Partitioned pipe two phase | preCICE

This tutorial describes how to run a partitioned two-phse fluid simulation using preCICE.

Edit me

Note: Get the case files of this tutorial. Read how in the tutorials introduction.

Setup

This scenario consists of two pipes connected in series, both simulated with OpenFOAM’s interFoam solver. Fluids can enter from the left (here $z=0$) boundary of the Fluid1 participant with a uniform velocity profile ($u_{in} = 1 m/s$) and fixed flux pressure boundary coundition. The simulation begins with some water being present at the bottom left of the pipe. The volume fraction variable alpha is set to be 1 (water) at the bottom half of the inlet and 0 (air) at the top half. The water stream will approach the coupling interface at around $t=5s$ in the simulation. At the right boundary of Fluid2 there is a zero gradient boundary condition for velocity and alpha as well as a total pressure set to zero.

two-phase-setup

On the coupling interface, Fluid1 sends velocity, and alpha to Fluid2 and receives pressure, velocity gradient and alpha gradient. Fluid2 uses the fixedFluxExtrapolatedPressure boundary condition as shown in the partitioned pipe tutorial.

To make sure that preCICE works on the correct OpenFOAM fields, the field names are passed to the OpenFOAM adapter in fluid*/system/preciceDict:

FF
{
  nameP   p_rgh;
  nameAlpha alpha.water;
}

Note: This is a very basic example case demonstrating the coupling of a two-phase flow. To keep it as simple as possible, gravity is set to $0$ to avoid any kind of turbulences/vortices. Read more in the accompanying conference paper [1].

Configuration

preCICE configuration (image generated using the precice-config-visualizer):

preCICE configuration visualization

Available solvers

Both Fluid1 and Fluid2 are simulated with OpenFOAM (interFoam). An incompressible multiphase solver for two immiscible fluids using the Volume-of-fluid method. For more information, have a look at the OpenFOAM adapter documentation.

Running the Simulation

Open two separate terminals and start the fluid1 and fluid2 participants by calling the respective run script. For example:

cd fluid1-openfoam
./run.sh

and

cd fluid2-openfoam
./run.sh

Post-processing

The OpenFOAM solvers generate a .foam file each. You can open this file in ParaView. You can see the water-air interface crossing the coupling interface at around $t=5.0s$.

result

Disclaimer: This offering is not approved or endorsed by OpenCFD Limited, producer and distributor of the OpenFOAM software via www.openfoam.com, and owner of the OPENFOAM® and OpenCFD® trade marks.

References

[1] M. Mühlhäußer, G. Chourdakis and B. Uekermann, Partitioned Flow Simulations with preCICE and OpenFOAM, in: COUPLED 2023. DOI: 10.23967/c.coupled.2023.014