CFD_Workflow_Detailed_Report

CFD Workflow for Airflow Simulation Around a Pipe (Detailed)

Overview

This report documents the end-to-end CFD workflow used to simulate steady incompressible airflow around a pipe inside a rectangular domain.

1) Geometry Creation (Fusion 360)

The CAD workflow was:

• Create the pipe solid.
• Create a surrounding box representing the external air domain.
• Subtract the pipe from the box to obtain the fluid volume.

This produced the computational domain for OpenFOAM, where the pipe behaves as an internal obstacle.

---

2) Geometry Export and Boundary Grouping (Salome)

Because STL export does not preserve CAD face metadata, boundary zones were rebuilt in Salome by creating surface groups:

• inlet
• outlet
• walls

These groups were exported as STL surfaces and used by snappyHexMesh.

3) Mesh Generation in OpenFOAM

Meshing used:

• blockMesh for background mesh
• snappyHexMesh -overwrite for geometry fitting/refinement
• checkMesh for mesh quality verification

3.1 Background mesh (blockMeshDict)

• Domain bounds (m):
  • min = (-0.08 -0.05 -0.01)
  • max = (0.02 0.07 0.09)
• Base cell counts: (20 20 20)
• Grading: simpleGrading (1 1 1)

This was chosen as a moderate base resolution that remains stable on 16 GB RAM.

3.2 Snappy settings (snappyHexMeshDict)

Final robust settings:

• castellatedMesh true;
• snap false;
• addLayers false;

Key memory-control parameters:

• maxLocalCells 120000;
• maxGlobalCells 250000;
• nCellsBetweenLevels 2;
• minRefinementCells 10;
• maxLoadUnbalance 0.10;

Surface refinement:

• inlet level (2 2);
• outlet level (2 2);
• walls level (2 2);
• resolveFeatureAngle 60;

Region refinement:

• refinementBox mode inside;
• refinementBox level 1;

Robust geometry selection:

• insidePoint (-0.03 0 0);

3.3 Why these values were selected

Earlier runs with stronger refinement and larger effective feature growth caused excessive memory use and froze the machine. The final settings above were selected to:

• preserve resolution near surfaces,
• cap global mesh growth hard,
• avoid expensive snapping/layer operations initially,
• guarantee reproducible runtime on a 16 GB system.

3.4 Final mesh quality (checkMesh)

Final mesh statistics:

• Cells: 116574
• Faces: 382163
• Points: 149188
• Boundary patches: 3

Patch topology in final mesh:

• box (wall): 1968 faces
• outlet (patch): 5032 faces
• walls (wall): 32952 faces

Quality highlights:

• Max non-orthogonality: 27.5052 (OK)
• Max skewness: 0.333333 (OK)
• Max aspect ratio: 1.2
• Result: Mesh OK

---

4) Simulation Setup (simpleFoam)

Steady incompressible RANS simulation in OpenFOAM 11.

4.1 Solver control (system/controlDict)

• application simpleFoam;
• startTime 0;
• endTime 500;
• deltaT 1; (iteration counter for steady solver)
• writeInterval 500; (write only final time)

4.2 Turbulence and fluid properties

constant/momentumTransport:

• simulationType RAS;
• model kOmegaSST;
• turbulence on;

constant/physicalProperties:

• viscosityModel constant;
• nu = 1.5e-05 m2/s

4.3 Boundary conditions used

Note: due to final snappy patching, the solved mesh uses box, outlet, and walls.

Velocity U (0/U)

• Internal field: uniform (5 0 0) m/s
• box: fixedValue (5 0 0)
• outlet: inletOutlet, inletValue (0 0 0)
• walls: noSlip

Pressure p (0/p)

• Internal field: uniform 0
• box: zeroGradient
• outlet: fixedValue 0
• walls: zeroGradient

Turbulence fields

k (0/k):

• Internal: 0.1
• box: fixedValue 0.1
• outlet: inletOutlet with inletValue 0.1
• walls: kqRWallFunction

omega (0/omega):

• Internal: 10
• box: fixedValue 10
• outlet: inletOutlet with inletValue 10
• walls: omegaWallFunction

nut (0/nut):

• Internal: 0
• box/outlet: calculated
• walls: nutkWallFunction

4.4 Numerics

fvSchemes:

• Steady state time discretization
• Bounded upwind for k and omega
• linearUpwindV grad(U) for momentum convection

fvSolution:

• Pressure: GAMG
• U/k/omega: smoothSolver + GaussSeidel
• SIMPLE with nNonOrthogonalCorrectors 0, consistent yes
• Relaxation: U 0.9, k 0.7, omega 0.7

---

5) Run Execution and Troubleshooting

Run command:

simpleFoam

OpenFOAM 11 internally redirects this to:

foamRun -solver incompressibleFluid

This is expected behavior in current OpenFOAM versions.

Run completed successfully to Time = 500 with exit code 0.

Observed during run:

• Stable residual progression
• Occasional bounding k messages (small local clipping), but no divergence
• Successful final write of solution fields at time 500

---

6) Post-Processing Verification (Numerical)

To confirm the solution is physically non-trivial (not just mesh), scalar checks were run at time 500:

• volAverage(U) = (4.89468 -0.00457188 -8.83707e-05)
• volAverage(p) = -24.3051
• cellMin(U) = (-33.875 -30.6823 -33.3505)
• cellMax(U) = (15.7593 22.5352 23.8255)
• cellMin(p) = -375.458
• cellMax(p) = 464.906

These values confirm computed flow and pressure gradients are present in the solved field.

---

7) ParaView Workflow Notes

If only a plain box appears in ParaView, common causes are:

• Time slider left at 0 instead of 500
• internalMesh disabled in OpenFOAM reader
• Coloring left on Solid Color instead of U, p, etc.

---

Tools Used

• Fusion 360 (CAD)
• Salome (surface grouping)
• OpenFOAM 11:
  • blockMesh
  • snappyHexMesh
  • checkMesh
  • simpleFoam (redirected to foamRun -solver incompressibleFluid)
• ParaView

---

Key Learnings

• STL-based workflows require explicit boundary group reconstruction.
• Mesh RAM usage is dominated by refinement controls; hard cell limits are essential on limited-memory hardware.
• Snapping and layers are useful but should be introduced after a stable baseline mesh exists.
• Always verify solved fields numerically (volAverage, min/max), not only visually.

---

Conclusion

A complete and stable CFD workflow was executed from CAD to converged steady-state solution and visualization. The final configuration balances mesh quality and computational robustness for a 16 GB workstation, while producing valid, non-uniform flow and pressure fields around the pipe.