I'm routing diffpairs on the 1st inner layer of a 4-layer pcb which are Z-matched to the 2nd inner layer which is entirely a ground pour. The top layer has traces and routing AND also a ground pour around the components/routing. Should I cut away the ground pour above the differential pairs ? This is my stackup:
If you need them to remain Z-matched, then yes. The spacing to their ground is 0.71mm, from your layup table. The spacing to their inadvertent top ground is only 0.018mm, which will dominate the impedance many-fold, and bring the impedance down to a very low value.
With a ground plane spacing of only 0.018mm, you won't have the accuracy on any practical board process to reduce the track width to keep them matched.
Do you need to keep them Z-matched? It depends on the length, and the operating frequency, and whether you can tolerate what would look like some extra shunt capacitance.
Note that if you remove the top pour above them, and the PCB fab puts some copper thieving in that area, the fact that the tracks are differential means that even isolated spots of copper will reduce the impedance. However spots will reduce the impedance less than a solid plane would. If the impedance is really critical, you need to document a total copper keepout to your PCB fab.
Do those tracks go under anything else? Components? Tracks? They might as well be on the top if you can't use the space they go under. The relatively poorly controlled dielectric of the thin pre-preg layer will be dominated by the much thicker laminate underneath, so there will be insignificant loss of impedance control.
While foil outsides is a cheaper four-layer process than two laminates stuck together, I've always used the latter for any impedance controlled work, as it gives the opportunity for two layers rather than one to be controlled.