Add Tutorial: Partitioned multiphase pipe flow (#418)

Co-authored-by: Gerasimos Chourdakis <[email protected]>

partitioned-pipe-two-phase/README.md

@@ -0,0 +1,73 @@
+---
+title: Partitioned pipe two phase
+permalink: tutorials-partitioned-pipe-two-phase.html
+keywords: tutorial, FF, fluid-fluid coupling, OpenFOAM, interFoam, multiphase
+summary: This tutorial describes how to run a partitioned two-phse fluid simulation using preCICE.
+---
+
+{% note %}
+Get the [case files of this tutorial](https://github.com/precice/tutorials/tree/master/partitioned-pipe-two-phase). Read how in the [tutorials introduction](https://www.precice.org/tutorials.html).
+{% endnote %}
+
+{% note %}
+This tutorial relies on yet unreleased features of the OpenFOAM adapter. You need [preCICE v2](https://github.com/precice/precice/releases)) and [the ff-develop branch of the OpenFOAM adapter](https://github.com/precice/openfoam-adapter/tree/ff-develop) to run this tutorial.
+{% endnote %}
+
+## 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](images/tutorials-partitioned-pipe-two-phase-setup.png)
+
+On the coupling interface, Fluid1 sends velocity, and alpha to Fluid2 and receives pressure, velocity gradient and alpha gradient. Fluid2 uses the [fixedFluxExtrapolatedPressure](https://www.openfoam.com/documentation/guides/v2112/api/classFoam_1_1fixedFluxExtrapolatedPressureFvPatchScalarField.html) boundary condition as shown in the [partitioned pipe tutorial](https://precice.org/tutorials-partitioned-pipe.html).
+
+To make sure that preCICE works on the correct OpenFOAM fields, the field names are passed to the OpenFOAM adapter in `fluid*/system/preciceDict`:
+
+```CPP
+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].
+{% endnote %}
+
+## 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](https://www.precice.org/adapter-openfoam-overview.html).
+
+## Running the Simulation
+
+Open two separate terminals and start the fluid1 and fluid2 participants by calling the respective run script. For example:
+
+```bash
+cd fluid1-openfoam
+./run.sh
+```
+
+and
+
+```bash
+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](images/tutorials-partitioned-pipe-two-phase-result.png)
+
+{% 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.
+{% enddisclaimer %}
+
+## 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](https://doi.org/10.23967/c.coupled.2023.014)

partitioned-pipe-two-phase/clean-tutorial.sh

@@ -0,0 +1 @@
+../tools/clean-tutorial-base.sh

partitioned-pipe-two-phase/fluid1-openfoam/0.orig/U

@@ -0,0 +1,36 @@
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volVectorField;
+    object      U;
+}
+
+dimensions      [0 1 -1 0 0 0 0];
+
+internalField   uniform (0 0 1);
+
+boundaryField
+{
+    inlet
+    {
+        type            fixedValue;
+        value           uniform (0 0 1);
+    }
+
+    outlet
+    {
+        type            fixedGradient;
+        gradient        uniform (0 0 0);
+    }
+
+    fixedWalls
+    {
+        type            noSlip;
+    }
+
+    defaultFaces
+    {
+        type            empty;
+    }
+}

partitioned-pipe-two-phase/fluid1-openfoam/0.orig/alpha.water

@@ -0,0 +1,57 @@
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      alpha.water;
+}
+
+dimensions      [0 0 0 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    inlet
+    {
+        type            codedFixedValue;
+        value           uniform 1;
+
+        // Name of generated boundary condition
+        name    halvedFixedValue;
+
+        // Split the inlet in half water / half air across the y-axis.
+        code
+        #{
+            const vectorField &faceCenters = this->patch().Cf();
+            scalarField &alphaIn = *this;
+            forAll(faceCenters, faceID)
+            {
+                if (faceCenters[faceID].y() < 0.0)
+                {
+                    alphaIn[faceID] = 1.0;
+                }
+                else
+                {
+                    alphaIn[faceID] = 0.0;
+                }
+            }
+        #};
+    }
+
+    outlet
+    {
+        type            fixedGradient;
+        gradient        uniform 0;
+    }
+
+    fixedWalls
+    {
+        type            zeroGradient;
+    }
+
+    defaultFaces
+    {
+        type            empty;
+    }
+}

