From 52e9651f45f0dac92033850d11547c3cf7a5159e Mon Sep 17 00:00:00 2001
From: DavidSCN <david.schneider@ipvs.uni-stuttgart.de>
Date: Thu, 11 Mar 2021 22:05:17 +0100
Subject: [PATCH 1/6] Add the flow-over-heated-plate for nearest-projection
---
.../README.md | 122 ++++++++++++++++++
.../clean.sh | 49 +++++++
.../fluid-openfoam/0.orig/T | 60 +++++++++
.../fluid-openfoam/0.orig/U | 55 ++++++++
.../fluid-openfoam/0.orig/alphat | 61 +++++++++
.../fluid-openfoam/0.orig/epsilon | 61 +++++++++
.../fluid-openfoam/0.orig/k | 61 +++++++++
.../fluid-openfoam/0.orig/nut | 61 +++++++++
.../fluid-openfoam/0.orig/p | 65 ++++++++++
.../fluid-openfoam/0.orig/p_rgh | 55 ++++++++
.../fluid-openfoam/constant/g | 22 ++++
.../constant/thermophysicalProperties | 49 +++++++
.../constant/turbulenceProperties | 26 ++++
.../fluid-openfoam/fluid-openfoam.foam | 0
.../fluid-openfoam/removeObsoleteFolders.sh | 22 ++++
.../fluid-openfoam/run.sh | 44 +++++++
.../fluid-openfoam/system/blockMeshDict | 121 +++++++++++++++++
.../fluid-openfoam/system/controlDict | 59 +++++++++
.../fluid-openfoam/system/decomposeParDict | 16 +++
.../fluid-openfoam/system/fvSchemes | 59 +++++++++
.../fluid-openfoam/system/fvSolution | 66 ++++++++++
.../fluid-openfoam/system/preciceDict | 51 ++++++++
.../precice-config.xml | 76 +++++++++++
.../solid-openfoam/0.orig/T | 47 +++++++
.../constant/transportProperties | 21 +++
.../solid-openfoam/removeObsoleteFolders.sh | 22 ++++
.../solid-openfoam/run.sh | 44 +++++++
.../solid-openfoam/solid-openfoam.foam | 0
.../solid-openfoam/system/blockMeshDict | 88 +++++++++++++
.../solid-openfoam/system/controlDict | 59 +++++++++
.../solid-openfoam/system/decomposeParDict | 16 +++
.../solid-openfoam/system/fvSchemes | 51 ++++++++
.../solid-openfoam/system/fvSolution | 35 +++++
.../solid-openfoam/system/preciceDict | 57 ++++++++
34 files changed, 1701 insertions(+)
create mode 100644 flow-over-heated-plate-nearest-projection/README.md
create mode 100755 flow-over-heated-plate-nearest-projection/clean.sh
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/T
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/U
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/alphat
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/epsilon
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/k
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/nut
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/p
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/p_rgh
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/g
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/thermophysicalProperties
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/turbulenceProperties
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/fluid-openfoam.foam
create mode 100755 flow-over-heated-plate-nearest-projection/fluid-openfoam/removeObsoleteFolders.sh
create mode 100755 flow-over-heated-plate-nearest-projection/fluid-openfoam/run.sh
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/system/blockMeshDict
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/system/controlDict
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/system/decomposeParDict
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/system/fvSchemes
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/system/fvSolution
create mode 100644 flow-over-heated-plate-nearest-projection/fluid-openfoam/system/preciceDict
create mode 100644 flow-over-heated-plate-nearest-projection/precice-config.xml
create mode 100644 flow-over-heated-plate-nearest-projection/solid-openfoam/0.orig/T
create mode 100644 flow-over-heated-plate-nearest-projection/solid-openfoam/constant/transportProperties
create mode 100755 flow-over-heated-plate-nearest-projection/solid-openfoam/removeObsoleteFolders.sh
create mode 100755 flow-over-heated-plate-nearest-projection/solid-openfoam/run.sh
create mode 100644 flow-over-heated-plate-nearest-projection/solid-openfoam/solid-openfoam.foam
create mode 100644 flow-over-heated-plate-nearest-projection/solid-openfoam/system/blockMeshDict
create mode 100644 flow-over-heated-plate-nearest-projection/solid-openfoam/system/controlDict
create mode 100644 flow-over-heated-plate-nearest-projection/solid-openfoam/system/decomposeParDict
create mode 100644 flow-over-heated-plate-nearest-projection/solid-openfoam/system/fvSchemes
create mode 100644 flow-over-heated-plate-nearest-projection/solid-openfoam/system/fvSolution
create mode 100644 flow-over-heated-plate-nearest-projection/solid-openfoam/system/preciceDict
diff --git a/flow-over-heated-plate-nearest-projection/README.md b/flow-over-heated-plate-nearest-projection/README.md
new file mode 100644
index 000000000..670c1c27b
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/README.md
@@ -0,0 +1,122 @@
+---
+title: Flow over heated plate nearest projection
+permalink: tutorials-flow-over-heated-plate-nearest-projection.html
+keywords: OpenFOAM, nearest-projection, CHT
+summary: This tutorial introduces an example simulation setup for nearest-projection mapping with the OpenFOAM adapter. The demonstrated "flow over a heated plate" scenario is exactly the same as in the `buoyantPimpleFoam-laplacianFoam` tutorial (with a thinner plate). The following text explains the _general functionality_ of the adapter, the _current capability_ of the adapter and the necessary _changes in the tutorials_ for your own simulation.
+---
+
+## Setup
+
+The setup is exactly the same as described in our [flow-over-heated-plate tutorial](tutorials-flow-over-heated-plate.html). Since the physical setup is not the main concern of this tutorial, we focus in the following on the nearest-projection mapping within preCICE. Let's start with general information about mapping methods. The [preCICE docs](configuration-mapping.html) contains an overview with available mapping methods in preCICE. The nearest-projection mapping is a second-order method. But, contrary to the RBF mapping, mesh connectivity information is needed for the interpolation.
+There are two participants in each mapping, but the connectivity of one mesh is sufficient for an interpolation. Which of the participants must provide mesh connectivity is not arbitrary and depends on the constraint type:
+
+- for `consistent` mappings, the `from` participant needs to provide connectivity
+- for `conservative` mappings, the `to` participant needs to provide connectivity
+
+For example, in our case, we exchange `Temperature` data in a `consistent` way from the `Fluid` to the `Solid` participant. Hence, `Fluid` needs to provide mesh connectivity.
+
+Notes:
+
+- In a standard **CHT** calculation, both data sets (heat flux and temperature) are mapped consistently. Therefore, both participants need to provide connectivity.
+- In a standard **FSI** calculation, forces are mapped conservatively from `Fluid` to `Solid`, while displacements are mapped consistently from `Solid` to `Fluid`. Hence, it is `Solid` that needs to provide connectivity and not `Fluid`.
+
+If mesh connectivity is not provided in the described way, you are nevertheless able to define a nearest-projection mapping in your `precice-config.xml`file, but it will _fall back to a first-order nearest-neighbor mapping_.
+
+## Available solvers
+
+Fluid participant:
+
+* OpenFOAM (buoyantPimpleFoam). For more information, have a look at the [OpenFOAM adapter documentation](adapter-openfoam-overview.html).
+
+Solid participant:
+
+* OpenFOAM (laplacianFoam). For more information, have a look at the [OpenFOAM adapter documentation](adapter-openfoam-overview.html).
+
+Since OpenFOAM is a finite-volume based solver, data is located in the middle of the cell, or on the cell face centers for a coupling interface. Mesh connectivity can be given to preCICE using the methods `setMeshTriangle` and `setMeshEdge`. Using the face centers as arguments for these methods is cumbersome. The main reason is that, although OpenFOAM decomposes the mesh for parallel simulations and distributes the subdomains to different processes, mesh connectivity needs to be defined over the partitioned mesh boundaries. This problem vanishes if we define mesh connectivity based on the face nodes, since boundary nodes can be shared among processors. Therefore, mesh connectivity can only be provided on the face nodes (not on the face centers).
