Uncertainty Qauntification in CFD simulations

This repository contains codes developed during my PhD at University of Groningen. The directory OpenFOAM contains applications (solvers, utilities) and src (fvOptions) compiled with version (v2106).

Stochastic Solver

Stochastic Model - algorithm and implementation Using an exiting deterministec solver pimpleFoam, a stoachastic solver based on Intrusive Polynomial Chaos (IPC) was developed in OpenFOAM called as gPCModelFormFoam. More details on this solver can be found in the following articles:

[1] Quantification and propagation of model-form uncertainties in RANS turbulence modeling via intrusive polynomial chaos. International Journal for Uncertainty Quantification. 2022

[2] Intrusive Polynomial Chaos for CFD Using OpenFOAM. Computational Science, ICCS 2020, Lecture Notes in Computer Science. Springer, Cham.

Important steps of the algorithm implemented are shown in the figure (below).

Benchmark Case - geometry, mesh and model parameters

Build instructions

The gPCModelFormFoam solver can be build (i.e. compiled like any other OpenFOAM solver) using make files.

cd OpenFOAM/v2106/applications/solvers/gPCModelFormFoam
./Allwclean # wclean
./Allwmake  # wmake

Stochatic Simulation (Run example)

The above case setup is used in section 6.1 from [1] and can be found in tutorials as periodicHill_REVF. The steps involed in setting up and running a stochastic RANS simulation for flow over Periodic Hills with a random eddy-viscoity field (REVF) are as follows:

1) Uncertainty Quantification

• After obtaining a (modeled) eddy viscosity field from a deterministic RANS simulation we can generate a Random Eddy Viscosity Field (REVF). The eigenmodes of the REVF can be obtained using a KL decomposition (expGp_gPCKLE_LogNProc.py in tutorials as periodicHill_REVF).
• For convinience we already provide these modes generated over a coarse mesh and projected onto the stochastic RANS simulation mesh. These projected modes can be located in the 0 directory as expGpCoeffs*.
• These eigenmodes will be used by the gPCModelFormFoam solver to contruct the PCE coefficients of the REVF (only at the start of the simulaiton).
• Below are the first six KL expansion modes shifted and normalized to the range of 0 (darkest) and 1 (lightest).

2) Uncertainty Propagation

• The first mode of velocity and pressure are initialized using the solution from the deterministic simulation, to speed up the convergence of the stochastic solver.

• Boundary conditions of the remaining modes are specified using 0/UQpBC.H and 0/UQUBC.H.

• The discretization schemes in system/fvSchemes and the solver settings in system/fvSolution are the same as that of the deterministic simulation.

• Solver parameters of gPCModelFormFoam are controled by system/controlDict. In this tutorial we have particularly used the following solver paramters:

  ...
  transientMode   on;    // 'off' for steady-state simulation 
  expItrMax       1;     // controls the number of explicit iterations
  Ptrunc          10;    // controls the number of modes to be solved
  ...

• The run script contains commands to run a batch job on SLURM based cluster.

  • blockMesh creartes the mesh
  • topSet sets the topology for the momentum source in system/fvOptions
  • decomposePar decomposes the domain according to system/decomposeParDict
  • foamJob -s -p gPCModelFormFoam -parallel runs gPCModelFormFoam in parallel
  • reconstructPar recontructs the solution

• The solver returns all the modes of velocity and pressure at writeInterval in system/controlDict.

• After obtaining the PCEs of velocity and pressure, further post-processing to obtain PCEs of other QoIs (like wall-shear stess) is straight-forward.

• In the figure below we have mean and variance of (a) turbulent viscosity, (b) streamwise velocity and (c) wall shear-stress at different locations in x-direction for the flow over periodic hills. Compared with deterministic (DET) and DNS results. Legend in (c) (top) applies to (a) and (b) as well.

Running on a PC/laptop

• A fairly less expensive version of this case is test_run, which can be used to test the simulation setting and can be run on a local PC/laptop.

  cd OpenFOAM/v2106/tutorials/incompressible/gPCModelFormFoam/test_run
  ./run_local
  
  

• It is assumed that OpenFOAM is installed and gPCModelFormFoam is alredy compiled before running the tutorial case(s).

Further Study

• Varying correlation length scales
• Techniques to overcome the curse of dimensionality
• Comparison between turbulence models
• Reducing uncertainty via data assimilation
• Random Reynolds-stress tensor field (RRSTF)

Please refer to [1] for detailed analysis.