1. OpenFOAM 14 Tutorial Workflow for pitzDailySteady

The official OpenFOAM Foundation Ubuntu guide uses pitzDailySteady as a first steady-state example and runs it with blockMesh, foamRun, and paraFoam. In this tutorial we keep that same core workflow, but expose one extra step: checkMesh. That lets us verify the grid before solving instead of treating meshing and solution as one opaque operation.

The case also includes an Allrun script. It is useful as an automated shortcut, but the main learning path below runs the important applications separately so each stage can be inspected.

2. Open the Case and Activate OpenFOAM 14

In the OceanTechReview setup, the copied Foundation tutorials are stored under:

~/OpenFOAM/<username>-14/run/tutorials

Navigate to incompressibleFluid/pitzDailySteady in the Ubuntu file manager, choose Open in Terminal, and activate the Foundation 14 shell:

of14

The of14 command is the isolated launcher created in the previous installation article; it is not a stock OpenFOAM command. If you use the standard single-version Foundation setup instead, activate the environment with:

source /opt/openfoam14/etc/bashrc

The isolated launcher used in this series preserves the directory from which it is started. That matters for day-to-day CFD work: you can browse to any case, open a terminal there, run of14, and remain in the case instead of being redirected to a generic run directory.

Verify the version, current directory, and top-level case contents:

foamVersion

pwd

ls -1

A clean starting case contains the familiar OpenFOAM directories 0, constant, and system, plus the tutorial automation script Allrun. Seeing OpenFOAM-14 from foamVersion confirms that the commands in the next sections will use the intended Foundation release.

3. Read the pitzDailySteady Case Structure

Before running a first OpenFOAM simulation, it is worth understanding what the main directories represent. OpenFOAM cases are intentionally file-based: the physical fields, models, numerical controls, and run settings live in plain-text dictionaries that can be inspected and version-controlled.

The 0 Directory: Initial and Boundary Fields

The 0 directory contains the initial and boundary conditions for the primary solution fields. In this incompressible turbulent case, that includes velocity U, pressure p, and the turbulence quantities required by the selected model.

The constant Directory: Physical and Mesh Data

The constant directory stores time-independent physical configuration and, after meshing, the generated polyMesh database. This is where OpenFOAM keeps the mesh connectivity and boundary-patch definitions used by the solver.

The system Directory: Numerics and Run Control

The system directory controls the calculation. The controlDict selects the solver module and run behaviour, fvSchemes defines discretisation schemes, and fvSolution contains linear-solver and SIMPLE/PIMPLE controls. For this case, foamRun reads the solver entry in controlDict and loads the corresponding incompressibleFluid module.

You can inspect the automation before running it:

sed -n '1,120p' Allrun

4. Understand the Backward-Facing-Step Flow

The physics are simple enough for a first CFD tutorial but still meaningful. Flow enters through the narrower upstream section and reaches a sudden expansion at the backward-facing step. The boundary layer can no longer follow the sharp corner, so the flow separates and creates a low-velocity recirculation region along the lower wall.

Farther downstream, the separated shear layer approaches the lower wall again and the main flow reattaches. This combination of acceleration, separation, reverse flow, and reattachment makes the case useful for learning how a CFD result should be interpreted instead of merely checking whether a solver reached End.

The tutorial is effectively two-dimensional: the mesh has only one cell through the thin spanwise direction and the frontAndBack patch removes that direction from the solution. That keeps the computational cost low while preserving the essential separated-flow behaviour in the streamwise plane.

The generated mesh has a bounding box from x = -0.0206 m to x = 0.29 m and from y = -0.0254 m to y = 0.0254 m. In other words, the geometry includes a 20.6 mm upstream section and extends 290 mm downstream of the step, with a full downstream height of 50.8 mm.

5. Generate and Check the Mesh

The Allrun script shows the exact mesh dictionary used by this case. To reproduce that step manually, run:

blockMesh -dict "$FOAM_TUTORIALS/resources/blockMesh/pitzDaily"

The mesh generated during this run contained 12,225 cells, all of them hexahedra. The five boundary patches were inlet, outlet, upperWall, lowerWall, and frontAndBack.

Before solving, check the mesh:

checkMesh

The mesh passed the standard checks with Mesh OK. The reported maximum non-orthogonality was approximately 5.95°, the maximum skewness was about 0.261, and the maximum aspect ratio was about 8.14. For this tutorial mesh, those values are comfortably within a range that allows us to proceed to the solution.