+
+As described already, the data is not stored on the face nodes, but on the face centers. Therefore, we use OpenFOAM functions to interpolate from face centers to face nodes. The following image illustrates the workflow:
+
+
+
+Data is obtained at the face centers, then interpolated to face nodes. Here, we have provided mesh connectivity and finally, preCICE performs the nearest-projection mapping.
+It is important to notice that the target data location is again the face center mesh of the coupling partner. In the standard CHT case, where both data sets are exchanged by a nearest-projection mapping, this leads to two interface meshes (centers and nodes) per participant. Having both the centers and nodes defined, we can skip one interpolation step and read data directly to the centers (cf. picture solver B).
+
+### Supported fields
+As already mentioned, the `Fluid` participant does not need to provide the mesh connectivity in case of a standard FSI. Therefore, the `Solid` participant needs to provide it and nothing special needs to be considered compared to other mapping methods.
+This implementation supports all CHT-related fields, which are mapped with a `consistent` constraint. The required settings and differences compared to the basic tutorial are given below.
+
+### Changes in the Simulation Setup
+
+As we are defining two meshes for each participant, we need to define them in the `precice-config.xml` and `preciceDict` configuration files. Additionally, we need to enable the `connectivity` switch for the adapter.
+
+### Changes in `precice-config.xml`
+In order to map from face nodes to face centers, both meshes need to be specified. The nodes-based mesh uses the write data and the centers-based mesh uses the read data. Have a look in the given `precice-config.xml` in this tutorial. Example: `Temperature` is calculated by the `Fluid` participant and passed to the `Solid` participant. Therefore, it is the write data of the participant `Fluid` and the read data of the participant `Solid`. This results in the following two meshes for this data:
+```
+<mesh name="Fluid-Mesh-Nodes">
+ <use-data name="Temperature"/>
+</mesh>
+<mesh name="Solid-Mesh-Centers">
+ <use-data name="Temperature"/>
+</mesh>
+```
+All further changes follow from this interface splitting. Have a look in the given config files for all details.
+
+### Changes in `preciceDict`
+
+By default, the OpenFOAM adapter doesn't provide any connectivity information. Therefore, a new boolean variable called `connectivity` is introduced. This variable is associated to each interface and can be set accordingly. Note: Mesh connectivity can only be provided in case `locations faceNodes` is set (see section Adapter Implementation). Similar to the interface splitting in the `precice-config.xml` file, the interfaces also need to be defined in the `preciceDict` file. For example:
+
+```
+interfaces
+{
+ Interface1
+ {
+ mesh Fluid-Mesh-Centers;
+ locations faceCenters;
+ connectivity false;
+ patches (interface);
+
+ readData
+ (
+ Heat-Flux
+ );
+
+ writeData
+ (
+ );
+ };
+
+ Interface2
+ {
+ mesh Fluid-Mesh-Nodes;
+ locations faceNodes;
+ connectivity true;
+ patches (interface);
+
+ readData
+ (
+ );
+
+ writeData
+ (
+ Temperature
+ );
+ };
+};
+```
+The participant `Fluid` has its read data `Heat-Flux`, which is read on the `faceCenters`, and its write data `Temperature`, which is written to the `faceNodes`. The mesh connectivity needs only to be provided in case of the `faceNodes`, using the option `connectivity true`.
+
+### General Notes
+
+Since you now define mesh connectivity on your interface, you can export your coupling interface with the tag `<export:vtk directory="preCICE-output" />` in your `precice-config.xml`.
+
+Visualizing these files (e.g. using ParaView) will show a triangular mesh, even though you use hexahedral meshes. This has nothing to do with your mesh and is just caused by the way the connectivity is defined in preCICE. As described above, the function `setMeshTriangles` is used to define the connectivity. Hence, every interface cell/face is represented by two triangles. The following image should give you an impression of a possible triangulated coupling mesh, which consists purely of hexahedral cells:
+
+
+
+Note: Connectivity is defined on meshes associated with mesh nodes, which are named respectively e.g. `Fluid-Mesh-Nodes`. In this case, you could directly see the interface without applying filters by loading the `.vtk` files. In order to visualize additionally center based meshes, where no connectivity is provided, select a Glyph filter in ParaView. Furthermore, it makes a difference, on which participant the `<export...` tag is defined in your `precice-config.xml` file. Each participant exports interface meshes, which he provides or receives. The receiving participant filters out mesh parts that it does not need (for the mapping). Hence, a received mesh might look incomplete.
+
+### Notes on 2D Cases
+
+The geometry of the tutorial differs compared to the existing example: The out-of-plane thickness of the domain is reduced clearly and it is recommended. Otherwise your face centers have a quite large distance to the face nodes, which might trigger a preCICE warning. In that case, preCICE may filter out one of the meshes, especially in parallel simulations.
+
+{% include disclaimer.html content="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." %}
diff --git a/flow-over-heated-plate-nearest-projection/clean.sh b/flow-over-heated-plate-nearest-projection/clean.sh
new file mode 100755
index 000000000..994a8e844
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/clean.sh
@@ -0,0 +1,49 @@
+#!/bin/sh
+cd ${0%/*} || exit 1 # Run from this directory
+
+echo "Cleaning..."
+
+clean_case(){
+ cd ${1}
+ # Clean the result and auxiliary files
+ rm -fv *.vtk
+ rm -fv ${1}.log
+ rm -fv precice-*.log \
+ rm -fv precice-postProcessingInfo.log \
+ rm -fv precice-*-events.json
+}
+
+finished_clean(){
+cd ..
+}
+
+# Openfoam
+Name="fluid-openfoam"
+clean_case ${Name}
+ # Clean specialized files
+ if [ -n "${WM_PROJECT}" ];
+ then
+ . $WM_PROJECT_DIR/bin/tools/CleanFunctions
+ cleanCase
+ rm -rfv ./0
+ touch ${Name}.foam
+ fi
+finished_clean
+
+Name="solid-openfoam"
+clean_case ${Name}
+ # Clean specialized files
+ if [ -n "${WM_PROJECT}" ];
+ then
+ . $WM_PROJECT_DIR/bin/tools/CleanFunctions
+ cleanCase
+ rm -rfv ./0
+ touch ${Name}.foam
+ fi
+finished_clean
+
+# Remove the preCICE address files
+rm -rfv precice-run
+
+echo "Cleaning complete!"