partitioned-pipe-two-phase/fluid1-openfoam/0.orig/p_rgh

@@ -0,0 +1,37 @@
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       volScalarField;
+    object      p_rgh;
+}
+
+dimensions      [1 -1 -2 0 0 0 0];
+
+internalField   uniform 0;
+
+boundaryField
+{
+    inlet
+    {
+        type            fixedFluxPressure;
+        value           uniform 0;
+    }
+
+    outlet
+    {
+        type            fixedValue;
+        value           uniform 0;
+    }
+
+    fixedWalls
+    {
+        type            fixedFluxPressure;
+        value           uniform 0;
+    }
+
+    defaultFaces
+    {
+        type            empty;
+    }
+}

partitioned-pipe-two-phase/fluid1-openfoam/clean.sh

@@ -0,0 +1,7 @@
+#!/bin/sh
+set -e -u
+
+. ../../tools/cleaning-tools.sh
+
+clean_openfoam .
+rm -rf ./0/

partitioned-pipe-two-phase/fluid1-openfoam/constant/g

@@ -0,0 +1,10 @@
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       uniformDimensionedVectorField;
+    object      g;
+}
+
+dimensions      [0 1 -2 0 0 0 0];
+value           (0 0 0);

partitioned-pipe-two-phase/fluid1-openfoam/constant/transportProperties

@@ -0,0 +1,25 @@
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      transportProperties;
+}
+
+phases          (water air);
+
+water
+{
+    transportModel  Newtonian;
+    nu              1e-06;
+    rho             1000;
+}
+
+air
+{
+    transportModel  Newtonian;
+    nu              1.48e-05;
+    rho             1;
+}
+
+sigma            0.07;

partitioned-pipe-two-phase/fluid1-openfoam/constant/turbulenceProperties

@@ -0,0 +1,9 @@
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    object      turbulenceProperties;
+}
+
+simulationType  laminar;

partitioned-pipe-two-phase/fluid1-openfoam/run.sh

@@ -0,0 +1,10 @@
+#!/bin/sh
+set -e -u
+
+blockMesh
+cp -r 0.orig 0
+setFields
+touch fluid1.foam
+
+../../tools/run-openfoam.sh "$@"
+. ../../tools/openfoam-remove-empty-dirs.sh && openfoam_remove_empty_dirs

partitioned-pipe-two-phase/fluid1-openfoam/system/blockMeshDict

@@ -0,0 +1,77 @@
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "constant/polyMesh";
+    object      blockMeshDict;
+}
+
+scale 1;
+
+
+zmin   0;
+zmax  10;
+
+xcells 1; // per block (5 blocks)
+ycells 10; // per block (5 blocks)
+zcells 20;
+
+vertices
+(
+    (0.0 -2.0 $zmin) // 0
+    (0.0 2.0  $zmin) // 1
+    (0.0 -2.0 $zmax) // 2
+    (0.0 2.0 $zmax)// 3
+    (-1.0 -2.0 $zmin) // 4
+    (-1.0 2.0 $zmin) // 5
+    (-1.0 -2.0 $zmax) // 6
+    (-1.0 2.0 $zmax) // 7
+);
+
+blocks
+(
+hex (4 0 1 5 6 2 3 7) pipe ($xcells $ycells $zcells)  edgeGrading (1 1 1 1 1 1 1 1 1 1 1 1)
+);
+
+edges
+(
+);
+
+
+patches
+(
+
+    patch fixedWalls
+    (
+        (0 4 6 2)
+        (1 3 7 5)
+    )
+
+    patch inlet
+    (
+        (0 1 5 4)
+    )
+
+    patch outlet
+    (
+        (3 2 6 7)
+    )
+);
+
+boundaries
+(
+    emptyWalls
+    {
+        type    empty;
+        faces
+        (
+            (0 2 3 1)
+            (4 5 7 6)            
+        )
+    }   
+);
+
+mergePatchPairs
+(
+);