Merge branch 'develop' into systemtests/add-timeout-support

Author: AdityaGupta716

changelog-entries/660.md

@@ -0,0 +1 @@
+- Added a new Partitioned Water Hammer tutorial including 1D–3D, 3D–1D, 1D–1D, and 3D–3D coupling configurations using OpenFOAM and Nutils [#660](https://github.com/precice/tutorials/pull/660) 

changelog-entries/677.md

@@ -0,0 +1 @@
+- Added a new Partitioned Pipe Multiscale tutorial including 1D–3D, 3D–1D, 1D–1D, and 3D–3D coupling configurations using OpenFOAM and Nutils [#677](https://github.com/precice/tutorials/pull/677)

partitioned-pipe-multiscale/README.md

@@ -0,0 +1,281 @@
+---
+title: Partitioned Pipe — Geometric Axial Multiscale
+keywords: OpenFOAM, Nutils, preCICE, geometric multiscale, fluid
+summary: The Partitioned Pipe — Geometric Axial Multiscale tutorial couples a 1D pipe model with a 3D CFD pipe using preCICE.
+---
+
+{% note %}
+Get the [case files of this tutorial](https://github.com/precice/tutorials/tree/develop/partitioned-pipe-multiscale), as continuously rendered here, or see the [latest released version](https://github.com/precice/tutorials/tree/master/partitioned-pipe-multiscale) (if there is already one). Read how in the [tutorials introduction](https://precice.org/tutorials.html).
+{% endnote %}
+
+## Setup
+
+We solve a simple **partitioned pipe problem** using a 1D–3D coupling approach.  
+In this tutorial, the computational domain is split into two coupled regions: a 1D pipe section and a 3D pipe section.  
+The coupling is performed using **preCICE**.
+
+In addition to the 1D–3D setup, this tutorial also includes configurations for **1D–1D** and **3D–3D** coupling.  
+These variants can be beneficial for validation studies, solver comparisons, or for investigating the influence of model dimensionality.
+
+In the following, $\mathrm{1D}$ denotes the reduced-order domain (e.g., a Nutils solver) and $\mathrm{3D}$ denotes the full 3D CFD domain (e.g., OpenFOAM).
+
+The problem consists of a straight pipe of length $L = 40 \mathrm{m}$ and diameter $D = 10 \mathrm{m}$. We partition the domain at $z_c = 20 \mathrm{m}$, where the coupling interface is located. The pipe axis is aligned with the z-axis.
+The **1D domain** solves the flow equations using Nutils, while the **3D domain** is solved using OpenFOAM.  
+Both solvers are coupled via preCICE by exchanging the **pressure** and **axial velocity** at the interface.
+
+Two coupling directions are possible:  
+
+- **1D → 3D**: The 1D solver provides the interface velocity to the 3D solver, which responds with pressure.  
+- **3D → 1D**: The 3D solver provides the velocity, and the 1D solver returns the pressure.
+
+The global outlet (end of the rightmost domain) is set to $p_{\mathrm{out}} = 0 \mathrm{Pa}$.
+
+For the **3D → 1D** coupling, the 3D inlet velocity is prescribed as a **parabolic (Poiseuille)** profile with a bulk velocity of $u_{\mathrm{in}} = 0.1 \mathrm{m/s}$
+implemented using a `codedFixedValue` boundary condition. This ensures a physically realistic velocity distribution consistent with the 1D model.
+
+For the **1D → 3D** coupling, the inlet velocity is set to $u_{\mathrm{in}} = 0.1 \mathrm{m/s}$.
+
+## Configuration
+
+preCICE configuration for the 1D-3D simulation (image generated using the [precice-config-visualizer](https://precice.org/tooling-config-visualization.html)):
+
+![preCICE configuration visualization 1D-3D](images/tutorials-partitioned-pipe-multiscale-1d3d-config.png)
+
+preCICE configuration for the 3D-1D simulation:
+
+![preCICE configuration visualization 3D-1D](images/tutorials-partitioned-pipe-multiscale-3d1d-config.png)
+
+## Available solvers
+
+- OpenFOAM (**pimpleFoam**). An incompressible/transient OpenFOAM solver. See the [OpenFOAM adapter documentation](https://precice.org/adapter-openfoam-overview.html).
+- Nutils. A Python-based finite element framework. For more information, see the [Nutils adapter documentation](https://precice.org/adapter-nutils.html)
+
+## Running the Simulation
+
+First, select which coupling you want to run. This sets the correct `precice-config.xml` symlink (by default, set to `1d3d`):
+
+```bash
+# Choose one configuration
+./setcase.sh 1d3d
+# or
+./setcase.sh 3d1d
+# or
+./setcase.sh 1d1d
+# or
+./setcase.sh 3d3d
+```
+
+Open **two terminals** and start the corresponding participants for your chosen setup.
+
+### Example A — 1D → 3D coupling
+
+Terminal 1:
+
+```bash
+cd fluid1d-left-nutils
+./run.sh
+```
+
+Terminal 2:
+
+```bash
+cd fluid3d-right-openfoam
+./run.sh
+```
+
+### Example B — 3D → 1D coupling
+
+Run `./setcase.sh 3d1d` and then navigate to the respective directories.
+
+Terminal 1:
+
+```bash
+cd fluid3d-left-openfoam
+./run.sh
+```
+
+Terminal 2:
+
+```bash
+cd fluid1d-right-nutils
+./run.sh
+```
+
+## Visualization
+
