Tutorial

OpenFOAM CFD Tutorial

Mesh a fluid domain, assign OpenFOAM patches, and inspect CFD results

Overview

This tutorial walks through a real OpenFOAM CFD example in confBuild. The screenshots were captured from the browser on 2026-06-21 using an example project named OpenFOAM Step Duct Tutorial Example, based on the OpenFOAM pitzDaily backward-facing step duct.

Time

About 20 minutes for a prepared model with clear inlet, outlet, and wall faces

Example mesh

blockMesh and checkMesh produced 25,012 points and 12,225 cells

Example result

simpleFoam reached time 20 with a 0.317% inlet/outlet flow-balance error

Example artifact

Case: OpenFOAM pitzDaily step duct, steady incompressible flow.
Commands completed: blockMesh, checkMesh, simpleFoam, and foamToVTK.
Velocity summary: mean 5.496 m/s, max 11.171 m/s. Pressure range: -9.937 Pa to 19.424 Pa.
Result loaded in confBuild as a completed CFD task with VTU field visualization.

Step 1: Open the real step-duct example

For CFD, the mesh represents the fluid volume, not the solid part. In this example the editor is loaded with a step-duct fluid domain, OpenFOAM solver settings, a 10 m/s inlet velocity, a 0 Pa outlet pressure, and named boundary roles for inlet, outlet, and no-slip walls.

Real confBuild browser screenshot of the OpenFOAM step duct example inputs

This is the actual browser screenshot from the example project, not a mockup. It shows the source setup before reviewing mesh and solver output.

Before you mesh

Use one closed volume for the region where the fluid should flow.
Name or identify the inlet, outlet, and wall surfaces clearly.
For thin 2D-style CFD, keep the front and back faces available as empty patches.
Start simple. Run the first case on a coarse or medium mesh before adding local refinements.

Step 2: Check mesh and face-group readiness

Open the mesh/load setup and confirm that the generated mesh exposes usable face groups. CFD boundary conditions need mesh metadata, not only visible geometry. If no groups appear in this panel, remesh with face-group output or provide OpenFOAM mesh artifacts with explicit patch roles.

Real confBuild Mesh and Loads panel showing face-group readiness for CFD setup

The screenshot is a real Mesh & Loads state. It documents the face-group gate before boundary assignment rather than pretending that every mesh is already ready.

Meshing checks

The selected object should be the flow volume, not an obstacle solid.
Face groups should survive mesh generation so CFD boundary conditions can reference them later.
For the tutorial example, the OpenFOAM case itself defines the patches: inlet, outlet, wall patches, and paired empty front/back patches.
Local refinements and boundary layers should be added only where they improve the intended result.

Step 3: Assign OpenFOAM regions and boundaries

Switch to the simulation setup and use the CFD flow path. The volume region becomes the OpenFOAM fluid region, while face groups become OpenFOAM boundary patches such as inlet, outlet, wall, symmetry, far_field, or empty.

Minimum boundary setup

At least one inlet or far-field patch should define a non-zero flow velocity.
An outlet or pressure-reference patch should let the pressure field close cleanly.
Wall patches should cover solid surfaces that the flow touches.
For 2D setups, the thin front/back faces should use empty.
In the captured example, upperWall and lowerWall are no-slip walls and frontAndBack uses empty.

Step 4: Run OpenFOAM

When the setup is complete, confBuild creates an OpenFOAM case from the mesh and boundary metadata. In this captured example, the OpenFOAM runner completed blockMesh, checkMesh, simpleFoam, and foamToVTK, then exported the velocity field from internal.vtu.

OpenFOAM solver run state in the simulation panel

This image is the actual OpenFOAM postprocessing preview from the tutorial run. checkMesh is still the gate before trusting solver output.

What happens in the runner

UNV meshes are converted with ideasUnvToFoam; MSH meshes are converted with gmshToFoam.
checkMesh validates topology and quality before the solver starts.
Steady incompressible cases use simpleFoam; transient incompressible cases use pimpleFoam.
Completed cases are exported with foamToVTK for visualization.
The example mesh passed with max non-orthogonality 5.95 degrees and max skew 0.261.

Step 5: Review the CFD result

After the solver completes, inspect both the field visualization and the numerical summary. A clean result should show the requested field, a passed mesh-quality state, reasonable residual behavior, and a low flow-balance error.

OpenFOAM CFD result summary and velocity field preview

The result screenshot is loaded from the real completed CFD task. It shows a 5.07e-4 m3/s total flow and 0.317% balance error.

Result review checklist

Check the displayed field, usually velocity magnitude or pressure.
Review OpenFOAM mesh status and mesh-quality warnings first.
Compare inlet and outlet flow totals to catch missing or duplicated patches.
Inspect residuals and solver steps before trusting detailed local values.
For this run, simpleFoam completed 20 solver steps at time 20.

Supported OpenFOAM scope

The current workflow focuses on practical incompressible CFD cases that can be prepared from editor geometry and mesh metadata.

Ready 3D incompressible flow Steady or transient cases with fluid volume meshes

Ready Thin 2D flow Use paired empty patches on the thin faces

Ready Laminar, k-epsilon, k-omega SST Select the turbulence model in the CFD setup

Ready Inlet, outlet, wall, symmetry, far-field patches Boundary roles are mapped from face groups

Not yet Compressible, porous, rotating, dynamic-mesh, heat-transfer, or species cases Keep these outside this editor workflow for now

Troubleshooting

No face groups appear

Regenerate the mesh and confirm that the selected object is the fluid domain. CFD boundaries need mesh metadata, not just visible faces.

`checkMesh` fails

Simplify tiny geometry, adjust mesh fineness, and reduce sliver faces before changing solver settings.

Solver setup is blocked

Check for a fluid region, non-zero inlet or far-field velocity, one pressure outlet or reference, and no duplicate patch assignments.

2D case fails

Make sure the thin front and back patches are assigned as empty and the case is configured as a 2D CFD setup.

Next steps

After the first valid run, refine only the parts of the workflow that affect the result you care about.

Use FEM Mesh Generation to review mesh fineness, element sizing, and face-group behavior.
Use FEM Simulation to understand the broader simulation workspace.
Run at least one mesh-refinement comparison before using CFD values for engineering decisions.

Back to Documentation