+#------------------------------------------------------------------------------
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/T b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/T
new file mode 100644
index 000000000..ed002e908
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/T
@@ -0,0 +1,60 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object T;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [ 0 0 0 1 0 0 0 ];
+
+internalField uniform 300;
+
+boundaryField
+{
+ interface
+ {
+ type fixedGradient;
+ gradient uniform 0;
+ }
+ inlet
+ {
+ type fixedValue;
+ value $internalField;
+ }
+ outlet
+ {
+ type zeroGradient;
+ }
+ top
+ {
+ type zeroGradient;
+ }
+ bottom
+ {
+ type zeroGradient;
+ }
+ slip-bottom
+ {
+ type zeroGradient;
+ }
+ outerWall
+ {
+ type zeroGradient;
+ }
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/U b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/U
new file mode 100644
index 000000000..3cc2f65ee
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/U
@@ -0,0 +1,55 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volVectorField;
+ object U;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [ 0 1 -1 0 0 0 0 ];
+
+internalField uniform ( 0.1 0 0 );
+
+boundaryField
+{
+ interface
+ {
+ type noSlip;
+ }
+ inlet
+ {
+ type fixedValue;
+ value $internalField;
+ }
+ outlet
+ {
+ type zeroGradient;
+ }
+ top
+ {
+ type slip;
+ }
+ bottom
+ {
+ type noSlip;
+ }
+ slip-bottom
+ {
+ type slip;
+ }
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/alphat b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/alphat
new file mode 100644
index 000000000..8cdbda4b4
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/alphat
@@ -0,0 +1,61 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object alphat;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [ 1 -1 -1 0 0 0 0 ];
+
+internalField uniform 0;
+
+boundaryField
+{
+ interface
+ {
+ type compressible::alphatWallFunction;
+ value uniform 0;
+ }
+ inlet
+ {
+ type compressible::alphatWallFunction;
+ value uniform 0;
+ }
+ outlet
+ {
+ type compressible::alphatWallFunction;
+ value uniform 0;
+ }
+ top
+ {
+ type compressible::alphatWallFunction;
+ value uniform 0;
+ }
+ bottom
+ {
+ type compressible::alphatWallFunction;
+ value uniform 0;
+ }
+ slip-bottom
+ {
+ type compressible::alphatWallFunction;
+ value uniform 0;
+ }
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/epsilon b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/epsilon
new file mode 100644
index 000000000..a1374d174
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/epsilon
@@ -0,0 +1,61 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object epsilon;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [ 0 2 -3 0 0 0 0 ];
+
+internalField uniform 0.01;
+
+boundaryField
+{
+ interface
+ {
+ type epsilonWallFunction;
+ value uniform 0.01;
+ }
+ inlet
+ {
+ type epsilonWallFunction;
+ value uniform 0.01;
+ }
+ outlet
+ {
+ type epsilonWallFunction;
+ value uniform 0.01;
+ }
+ top
+ {
+ type epsilonWallFunction;
+ value uniform 0.01;
+ }
+ bottom
+ {
+ type epsilonWallFunction;
+ value uniform 0.01;
+ }
+ slip-bottom
+ {
+ type epsilonWallFunction;
+ value uniform 0.01;
+ }
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/k b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/k
new file mode 100644
index 000000000..87a6a0a83
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/k
@@ -0,0 +1,61 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object k;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [ 0 2 -2 0 0 0 0 ];
+
+internalField uniform 0.1;
+
+boundaryField
+{
+ interface
+ {
+ type kqRWallFunction;
+ value uniform 0.1;
+ }
+ inlet
+ {
+ type kqRWallFunction;
+ value uniform 0.1;
+ }
+ outlet
+ {
+ type kqRWallFunction;
+ value uniform 0.1;
+ }
+ top
+ {
+ type kqRWallFunction;
+ value uniform 0.1;
+ }
+ slip-bottom
+ {
+ type kqRWallFunction;
+ value uniform 0.1;
+ }
+ bottom
+ {
+ type kqRWallFunction;
+ value uniform 0.1;
+ }
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/nut b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/nut
new file mode 100644
index 000000000..9cb00d410
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/nut
@@ -0,0 +1,61 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ location "0";
+ object nut;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [ 0 2 -1 0 0 0 0 ];
+
+internalField uniform 0;
+
+boundaryField
+{
+ interface
+ {
+ type nutkWallFunction;
+ value uniform 0;
+ }
+ inlet
+ {
+ type nutkWallFunction;
+ value uniform 0;
+ }
+ outlet
+ {
+ type nutkWallFunction;
+ value uniform 0;
+ }
+ top
+ {
+ type nutkWallFunction;
+ value uniform 0;
+ }
+ bottom
+ {
+ type nutkWallFunction;
+ value uniform 0;
+ }
+ slip-bottom
+ {
+ type nutkWallFunction;
+ value uniform 0;
+ }
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/p b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/p
new file mode 100644
index 000000000..33c185074
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/p
@@ -0,0 +1,65 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object p;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [ 1 -1 -2 0 0 0 0 ];
+
+internalField uniform 103500;
+
+boundaryField
+{
+ interface
+ {
+ type calculated;
+ value $internalField;
+ }
+ inlet
+ {
+ type calculated;
+ value $internalField;
+ }
+ outlet
+ {
+ type calculated;
+ value $internalField;
+ }
+ outerWall
+ {
+ type calculated;
+ value $internalField;
+ }
+ top
+ {
+ type calculated;
+ value $internalField;
+ }
+ bottom
+ {
+ type calculated;
+ value $internalField;
+ }
+ slip-bottom
+ {
+ type calculated;
+ value $internalField;
+ }
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/p_rgh b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/p_rgh
new file mode 100644
index 000000000..6829b2c16
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/p_rgh
@@ -0,0 +1,55 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object p_rgh;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [ 1 -1 -2 0 0 0 0 ];
+
+internalField uniform 103500;
+
+boundaryField
+{
+ interface
+ {
+ type zeroGradient;
+ }
+ inlet
+ {
+ type zeroGradient;
+ }
+ outlet
+ {
+ type fixedValue;
+ value $internalField;
+ }
+ top
+ {
+ type zeroGradient;
+ }
+ slip-bottom
+ {
+ type zeroGradient;
+ }
+ bottom
+ {
+ type zeroGradient;
+ }
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/g b/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/g
new file mode 100644
index 000000000..66a77f74e
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/g
@@ -0,0 +1,22 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class uniformDimensionedVectorField;
+ location "constant";
+ object g;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 1 -2 0 0 0 0];
+value (0 -9.81 0);
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/thermophysicalProperties b/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/thermophysicalProperties
new file mode 100644
index 000000000..e47cdd82e
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/thermophysicalProperties
@@ -0,0 +1,49 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object thermophysicalProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+thermoType
+{
+ type heRhoThermo;
+ mixture pureMixture;
+ transport const;
+ thermo hConst;
+ equationOfState perfectGas;
+ specie specie;
+ energy sensibleEnthalpy;
+}
+
+mixture
+{
+ specie
+ {
+ nMoles 1;
+ molWeight 24.0999;
+ }
+ thermodynamics
+ {
+ Cp 5000.0;
+ Hf 0;
+ }
+ transport
+ {
+ mu 0.0002;
+ Pr 0.01;
+ }
+}
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/turbulenceProperties b/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/turbulenceProperties
new file mode 100644
index 000000000..95da7141e
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/turbulenceProperties
@@ -0,0 +1,26 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object turbulenceProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+simulationType laminar;
+
+RAS
+{
+ RASModel kEpsilon;
+ turbulence off;
+}
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/fluid-openfoam.foam b/flow-over-heated-plate-nearest-projection/fluid-openfoam/fluid-openfoam.foam
new file mode 100644
index 000000000..e69de29bb
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/removeObsoleteFolders.sh b/flow-over-heated-plate-nearest-projection/fluid-openfoam/removeObsoleteFolders.sh
new file mode 100755
index 000000000..167e40f61
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/removeObsoleteFolders.sh
@@ -0,0 +1,22 @@
+#! /bin/bash
+
+echo "Looking for any time directories without results (e.g. stray functionObjectProperties files, see issue #26 on GitHub)..."
+
+for f in [0-9]* [0-9]*.[0-9]*; do
+ if ! [ -f $f/U ] && ! [ -f $f/T ]; then
+ rm -rfv $f
+ fi
+done
+if [ -d processor0 ]; then
+ for g in processor*; do
+ cd $g
+ for f in [0-9]* [0-9]*.[0-9]*; do
+ if ! [ -f $f/U ] && ! [ -f $f/T ]; then
+ rm -rfv $f
+ fi
+ done
+ cd ..
+ done
+fi
+cd ..
+
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/run.sh b/flow-over-heated-plate-nearest-projection/fluid-openfoam/run.sh
new file mode 100755
index 000000000..29c9416f4
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/run.sh
@@ -0,0 +1,44 @@
+#!/bin/bash
+cd ${0%/*} || exit 1 # Run from this directory
+. $WM_PROJECT_DIR/bin/tools/RunFunctions # Tutorial run functions
+
+# Fluid participant
+
+# Run this script in one terminal and the "runSolid" script in another terminal.
+# These scripts present how the two participants would be started manually.
+# Alternatively, you may execute the "Allrun" script in one terminal.
+
+# Run this script with "-parallel" for parallel simulations
+
+# The script "Allclean" cleans-up the result and log files.