+The output of the coupled simulation is written into the folders `fluid1d-left-nutils`, `fluid1d-right-nutils`, `fluid3d-left-openfoam`, and `fluid3d-right-openfoam`, depending on which coupling direction (`1d3d` or `3d1d`) you selected.
+
+### 3D domain (OpenFOAM)
+
+For the 3D participant, all simulation results are stored in the time directories inside the respective case folder (e.g., `fluid3d-right-openfoam/`).  
+You can visualize the flow field and pressure distribution using **ParaView** by opening the case file:
+
+```bash
+paraview fluid3d-right-openfoam/fluid3d-right-openfoam.foam
+```
+
+or, for the left domain if applicable:
+
+```bash
+paraview fluid3d-left-openfoam/fluid3d-left-openfoam.foam
+```
+
+Typical fields to inspect include:  
+
+- `p` – pressure
+- `U` – velocity
+
+We also record pressure and velocity at fixed points each time step using the OpenFOAM `probes` function object.
+
+**Probe setup (excerpt):**
+
+```c
+#includeEtc "caseDicts/postProcessing/probes/probes.cfg"
+
+fields (p U);
+probeLocations
+(
+    (0 0 20)
+    (0 0 40)
+);
+// For the left 3D domain use instead:
+// probeLocations ((0 0 0) (0 0 20));
+```
+
+**Output location:**  
+
+- `fluid3d-right-openfoam/postProcessing/probes/0/p`  
+- `fluid3d-right-openfoam/postProcessing/probes/0/U`
+
+In addition to point probes, the 3D participant samples the **axial pressure distribution** along the pipe centerline using `sampleDict`. This provides the spatial pressure variation along the pipe and allows direct comparison with the 1D solution at the latest time step.
+
+The tutorial includes a `sampleDict` in the 3D cases:
+
+- `fluid3d-left-openfoam/system/sampleDict`  
+- `fluid3d-right-openfoam/system/sampleDict`  
+
+**sampleDict (excerpt):**
+
+```cpp
+FoamFile
+{
+    version     2.0;
+    format      ascii;
+    class       dictionary;
+    location    "system";
+    object      sampleDict;
+}
+
+type            sets;
+libs            ("libsampling.so");
+
+setFormat       raw;
+
+sets
+(
+    centerline
+    {
+        type    uniform;
+        axis    z;
+        start   (0 0 0);
+        end     (0 0 20);
+        nPoints 200;
+    }
+);
+
+fields (p);
+```
+
+The sampling is executed automatically during the run.
+
+**Output location:**
+
+```text
+postProcessing/sampleDict/<latestTime>/centerline_p.xy
+```
+
+The file contains two columns:
+
+1. axial coordinate `z`  
+2. pressure `p`
+
+### 1D domain (Nutils)
+
+The 1D solver writes a `probes.txt` with semicolon-separated time series:
+
+```text
+time; p_in; u_in; p_out; u_out; p_mid; u_mid
+```
+
+where:
+
+- `p_in`, `u_in` → pressure and velocity at the inlet of the 1D domain  
+- `p_out`, `u_out` → pressure and velocity at the outlet of the 1D domain  
+- `p_mid`, `u_mid` → pressure and velocity at the midpoint of the 1D domain
+
+The 1D solver also writes a `final_fields.txt` with space-separated values:
+
+```text
+x u p
+```
+
+They correspond to the axial position, velocity and pressure at the last time-step, i.e., at $t = 5 \mathrm{s}$.
+
+### Plotting axial pressure distribution (optional)
+
+To reproduce the axial pressure distribution shown in the figure below, a helper script is provided:
+
+```bash
+python plot-pressure-distribution.py
+```
+
+By default, the script uses the `1d3d` case.
+
+You can also specify the coupling configuration explicitly:
+
+```bash
+python plot-pressure-distribution.py 1d3d
+```
+
+```bash
+python plot-pressure-distribution.py 3d1d
+```
+
+```bash
+python plot-pressure-distribution.py 1d1d
+```
+
+```bash
+python plot-pressure-distribution.py 3d3d
+```
+
+Allowed cases are:
+
+- `1d3d`
+- `3d1d`
+- `1d1d`
+- `3d3d`
+
+Depending on the selected case, the script reads:
+
+- `final_fields.txt` from the 1D Nutils solver
+- `centerline_p.xy` from the 3D OpenFOAM participant
+
+and combines both datasets to plot the pressure distribution along the coupled pipe.
+
+By default, the figures are saved to:
+
+```text
+images/pressure_distribution_<case>.png
+```
+
+### Example visualization
+
+![Pressure distribution along the main axis in the 3D-1D Coupled Pipe](images/tutorials-partitioned-pipe-multiscale-3d1d-pressure-distribution.png)
+
+**Pressure along the pipe centerline.** The pressure decreases nearly linearly from **≈12.8 Pa** at the 3D inlet to **0 Pa** at the 1D outlet, consistent with steady, laminar Poiseuille flow. The 3D (0–20 m) and 1D (20–40 m) sections connect smoothly at the coupling interface.
+
+![Velocity at the 3D coupling interface in the 3D-1D Coupled Pipe](images/tutorials-partitioned-pipe-multiscale-3d1d-velocityProfileInterface3d.png)
+
+**Parabolic velocity profile at the 3D outlet / coupling interface (z = 20 m).**  
+The profile is Poiseuille-like with a bulk velocity of **0.1 m/s**; consequently the **centerline velocity is ≈ 0.2 m/s** (≈ 2 × bulk) and vanishes at the wall (no-slip). This is the velocity state at the interface used for coupling to the 1D domain.

