works best.