+
+# 1 for true, 0 for false
+parallel=0
+if [ "$1" = "-parallel" ]; then
+ parallel=1
+fi
+
+echo "Preparing and running the Fluid participant..."
+
+rm -rfv 0/
+cp -r 0.orig/ 0/
+blockMesh
+checkMesh
+
+# Run
+solver=$(getApplication)
+procs=$(getNumberOfProcessors)
+
+if [ $parallel -eq 1 ]; then
+ decomposePar -force
+ mpirun -np $procs $solver -parallel
+ reconstructPar
+else
+ $solver
+fi
+
+# Workaround for issue #26
+./removeObsoleteFolders.sh
+
+echo ""
+echo "### NOTE ### Make sure to use the correct solver for your OpenFOAM version! (pimpleFoam for OpenFOAM v1806, OpenFOAM 6, or newer, vs pimpleDyMFoam for older) You may change this in your Fluid/system/controlDict file, if needed."
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/blockMeshDict b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/blockMeshDict
new file mode 100644
index 000000000..a16782a68
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/blockMeshDict
@@ -0,0 +1,121 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+convertToMeters 1;
+
+vertices
+(
+ (0 0 0)
+ (1 0 0)
+ (1 .5 0)
+ (0 .5 0)
+
+ (0 0 .01)
+ (1 0 .01)
+ (1 .5 .01)
+ (0 .5 .01)
+
+ (3 0 0)
+ (3 .5 0)
+
+ (3 0 .01)
+ (3 .5 .01)
+
+ (-.5 0 0)
+ (-.5 .5 0)
+
+ (-.5 .5 .01)
+ (-.5 0 .01)
+
+);
+
+blocks
+(
+ hex (12 0 3 13 15 4 7 14) (81 41 1) simpleGrading (.2 15 1)
+ hex (0 1 2 3 4 5 6 7) (161 41 1) simpleGrading (5 15 1)
+ hex (1 8 9 2 5 10 11 6) (51 41 1) simpleGrading (1 15 1)
+);
+
+edges
+(
+);
+
+boundary
+(
+
+ inlet
+ {
+ type wall;
+ faces
+ (
+ (13 12 15 14)
+ );
+ }
+
+ outlet
+ {
+ type wall;
+ faces
+ (
+ (8 9 11 10)
+ );
+ }
+
+ top
+ {
+ type wall;
+ faces
+ (
+ (7 6 2 3)
+ (9 2 6 11)
+ (13 3 7 14)
+ );
+ }
+
+ slip-bottom
+ {
+ type wall;
+ faces
+ (
+ (15 12 0 4)
+ );
+ }
+
+ bottom
+ {
+ type wall;
+ faces
+ (
+ (1 8 10 5)
+ );
+ }
+
+ interface
+ {
+ type wall;
+ faces
+ (
+ (4 0 1 5)
+ );
+ }
+
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/controlDict b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/controlDict
new file mode 100644
index 000000000..bdfdb5da9
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/controlDict
@@ -0,0 +1,59 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application buoyantPimpleFoam;
+
+startFrom startTime;
+
+startTime 0;
+
+stopAt endTime;
+
+endTime 1;
+
+deltaT 0.01;
+
+writeControl runTime;
+
+writeInterval 0.2;
+
+purgeWrite 0;
+
+writeFormat ascii;
+
+writePrecision 6;
+
+writeCompression off;
+
+timeFormat general;
+
+timePrecision 6;
+
+runTimeModifiable false;
+
+functions
+{
+ preCICE_Adapter
+ {
+ type preciceAdapterFunctionObject;
+ libs ("libpreciceAdapterFunctionObject.so");
+ }
+}
+
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/decomposeParDict b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/decomposeParDict
new file mode 100644
index 000000000..ad99cf6c5
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/decomposeParDict
@@ -0,0 +1,16 @@
+FoamFile {
+ version 2.0;
+ class dictionary;
+ object decomposeParDict;
+ format ascii;
+}
+
+numberOfSubdomains 2;
+
+method simple;
+
+simpleCoeffs
+{
+ n (2 1 1);
+ delta 0.001;
+}
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/fvSchemes b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/fvSchemes
new file mode 100644
index 000000000..3eb3688c2
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/fvSchemes
@@ -0,0 +1,59 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+ default Euler;
+}
+
+gradSchemes
+{
+ default Gauss linear;
+}
+
+divSchemes
+{
+ default none;
+ div(phi,U) Gauss upwind;
+ div(phi,h) Gauss upwind;
+ div(phi,e) Gauss upwind;
+ div(phi,k) Gauss upwind;
+ div(phi,epsilon) Gauss upwind;
+ div(phi,R) Gauss upwind;
+ div(phi,K) Gauss linear;
+ div(phi,Ekp) Gauss linear;
+ div(R) Gauss linear;
+ div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
+}
+
+laplacianSchemes
+{
+ default Gauss linear corrected;
+}
+
+interpolationSchemes
+{
+ default linear;
+}
+
+snGradSchemes
+{
+ default corrected;
+}
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/fvSolution b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/fvSolution
new file mode 100644
index 000000000..e55987f34
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/fvSolution
@@ -0,0 +1,66 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+ "rho.*"
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 0;
+ relTol 0;
+ }
+
+ p_rgh
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 1e-8;
+ relTol 0.01;
+ }
+
+ p_rghFinal
+ {
+ $p_rgh;
+ relTol 0;
+ }
+
+ "(U|h|e|k|epsilon|R)"
+ {
+ solver PBiCGStab;
+ preconditioner DILU;
+ tolerance 1e-6;
+ relTol 0.1;
+ }
+
+ "(U|h|e|k|epsilon|R)Final"
+ {
+ $U;
+ relTol 0;
+ }
+}
+
+PIMPLE
+{
+ momentumPredictor yes;
+ nOuterCorrectors 1;
+ nCorrectors 2;
+ nNonOrthogonalCorrectors 0;
+}
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/preciceDict b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/preciceDict
new file mode 100644
index 000000000..57df62850
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/preciceDict
@@ -0,0 +1,51 @@
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object preciceDict;
+}
+
+preciceConfig "../precice-config.xml";
+
+participant Fluid;
+
+modules (CHT);
+
+interfaces
+{
+ Interface1
+ {
+ mesh Fluid-Mesh-Centers;
+ locations faceCenters;
+ connectivity false;
+ patches (interface);
+
+ readData
+ (
+ Heat-Flux
+ );
+
+ writeData
+ (
+ );
+ };
+
+ Interface2
+ {
+ mesh Fluid-Mesh-Nodes;
+ locations faceNodes;
+ connectivity true;
+ patches (interface);
+
+ readData
+ (
+ );
+
+ writeData
+ (
+ Temperature
+ );
+ };
+};
diff --git a/flow-over-heated-plate-nearest-projection/precice-config.xml b/flow-over-heated-plate-nearest-projection/precice-config.xml
new file mode 100644
index 000000000..36e346ae8
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/precice-config.xml