partitioned-pipe-multiscale/clean-tutorial.sh

@@ -0,0 +1,11 @@
+#!/usr/bin/env sh
+set -e -u
+
+# shellcheck disable=SC1091
+. ../tools/cleaning-tools.sh
+
+clean_tutorial .
+clean_precice_logs .
+rm -fv ./*.log
+rm -fv ./*.vtu
+

partitioned-pipe-multiscale/fluid1d-left-nutils/.gitignore

@@ -0,0 +1,2 @@
+probes.txt
+final_fields.txt

partitioned-pipe-multiscale/fluid1d-left-nutils/clean.sh

@@ -0,0 +1,10 @@
+#!/usr/bin/env sh
+set -e -u
+
+. ../../tools/cleaning-tools.sh
+
+rm -f ./results/Fluid1D_*
+rm -f ./probes.txt
+rm -f ./final_fields.txt
+clean_precice_logs .
+clean_case_logs .

partitioned-pipe-multiscale/fluid1d-left-nutils/requirements.txt

@@ -0,0 +1,5 @@
+setuptools # required by nutils
+nutils==9
+numpy >1, <2
+pyprecice~=3.0
+matplotlib

partitioned-pipe-multiscale/fluid1d-left-nutils/run.sh

@@ -0,0 +1,13 @@
+#!/usr/bin/env bash
+set -e -u
+
+. ../../tools/log.sh
+exec > >(tee --append "$LOGFILE") 2>&1
+
+python3 -m venv .venv
+. .venv/bin/activate
+pip install -r requirements.txt && pip freeze > pip-installed-packages.log
+
+NUTILS_RICHOUTPUT=no python3 ../solver-fluid1d-nutils/Fluid1D.py side=Left
+
+close_log

partitioned-pipe-multiscale/fluid1d-right-nutils/.gitignore

@@ -0,0 +1,2 @@
+probes.txt
+final_fields.txt

partitioned-pipe-multiscale/fluid1d-right-nutils/clean.sh

@@ -0,0 +1,10 @@
+#!/usr/bin/env sh
+set -e -u
+
+. ../../tools/cleaning-tools.sh
+
+rm -f ./results/Fluid1D_*
+rm -f ./probes.txt
+rm -f ./final_fields.txt
+clean_precice_logs .
+clean_case_logs .