These numbers are not universal acceptance limits for every CFD project. Mesh quality must always be judged together with the discretisation, solver robustness, local refinement needs, and the quantities of interest. Here they simply confirm that the untouched reference mesh is behaving as expected before we move on to the solver.

Open the case in ParaView:

paraFoam

6. What the Core Case Files Control

At this point the case has a valid mesh, but it is useful to connect the directory structure with what the solver is about to do. The table below summarises the parts of pitzDailySteady that matter most in this first OpenFOAM 14 simulation.

For a first run, you do not need to edit these dictionaries. The value of reading them now is conceptual: when you later change a boundary condition, turbulence model, scheme, or convergence tolerance, you will know which part of the case owns that decision.

One item is especially useful to remember for later tutorials: fvSolution contains the SIMPLE controls and the residualControl criteria that determine when this steady-state solution is allowed to stop. The solver does not terminate merely because a fixed number of iterations has been reached; it stops once the configured convergence criteria are satisfied.

7. Run the Simulation with foamRun or Allrun

With the mesh checked, run the solver directly from the case directory:

foamRun

This is the clearest command for the manual workflow because the simulation progress is printed directly in the terminal. The OpenFOAM v14 backward-facing-step user guide explains that foamRun loads the solver module from the solver entry in controlDict and reports the residuals for each equation as the solution advances.

The case also provides Allrun. Its essential commands are:

. $WM_PROJECT_DIR/bin/tools/RunFunctions
runApplication blockMesh -dict $FOAM_TUTORIALS/resources/blockMesh/pitzDaily
runApplication foamRun

Therefore the shortcut is simply:

./Allrun

When Allrun calls runApplication, the tutorial helper writes application output to log files such as log.blockMesh and log.foamRun. You do not need to source RunFunctions manually before executing ./Allrun; the script already does that itself.

If you prefer the manual workflow but still want a persistent solver log, you can also use foamRun | tee log.foamRun. That preserves the live terminal output while writing the same text to a file for later inspection.

8. Verify SIMPLE Convergence from the Solver Log

Solver completion is not the same thing as numerical convergence. The useful evidence is in the residual history and the termination message. If the case was run with Allrun, inspect the end of the log:

tail -n 20 log.foamRun

In the final recorded iteration, the initial residuals were approximately 1.21e-4 for Ux, 9.96e-4 for Uy, 1.34e-3 for p, 1.38e-4 for epsilon, and 2.21e-4 for k. The exact intermediate values are less important than the overall pattern: the equations continue to reduce their residuals until the SIMPLE residual controls are met.

The run also executed the case’s streamline post-processing function, reporting 10 seeded particles and 12,040 sampled locations before the final End message. That gives us both a converged solution and post-processing data to inspect.

9. View Velocity and Recirculation in ParaView

Open the solved case in ParaView with:

paraFoam

Select the final solution state, choose U as the colouring field, and display its Magnitude. A Surface representation gives a clean view of the velocity distribution. Use Rescale to Data Range so the colour legend reflects the solved field rather than an earlier display range. The hero image at the top of this article shows the converged velocity-magnitude field from this run.

For a streamline view, apply Stream Tracer to the case, use U as the vector field, and seed lines through the separated region. The exact seed density is a display choice rather than a change to the CFD solution; the purpose is to make the reverse-flow path behind the step visually readable.

What the First Simulation Has Demonstrated

This one tutorial has already introduced the full OpenFOAM workflow: activate the correct environment, inspect a case, generate a mesh, verify mesh quality, run a solver, judge convergence from residuals, and post-process a physically meaningful flow feature. That sequence is far more transferable to Marine CFD than memorising a single tutorial command.

Common First-Run Problems

foamRun: command not found: the OpenFOAM 14 environment is not active. Enter the Foundation shell first with of14 in this series, or source /opt/openfoam14/etc/bashrc in a standard setup.

foamRUN: command not found: Linux commands are case-sensitive. The correct application name is foamRun, with only the R capitalised.

Mesh files are missing: run blockMesh -dict "$FOAM_TUTORIALS/resources/blockMesh/pitzDaily" before launching foamRun.

log.foamRun does not exist: a direct foamRun command writes progress to the terminal. The log.foamRun file is created when the tutorial runs the application through runApplication, such as with ./Allrun.

ParaView reports an xcb/display error on Ubuntu Wayland: use the corrected graphical-session handling described in the OpenFOAM on Ubuntu 24.04 installation guide . In the OceanTechReview isolated shell, Qt is configured to use the Wayland backend when a Wayland session is active.