@@ -0,0 +1,76 @@
+<?xml version="1.0" encoding="UTF-8" ?>
+<precice-configuration>
+ <log>
+ <sink
+ filter="%Severity% > debug and %Rank% = 0"
+ format="---[precice] %ColorizedSeverity% %Message%"
+ enabled="true" />
+ </log>
+
+ <solver-interface dimensions="3">
+ <data:scalar name="Temperature" />
+ <data:scalar name="Heat-Flux" />
+
+ <mesh name="Fluid-Mesh-Centers">
+ <use-data name="Heat-Flux" />
+ </mesh>
+
+ <mesh name="Fluid-Mesh-Nodes">
+ <use-data name="Temperature" />
+ </mesh>
+
+ <mesh name="Solid-Mesh-Centers">
+ <use-data name="Temperature" />
+ </mesh>
+
+ <mesh name="Solid-Mesh-Nodes">
+ <use-data name="Heat-Flux" />
+ </mesh>
+
+ <participant name="Fluid">
+ <use-mesh name="Fluid-Mesh-Centers" provide="yes" />
+ <use-mesh name="Fluid-Mesh-Nodes" provide="yes" />
+ <use-mesh name="Solid-Mesh-Nodes" from="Solid" />
+ <read-data name="Heat-Flux" mesh="Fluid-Mesh-Centers" />
+ <write-data name="Temperature" mesh="Fluid-Mesh-Nodes" />
+ <mapping:nearest-projection
+ direction="read"
+ from="Solid-Mesh-Nodes"
+ to="Fluid-Mesh-Centers"
+ constraint="consistent" />
+ </participant>
+
+ <participant name="Solid">
+ <use-mesh name="Fluid-Mesh-Nodes" from="Fluid" />
+ <use-mesh name="Solid-Mesh-Nodes" provide="yes" />
+ <use-mesh name="Solid-Mesh-Centers" provide="yes" />
+ <read-data name="Temperature" mesh="Solid-Mesh-Centers" />
+ <write-data name="Heat-Flux" mesh="Solid-Mesh-Nodes" />
+ <!-- <export:vtk directory="preCICE-output" /> -->
+ <mapping:nearest-projection
+ direction="read"
+ from="Fluid-Mesh-Nodes"
+ to="Solid-Mesh-Centers"
+ constraint="consistent" />
+ </participant>
+
+ <m2n:sockets from="Fluid" to="Solid" exchange-directory=".."/>
+
+ <coupling-scheme:serial-implicit>
+ <time-window-size value="0.01" />
+ <max-time value="1" />
+ <participants first="Fluid" second="Solid" />
+ <exchange data="Temperature" mesh="Fluid-Mesh-Nodes" from="Fluid" to="Solid" />
+ <exchange data="Heat-Flux" mesh="Solid-Mesh-Nodes" from="Solid" to="Fluid" />
+ <max-iterations value="200" />
+ <relative-convergence-measure limit="1.0e-6" data="Temperature" mesh="Fluid-Mesh-Nodes" />
+ <acceleration:IQN-ILS>
+ <data mesh="Solid-Mesh-Nodes" name="Heat-Flux" />
+ <initial-relaxation value="0.01" />
+ <max-used-iterations value="80" />
+ <time-windows-reused value="10" />
+ <filter type="QR1" limit="1e-8" />
+ </acceleration:IQN-ILS>
+ </coupling-scheme:serial-implicit>
+ </solver-interface>
+</precice-configuration>
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/0.orig/T b/flow-over-heated-plate-nearest-projection/solid-openfoam/0.orig/T
new file mode 100644
index 000000000..ffaa360be
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/0.orig/T
@@ -0,0 +1,47 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class volScalarField;
+ object T;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+dimensions [0 0 0 1 0 0 0];
+
+internalField uniform 310;
+
+boundaryField
+{
+ interface
+ {
+ type fixedValue;
+ value $internalField;
+ }
+ left
+ {
+ type zeroGradient;
+ }
+ right
+ {
+ type zeroGradient;
+ }
+ bottom
+ {
+ type fixedValue;
+ value $internalField;
+ }
+ defaultFaces
+ {
+ type empty;
+ }
+}
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/constant/transportProperties b/flow-over-heated-plate-nearest-projection/solid-openfoam/constant/transportProperties
new file mode 100644
index 000000000..40eaee612
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/constant/transportProperties
@@ -0,0 +1,21 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "constant";
+ object transportProperties;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+DT DT [ 0 2 -1 0 0 0 0 ] 1;
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/removeObsoleteFolders.sh b/flow-over-heated-plate-nearest-projection/solid-openfoam/removeObsoleteFolders.sh
new file mode 100755
index 000000000..167e40f61
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/removeObsoleteFolders.sh
@@ -0,0 +1,22 @@
+#! /bin/bash
+
+echo "Looking for any time directories without results (e.g. stray functionObjectProperties files, see issue #26 on GitHub)..."
+
+for f in [0-9]* [0-9]*.[0-9]*; do
+ if ! [ -f $f/U ] && ! [ -f $f/T ]; then
+ rm -rfv $f
+ fi
+done
+if [ -d processor0 ]; then
+ for g in processor*; do
+ cd $g
+ for f in [0-9]* [0-9]*.[0-9]*; do
+ if ! [ -f $f/U ] && ! [ -f $f/T ]; then
+ rm -rfv $f
+ fi
+ done
+ cd ..
+ done
+fi
+cd ..
+
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/run.sh b/flow-over-heated-plate-nearest-projection/solid-openfoam/run.sh
new file mode 100755
index 000000000..29c9416f4
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/run.sh
@@ -0,0 +1,44 @@
+#!/bin/bash
+cd ${0%/*} || exit 1 # Run from this directory
+. $WM_PROJECT_DIR/bin/tools/RunFunctions # Tutorial run functions
+
+# Fluid participant
+
+# Run this script in one terminal and the "runSolid" script in another terminal.
+# These scripts present how the two participants would be started manually.
+# Alternatively, you may execute the "Allrun" script in one terminal.
+
+# Run this script with "-parallel" for parallel simulations
+
+# The script "Allclean" cleans-up the result and log files.
+
+# 1 for true, 0 for false
+parallel=0
+if [ "$1" = "-parallel" ]; then
+ parallel=1
+fi
+
+echo "Preparing and running the Fluid participant..."
+
+rm -rfv 0/
+cp -r 0.orig/ 0/
+blockMesh
+checkMesh
+
+# Run
+solver=$(getApplication)
+procs=$(getNumberOfProcessors)
+
+if [ $parallel -eq 1 ]; then
+ decomposePar -force
+ mpirun -np $procs $solver -parallel
+ reconstructPar
+else
+ $solver
+fi
+
+# Workaround for issue #26
+./removeObsoleteFolders.sh
+
+echo ""
+echo "### NOTE ### Make sure to use the correct solver for your OpenFOAM version! (pimpleFoam for OpenFOAM v1806, OpenFOAM 6, or newer, vs pimpleDyMFoam for older) You may change this in your Fluid/system/controlDict file, if needed."
