The reason as to why the incompressible simulation is so fast is because it is a steady state simulation (SS). SS simulations are always orders of magnitude computationally cheaper to run compared to the multi-phase simulation which is currently set to transient.
SS simulations do not require the actual progression of “time” per say. They just solve for the solution that is inherently within the domain (aka the meshed geometry) hence its a matter of how many mathematical iterations to get to the final solution that is most accurate. There is no need to resolve many solutions to get to the final one for SS simulations in a sense.
Compare this to transient simulations where time does exist and the solution has to progressively be solved through per timestep for the total time, you can see why this is so much more inherently time consuming as the solution always changes every timestep and has to be constantly solved again and again till the end time is reached. Considering that also that information cannot travel faster than the flow per say, you have to maintain solution continuity by ensuring as such. This brings in the consideration of courant number and again contributes to the further computational costs of transient simulations.\
So for starters, there is really nothing wrong with your simulation. It is the nature of transient simulations to take this long and to be costly. For context, a 2D simulation with 2mil nodes (similar to yours) transient laminar one that I did takes about 8-10 hours to complete for a end time of 0.25s and a maximum courant of 0.7.
That being said, you need to adjust your simulation control. Currently your end time is set to 0.5s which can be further optimized as you dont want to run the simulation for longer that it needs to as it is a waste of computational resources. You need to roughly calculate how long it takes for the flow at the furthest end to reach the end of the pipe. For example if your flow travels at 1m/s for a pipe that is 1m long then your end time should be 1s. Though you will probably need to add some factor of safety into it and give say 10% more the solution to reach a pseudo “steady-state” where the solution does not deviate too much and can give you reliable results to extract out.
You can also set the Maximal CO to 1 and that should help in reducing your simulation time significantly. Your mesh has no errors and setup looks alright so do try it out and let us know. Oh and last thing, you might want to set some sort of result control to monitor the results within the geometry and maybe at the outlet so that you can tell if the simulation has reached this pseudo “steady-state”. The convergence plot is likely insufficient to give you a good tell.