The variation of velocity at inlet and outlet boundary
 

Hello everyone,

I simulated flow in pipe. Type of boundaries: velocity inlet, pressure outlet, unsteady flow, material: water
At time t=100s I increased velocity at inlet boundary, U1, from 5cm/s to 7cm/s. And immediately, at t=100s, I also saw velocity at outlet boundary U2=7cm/s. However, I expected this variation (U2=7cm/s) occur at outlet boundary after several seconds (example t=102s,etc..). If we have long pipe, the variation occur immediately at both inlet and outlet at same time, that does not make sense.
I would appreciate if anyone can tell how to setup for model working.

Thank you,

It is not totally unbelievable.

By the conservation of mass principle, the rate of mass leaving a control volume must be equal to the rate of mass entering the value +/- any unsteady storage term.

If you modeled the water as constant density fluid then you will not have the proper storage term (since density is fixed) and you will see an immediate rise in velocity at the outlet. Even if you had the right equation of state, water at typical conditions is highly incompressible and you will expect to see the velocity at the exit rise almost instantaneously.

The almost immediate increase in flowrate at the exit does not come free, it shows up as a pressure difference between inlet and exit. The time-scale that it takes for the water to react to the new boundary conditions (new velocity at the inlet) is proportional to the speed of sound (and not the convective time-scale, the velocity time-scale). So even for very long pipes, you can still see the velocity at the exit increase with an increase in inlet velocity almost immediately. The speed of sound in water is ~1400 m/s. This effect can be found in gas flows such as air, where the speed of sound is ~300 m/s. The speed at which these pressure waves propagate is much faster than your velocity time-scale which is merely a few cm/s.

In order for your modelling to predict the slow response, you would have to use an approach that is compatible with compressible flows and not incompressible flows. This means having the proper equation of state and possibly using the density based solver, although you could also do it with the pressure-based solver.