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/solid-openfoam.foam b/flow-over-heated-plate-nearest-projection/solid-openfoam/solid-openfoam.foam
new file mode 100644
index 000000000..e69de29bb
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/system/blockMeshDict b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/blockMeshDict
new file mode 100644
index 000000000..5b1e1e579
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/blockMeshDict
@@ -0,0 +1,88 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 2.4.0 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ object blockMeshDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+convertToMeters 1;
+
+vertices
+(
+
+ (0 -.25 0)
+ (1 -.25 0)
+ (1 0 0)
+ (0 0 0)
+
+ (0 -.25 .01)
+ (1 -.25 .01)
+ (1 0 .01)
+ (0 0 .01)
+
+);
+
+blocks
+(
+ hex (0 1 2 3 4 5 6 7) (32 16 1) simpleGrading (1 1 1)
+);
+
+edges
+(
+);
+
+boundary
+(
+
+ left
+ {
+ type wall;
+ faces
+ (
+ (4 7 3 0)
+ );
+ }
+
+ right
+ {
+ type wall;
+ faces
+ (
+ (1 2 6 5)
+ );
+ }
+
+ interface
+ {
+ type wall;
+ faces
+ (
+ (7 6 2 3)
+ );
+ }
+
+ bottom
+ {
+ type wall;
+ faces
+ (
+ (4 0 1 5)
+ );
+ }
+
+);
+
+mergePatchPairs
+(
+);
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/system/controlDict b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/controlDict
new file mode 100644
index 000000000..5570d8606
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/controlDict
@@ -0,0 +1,59 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object controlDict;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+application laplacianFoam;
+
+startFrom startTime;
+
+startTime 0;
+
+stopAt endTime;
+
+endTime 1;
+
+deltaT 0.01;
+
+writeControl runTime;
+
+writeInterval 0.2;
+
+purgeWrite 0;
+
+writeFormat ascii;
+
+writePrecision 6;
+
+writeCompression off;
+
+timeFormat general;
+
+timePrecision 6;
+
+runTimeModifiable false;
+
+functions
+{
+ preCICE_Adapter
+ {
+ type preciceAdapterFunctionObject;
+ libs ("libpreciceAdapterFunctionObject.so");
+ }
+}
+
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/system/decomposeParDict b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/decomposeParDict
new file mode 100644
index 000000000..ad99cf6c5
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/decomposeParDict
@@ -0,0 +1,16 @@
+FoamFile {
+ version 2.0;
+ class dictionary;
+ object decomposeParDict;
+ format ascii;
+}
+
+numberOfSubdomains 2;
+
+method simple;
+
+simpleCoeffs
+{
+ n (2 1 1);
+ delta 0.001;
+}
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/system/fvSchemes b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/fvSchemes
new file mode 100644
index 000000000..b615f6dc7
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/fvSchemes
@@ -0,0 +1,51 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object fvSchemes;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+ddtSchemes
+{
+ default Euler;
+}
+
+gradSchemes
+{
+ default Gauss linear;
+ grad(T) Gauss linear;
+}
+
+divSchemes
+{
+ default none;
+}
+
+laplacianSchemes
+{
+ default none;
+ laplacian(DT,T) Gauss linear corrected;
+}
+
+interpolationSchemes
+{
+ default linear;
+}
+
+snGradSchemes
+{
+ default corrected;
+}
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/system/fvSolution b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/fvSolution
new file mode 100644
index 000000000..8362241bb
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/fvSolution
@@ -0,0 +1,35 @@
+/*--------------------------------*- C++ -*----------------------------------*\
+| ========= | |
+| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
+| \\ / O peration | Version: 5 |
+| \\ / A nd | Web: www.OpenFOAM.org |
+| \\/ M anipulation | |
+\*---------------------------------------------------------------------------*/
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object fvSolution;
+}
+// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
+
+solvers
+{
+ T
+ {
+ solver PCG;
+ preconditioner DIC;
+ tolerance 1e-06;
+ relTol 0;
+ }
+}
+
+SIMPLE
+{
+ nNonOrthogonalCorrectors 2;
+}
+
+
+// ************************************************************************* //
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/system/preciceDict b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/preciceDict
new file mode 100644
index 000000000..3d3e6ebaa
--- /dev/null
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/preciceDict
@@ -0,0 +1,57 @@
+FoamFile
+{
+ version 2.0;
+ format ascii;
+ class dictionary;
+ location "system";
+ object preciceDict;
+}
+
+preciceConfig "../precice-config.xml";
+
+participant Solid;
+
+modules (CHT);
+
+interfaces
+{
+ Interface1
+ {
+ mesh Solid-Mesh-Centers;
+ locations faceCenters;
+ connectivity false;
+ patches (interface);
+
+ readData
+ (
+ Temperature
+ );
+
+ writeData
+ (
+ );
+ };
+
+ Interfaces2
+ {
+ mesh Solid-Mesh-Nodes;
+ locations faceNodes;
+ connectivity true;
+ patches (interface);
+
+ readData
+ (
+ );
+
+ writeData
+ (
+ Heat-Flux
+ );
+ };
+};
+
+CHT
+{
+ k [ 1 1 -3 -1 0 0 0 ] 100;
+ solverType "basic";
+};
From fe669a3eca269ecddc6cc0cd0550281c2ae7f2a6 Mon Sep 17 00:00:00 2001
From: DavidSCN <david.schneider@ipvs.uni-stuttgart.de>
Date: Fri, 12 Mar 2021 15:12:30 +0100
Subject: [PATCH 2/6] Remove OpenFOAM merch header
---
.../fluid-openfoam/0.orig/T | 7 -------
.../fluid-openfoam/0.orig/U | 7 -------
.../fluid-openfoam/0.orig/alphat | 7 -------
.../fluid-openfoam/0.orig/epsilon | 7 -------
.../fluid-openfoam/0.orig/k | 7 -------
.../fluid-openfoam/0.orig/nut | 7 -------
.../fluid-openfoam/0.orig/p | 7 -------
.../fluid-openfoam/0.orig/p_rgh | 7 -------
.../solid-openfoam/0.orig/T | 7 -------
9 files changed, 63 deletions(-)
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/T b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/T
index ed002e908..fad9ded3e 100644
--- a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/T
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/T
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/U b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/U
index 3cc2f65ee..2d9ee8fcb 100644
--- a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/U
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/U
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/alphat b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/alphat
index 8cdbda4b4..658075c8a 100644
--- a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/alphat
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/alphat
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/epsilon b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/epsilon
index a1374d174..763f85ba3 100644
--- a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/epsilon
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/epsilon
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/k b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/k
index 87a6a0a83..3fcebfa3c 100644
--- a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/k
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/k
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/nut b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/nut
index 9cb00d410..72e6ef35a 100644
--- a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/nut
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/nut
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/p b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/p
index 33c185074..6eb21cecf 100644
--- a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/p
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/p
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/p_rgh b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/p_rgh
index 6829b2c16..31673b434 100644
--- a/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/p_rgh
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/0.orig/p_rgh
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/0.orig/T b/flow-over-heated-plate-nearest-projection/solid-openfoam/0.orig/T
index ffaa360be..96fc74129 100644
--- a/flow-over-heated-plate-nearest-projection/solid-openfoam/0.orig/T
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/0.orig/T
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
From d792db9193949bbd934b072af9932b3e8c407d2e Mon Sep 17 00:00:00 2001
From: DavidSCN <david.schneider@ipvs.uni-stuttgart.de>
Date: Fri, 12 Mar 2021 15:14:47 +0100
Subject: [PATCH 3/6] Remove OpenFOAM merch header pt 2
---
.../fluid-openfoam/constant/g | 7 -------
.../fluid-openfoam/constant/thermophysicalProperties | 7 -------
.../fluid-openfoam/constant/turbulenceProperties | 7 -------
.../fluid-openfoam/system/blockMeshDict | 7 -------
.../fluid-openfoam/system/controlDict | 7 -------
.../fluid-openfoam/system/fvSchemes | 7 -------
.../fluid-openfoam/system/fvSolution | 7 -------
.../solid-openfoam/constant/transportProperties | 7 -------
.../solid-openfoam/system/blockMeshDict | 7 -------
.../solid-openfoam/system/controlDict | 7 -------
.../solid-openfoam/system/fvSchemes | 8 --------
.../solid-openfoam/system/fvSolution | 7 -------
12 files changed, 85 deletions(-)
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/g b/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/g
index 66a77f74e..9d33548db 100644
--- a/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/g
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/g
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/thermophysicalProperties b/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/thermophysicalProperties
index e47cdd82e..9992c3670 100644
--- a/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/thermophysicalProperties
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/thermophysicalProperties
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/turbulenceProperties b/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/turbulenceProperties
index 95da7141e..a5ca2ead4 100644
