[mortezahdr]

Hello all,
I am trying to simulate the air flow entering a tube shown in the following image. The tube has some small holes from which the flow exits, but since the flow field outside the tube is needed, computational domain is much larger than the tube and the outlet is located far from it. The tube boundary is called airbar and the boundaries not labled in the image are called walls.

The only numeric boundary condition I have is 70 psi at inlet (=482600 pa) and because of that, I am using rhoPimpleFoam, as it obviously is a compressible flow.
The problem is that the solution does not become stable and if I use a table to gradually increase the inlet pressure from environment (101325 pa) to 482600 pa, it helps stabilizing the solution, but it gets a very small time step of order of 10^-7 or 10^-8, which is useless.
Is there any solution (schemes/turbulence model for example) to increase the time step? Or do you think it is possible at all to solve a flow with such a large inlet pressure with OpenFOAMor not? I use LES turbulence model and the average y+ on the tube is around 1. Boundary conditions for U and p are shown below:

U:

boundaryField
{
inlet
{
type pressureDirectedInletVelocity;
phi phi;
rho rho;
inletDirection uniform (0 0 -1);
value uniform (0 0 -1);
}

outlet
{
type zeroGradient;
}

airbar
{
type noSlip;
}

walls
{
type noSlip;
}

}

p:
dimensions [1 -1 -2 0 0 0 0];

internalField uniform 101325;

boundaryField
{
inlet
{
type uniformTotalPressure;
p0 tableFile;
file "data_p";
gamma 1.4;
}

outlet
{
type fixedValue;
value uniform 101325;
}

airbar
{
type zeroGradient;
}

walls
{
type zeroGradient;
}
}

[Alczem]

Hey,


Can you do a steady state simulation with rhoSimpleFoam? It will be faster to achieve a final state. And you could use this to initialize a transient simulation with an already developped flow.


Otherwise, if the steadystate solver is unstable, you might want to give Local Time Stepping a try, by using a ddt scheme like localEuler or SLTS.


If you need a full transient simulation, I don't think you have a choice about the small timesteps are you sure your velocities are correct? You could also do a steady state simulation of the interior of the tube and use this solution to do a transient simulation of the exterior.


Can you coarsen your mesh somehow? It will increase the timestep. Can you share a picture of your mesh near the holes?



Lats thing, you might achieve a larger timestep using PIMPLE and several outer iterations to use a larger Courant number.