Hello-

I am analyzing flow through a valve. The geometry is complex and 3-d. There are three different ways i have been trying to simulate it:

1) Mass flow at inlet and outlet = 0.2 kg/s. In this case, the solution converges in 1 iteration without even showing the error residuals. Is it believable?

2) Mass flow at inlet = 0.2 kg/s and outlet= 0 bar static pressure. Again, the solution converges in 1 iteration saying that error residuals are below the target values.

3) pressure inlet and pressure outlet BC. The solution converges in about 100 iteration, which i think is normal.

What do you think of the first two cases? Applying mass flow at inlet and outlet, is it reasonable? Also, mass flow at inlet and pressure at outlet, is that reasonable approach?

Thanks in advance,

CFDLife

Also, when i use the mass flow rate obtained from case(3) to simulate the valve as in case (1) and (2), i do not get the same pressure differential as (3). So, am assuming that (1) and (2) are not the right approaches. Anyone experienced this before?

Are you looking at compressible or incompressible flow? How many elements does your mesh contain? What target residual did you set?

Case 1. Imposing mass flow on both inlet and outlet is not valid; either the inlet or the outlet condition is redundant, because it does not pose an additional constraint necessary to solve the system.

Case 2. Valid, but what reference pressure did you set? Your reference pressure should be larger than 0 [bar] if you set the boundary condition at 0 [bar].

Case 3. Not a good combination. Puts a weak constraint on the system. Moreover, convergence in 100 timesteps sounds a bit suspicious for a complex 3d geometry.

In general you want to give the system some information about velocity and some information about static pressure, without under- or overconstraining it. A combination of mass flow inlet (velocity info) and static pressure outlet or a combination of total pressure (static pressure and velocity) inlet and static pressure outlet generally work. Besides that it is important to choose your boundary conditions according to the physics.

Thanks Timon

In case (3), I provide a pressure differential across inlet and outlet, say 100 bar at inlet and 0 bar at outlet, why is it a bad combination?? The solution that i obtain seems reasonable (it takes anywhere between 100-1000 iterations depending on the changes in the geometry).

In all the cases that i mentioned, i have used the default reference pressure, which is 1 atm.

What do you think?

Forgot to mention that in case (2), i am using total pressure inlet (100 bar) and static pressure outlet (0 bar).

When you impose static pressure on both inlet and outlet, both total pressure and mass flow are an implicit result of your simulation. The constraints you put on your system are too weak. Look at it this way: if you merely specify the static pressure in your domain, how can the solver determine the kinetic energy of the fluid?