--- a/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/turbulenceProperties
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/constant/turbulenceProperties
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/blockMeshDict b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/blockMeshDict
index a16782a68..de9322736 100644
--- a/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/blockMeshDict
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/blockMeshDict
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/controlDict b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/controlDict
index bdfdb5da9..1f4d27106 100644
--- a/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/controlDict
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/controlDict
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/fvSchemes b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/fvSchemes
index 3eb3688c2..16fe50adc 100644
--- a/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/fvSchemes
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/fvSchemes
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/fvSolution b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/fvSolution
index e55987f34..ea2b78f4c 100644
--- a/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/fvSolution
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/system/fvSolution
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/constant/transportProperties b/flow-over-heated-plate-nearest-projection/solid-openfoam/constant/transportProperties
index 40eaee612..2a7a60f85 100644
--- a/flow-over-heated-plate-nearest-projection/solid-openfoam/constant/transportProperties
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/constant/transportProperties
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/system/blockMeshDict b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/blockMeshDict
index 5b1e1e579..d0fb694e6 100644
--- a/flow-over-heated-plate-nearest-projection/solid-openfoam/system/blockMeshDict
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/blockMeshDict
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 2.4.0 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/system/controlDict b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/controlDict
index 5570d8606..0920237a7 100644
--- a/flow-over-heated-plate-nearest-projection/solid-openfoam/system/controlDict
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/controlDict
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/system/fvSchemes b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/fvSchemes
index b615f6dc7..da42ee4e0 100644
--- a/flow-over-heated-plate-nearest-projection/solid-openfoam/system/fvSchemes
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/fvSchemes
@@ -1,11 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
-FoamFile
{
version 2.0;
format ascii;
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/system/fvSolution b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/fvSolution
index 8362241bb..74d1bdfd5 100644
--- a/flow-over-heated-plate-nearest-projection/solid-openfoam/system/fvSolution
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/system/fvSolution
@@ -1,10 +1,3 @@
-/*--------------------------------*- C++ -*----------------------------------*\
-| ========= | |
-| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
-| \\ / O peration | Version: 5 |
-| \\ / A nd | Web: www.OpenFOAM.org |
-| \\/ M anipulation | |
-\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
From d026b15d0a3cc929e5085d9fc5b5a9153d6879a8 Mon Sep 17 00:00:00 2001
From: DavidSCN <david.schneider@ipvs.uni-stuttgart.de>
Date: Fri, 12 Mar 2021 15:21:05 +0100
Subject: [PATCH 4/6] Update run.sh script documentation
---
.../fluid-openfoam/run.sh | 7 +------
.../solid-openfoam/run.sh | 7 +------
perpendicular-flap/fluid-openfoam/run.sh | 7 +------
3 files changed, 3 insertions(+), 18 deletions(-)
diff --git a/flow-over-heated-plate-nearest-projection/fluid-openfoam/run.sh b/flow-over-heated-plate-nearest-projection/fluid-openfoam/run.sh
index 29c9416f4..c39667789 100755
--- a/flow-over-heated-plate-nearest-projection/fluid-openfoam/run.sh
+++ b/flow-over-heated-plate-nearest-projection/fluid-openfoam/run.sh
@@ -4,14 +4,9 @@ cd ${0%/*} || exit 1 # Run from this directory
# Fluid participant
-# Run this script in one terminal and the "runSolid" script in another terminal.
-# These scripts present how the two participants would be started manually.
-# Alternatively, you may execute the "Allrun" script in one terminal.
-
+# Run this script in one terminal in order to start this participant.
# Run this script with "-parallel" for parallel simulations
-# The script "Allclean" cleans-up the result and log files.
-
# 1 for true, 0 for false
parallel=0
if [ "$1" = "-parallel" ]; then
diff --git a/flow-over-heated-plate-nearest-projection/solid-openfoam/run.sh b/flow-over-heated-plate-nearest-projection/solid-openfoam/run.sh
index 29c9416f4..c39667789 100755
--- a/flow-over-heated-plate-nearest-projection/solid-openfoam/run.sh
+++ b/flow-over-heated-plate-nearest-projection/solid-openfoam/run.sh
@@ -4,14 +4,9 @@ cd ${0%/*} || exit 1 # Run from this directory
# Fluid participant
-# Run this script in one terminal and the "runSolid" script in another terminal.
-# These scripts present how the two participants would be started manually.
-# Alternatively, you may execute the "Allrun" script in one terminal.
-
+# Run this script in one terminal in order to start this participant.
# Run this script with "-parallel" for parallel simulations
-# The script "Allclean" cleans-up the result and log files.
-
# 1 for true, 0 for false
parallel=0
if [ "$1" = "-parallel" ]; then
diff --git a/perpendicular-flap/fluid-openfoam/run.sh b/perpendicular-flap/fluid-openfoam/run.sh
index 29c9416f4..c39667789 100755
--- a/perpendicular-flap/fluid-openfoam/run.sh
+++ b/perpendicular-flap/fluid-openfoam/run.sh
@@ -4,14 +4,9 @@ cd ${0%/*} || exit 1 # Run from this directory
# Fluid participant
-# Run this script in one terminal and the "runSolid" script in another terminal.
-# These scripts present how the two participants would be started manually.
-# Alternatively, you may execute the "Allrun" script in one terminal.
-
+# Run this script in one terminal in order to start this participant.
# Run this script with "-parallel" for parallel simulations
-# The script "Allclean" cleans-up the result and log files.
-
# 1 for true, 0 for false
parallel=0
if [ "$1" = "-parallel" ]; then
From 6595fe8a724166986a4de3effd66df2cd5918026 Mon Sep 17 00:00:00 2001
From: DavidSCN <david.schneider@ipvs.uni-stuttgart.de>
Date: Mon, 22 Mar 2021 14:00:42 +0100
Subject: [PATCH 5/6] Move parts from this tutorial to the adapter docs
---
.../README.md | 94 +++++--------------
1 file changed, 22 insertions(+), 72 deletions(-)
diff --git a/flow-over-heated-plate-nearest-projection/README.md b/flow-over-heated-plate-nearest-projection/README.md
index 670c1c27b..1b9b99bcb 100644
--- a/flow-over-heated-plate-nearest-projection/README.md
+++ b/flow-over-heated-plate-nearest-projection/README.md
@@ -2,25 +2,12 @@
title: Flow over heated plate nearest projection
permalink: tutorials-flow-over-heated-plate-nearest-projection.html
keywords: OpenFOAM, nearest-projection, CHT
-summary: This tutorial introduces an example simulation setup for nearest-projection mapping with the OpenFOAM adapter. The demonstrated "flow over a heated plate" scenario is exactly the same as in the `buoyantPimpleFoam-laplacianFoam` tutorial (with a thinner plate). The following text explains the _general functionality_ of the adapter, the _current capability_ of the adapter and the necessary _changes in the tutorials_ for your own simulation.
+summary: This tutorial introduces an example simulation setup for a nearest-projection mapping. At the moment, it only contains an example with the OpenFOAM adapter. The demonstrated "flow over a heated plate" scenario is exactly the same as in the `buoyantPimpleFoam-laplacianFoam` tutorial.
---
## Setup
-The setup is exactly the same as described in our [flow-over-heated-plate tutorial](tutorials-flow-over-heated-plate.html). Since the physical setup is not the main concern of this tutorial, we focus in the following on the nearest-projection mapping within preCICE. Let's start with general information about mapping methods. The [preCICE docs](configuration-mapping.html) contains an overview with available mapping methods in preCICE. The nearest-projection mapping is a second-order method. But, contrary to the RBF mapping, mesh connectivity information is needed for the interpolation.
-There are two participants in each mapping, but the connectivity of one mesh is sufficient for an interpolation. Which of the participants must provide mesh connectivity is not arbitrary and depends on the constraint type:
-
-- for `consistent` mappings, the `from` participant needs to provide connectivity
-- for `conservative` mappings, the `to` participant needs to provide connectivity
-
-For example, in our case, we exchange `Temperature` data in a `consistent` way from the `Fluid` to the `Solid` participant. Hence, `Fluid` needs to provide mesh connectivity.
-
-Notes:
-
-- In a standard **CHT** calculation, both data sets (heat flux and temperature) are mapped consistently. Therefore, both participants need to provide connectivity.
-- In a standard **FSI** calculation, forces are mapped conservatively from `Fluid` to `Solid`, while displacements are mapped consistently from `Solid` to `Fluid`. Hence, it is `Solid` that needs to provide connectivity and not `Fluid`.
-
-If mesh connectivity is not provided in the described way, you are nevertheless able to define a nearest-projection mapping in your `precice-config.xml`file, but it will _fall back to a first-order nearest-neighbor mapping_.
+The setup is exactly the same as described in our [flow-over-heated-plate tutorial](tutorials-flow-over-heated-plate.html).
## Available solvers
@@ -32,20 +19,26 @@ Solid participant:
* OpenFOAM (laplacianFoam). For more information, have a look at the [OpenFOAM adapter documentation](adapter-openfoam-overview.html).
-Since OpenFOAM is a finite-volume based solver, data is located in the middle of the cell, or on the cell face centers for a coupling interface. Mesh connectivity can be given to preCICE using the methods `setMeshTriangle` and `setMeshEdge`. Using the face centers as arguments for these methods is cumbersome. The main reason is that, although OpenFOAM decomposes the mesh for parallel simulations and distributes the subdomains to different processes, mesh connectivity needs to be defined over the partitioned mesh boundaries. This problem vanishes if we define mesh connectivity based on the face nodes, since boundary nodes can be shared among processors. Therefore, mesh connectivity can only be provided on the face nodes (not on the face centers).
+The solvers are currently only OpenFOAM related. For information regarding the nearest-projection mapping, have a look in the [OpenFOAM configuration section](adapter-openfoam-config.html).
-As described already, the data is not stored on the face nodes, but on the face centers. Therefore, we use OpenFOAM functions to interpolate from face centers to face nodes. The following image illustrates the workflow:
-
+## Running the Simulation
-Data is obtained at the face centers, then interpolated to face nodes. Here, we have provided mesh connectivity and finally, preCICE performs the nearest-projection mapping.
-It is important to notice that the target data location is again the face center mesh of the coupling partner. In the standard CHT case, where both data sets are exchanged by a nearest-projection mapping, this leads to two interface meshes (centers and nodes) per participant. Having both the centers and nodes defined, we can skip one interpolation step and read data directly to the centers (cf. picture solver B).
+Open two separate terminals and start each participant by calling the respective run script.
-### Supported fields
-As already mentioned, the `Fluid` participant does not need to provide the mesh connectivity in case of a standard FSI. Therefore, the `Solid` participant needs to provide it and nothing special needs to be considered compared to other mapping methods.
-This implementation supports all CHT-related fields, which are mapped with a `consistent` constraint. The required settings and differences compared to the basic tutorial are given below.
+```
+cd fluid-openfoam
+./run.sh
+```
+and
+```
+cd solid-openfoam
+./run.sh
+```
-### Changes in the Simulation Setup
+You can also run OpenFOAM in parallel by `./run.sh -parallel`. If you are using OpenFOAM v1712 / 5.x or older have a look in the `fluid-openfoam/system/controlDict` file and set the appropriate solver name.
+
+## Changes in the Simulation Setup
As we are defining two meshes for each participant, we need to define them in the `precice-config.xml` and `preciceDict` configuration files. Additionally, we need to enable the `connectivity` switch for the adapter.
@@ -61,62 +54,19 @@ In order to map from face nodes to face centers, both meshes need to be specifie
```
All further changes follow from this interface splitting. Have a look in the given config files for all details.
-### Changes in `preciceDict`
-
-By default, the OpenFOAM adapter doesn't provide any connectivity information. Therefore, a new boolean variable called `connectivity` is introduced. This variable is associated to each interface and can be set accordingly. Note: Mesh connectivity can only be provided in case `locations faceNodes` is set (see section Adapter Implementation). Similar to the interface splitting in the `precice-config.xml` file, the interfaces also need to be defined in the `preciceDict` file. For example:
+### Notes on 2D Cases
-```
-interfaces
-{
- Interface1
- {
- mesh Fluid-Mesh-Centers;
- locations faceCenters;
- connectivity false;
- patches (interface);
-
- readData
- (
- Heat-Flux
- );
-
- writeData
- (
- );
- };
-
- Interface2
- {
- mesh Fluid-Mesh-Nodes;
- locations faceNodes;
- connectivity true;
- patches (interface);
-
- readData
- (
- );
-
- writeData
- (
- Temperature
- );
- };
-};
-```
-The participant `Fluid` has its read data `Heat-Flux`, which is read on the `faceCenters`, and its write data `Temperature`, which is written to the `faceNodes`. The mesh connectivity needs only to be provided in case of the `faceNodes`, using the option `connectivity true`.
+from a preCICE point of view, the simulation here is in 3D as opposed to the original case. This leads to the fact that the out-of-plane thickness of the domain is reduced clearly and it is recommended. Otherwise your face centers have a quite large distance to the face nodes, which might trigger a preCICE warning. In that case, preCICE may filter out one of the meshes, especially in parallel simulations.
-### General Notes
-Since you now define mesh connectivity on your interface, you can export your coupling interface with the tag `<export:vtk directory="preCICE-output" />` in your `precice-config.xml`.
+## Post-processing
+Have a look at the [flow-over heated-plate](tutorials-flow-over-heated-plate.html) tutorial for the general aspects of post-processing.
+Since we now defined mesh connectivity on our interface, we can export the coupling interface with the tag `<export:vtk directory="preCICE-output" />` in our `precice-config.xml`.
Visualizing these files (e.g. using ParaView) will show a triangular mesh, even though you use hexahedral meshes. This has nothing to do with your mesh and is just caused by the way the connectivity is defined in preCICE. As described above, the function `setMeshTriangles` is used to define the connectivity. Hence, every interface cell/face is represented by two triangles. The following image should give you an impression of a possible triangulated coupling mesh, which consists purely of hexahedral cells:
Note: Connectivity is defined on meshes associated with mesh nodes, which are named respectively e.g. `Fluid-Mesh-Nodes`. In this case, you could directly see the interface without applying filters by loading the `.vtk` files. In order to visualize additionally center based meshes, where no connectivity is provided, select a Glyph filter in ParaView. Furthermore, it makes a difference, on which participant the `<export...` tag is defined in your `precice-config.xml` file. Each participant exports interface meshes, which he provides or receives. The receiving participant filters out mesh parts that it does not need (for the mapping). Hence, a received mesh might look incomplete.
-### Notes on 2D Cases
-
-The geometry of the tutorial differs compared to the existing example: The out-of-plane thickness of the domain is reduced clearly and it is recommended. Otherwise your face centers have a quite large distance to the face nodes, which might trigger a preCICE warning. In that case, preCICE may filter out one of the meshes, especially in parallel simulations.
-
{% include disclaimer.html content="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." %}
From 97d5a55491cfccb701edcd4b841653a032fd8137 Mon Sep 17 00:00:00 2001
From: David Schneider <dav.schneider@tum.de>
Date: Tue, 23 Mar 2021 07:54:00 +0100
Subject: [PATCH 6/6] Update
flow-over-heated-plate-nearest-projection/README.md
Co-authored-by: Gerasimos Chourdakis <chourdak@in.tum.de>
---
flow-over-heated-plate-nearest-projection/README.md | 2 +-
1 file changed, 1 insertion(+), 1 deletion(-)
diff --git a/flow-over-heated-plate-nearest-projection/README.md b/flow-over-heated-plate-nearest-projection/README.md
index 1b9b99bcb..0dd77c0f4 100644
--- a/flow-over-heated-plate-nearest-projection/README.md
+++ b/flow-over-heated-plate-nearest-projection/README.md
@@ -56,7 +56,7 @@ All further changes follow from this interface splitting. Have a look in the giv
### Notes on 2D Cases
-from a preCICE point of view, the simulation here is in 3D as opposed to the original case. This leads to the fact that the out-of-plane thickness of the domain is reduced clearly and it is recommended. Otherwise your face centers have a quite large distance to the face nodes, which might trigger a preCICE warning. In that case, preCICE may filter out one of the meshes, especially in parallel simulations.
+From the preCICE point of view, the simulation here is in 3D, as opposed to the original 2D case, as is often the case with 3D solvers (such as OpenFOAM). In such cases, we recommend keeping the out-of-plane thickness of the domain small and comparable to the in-plane cell size. Otherwise, the face centers will have a large distance to the face nodes, which might trigger a preCICE warning and preCICE may even filter out one of the meshes, especially in parallel simulations.
## Post-processing