Adaptive Mesh Refinement With a Moving Mesh using sprayDyMFoam - - PowerPoint PPT Presentation

Adaptive Mesh Refinement With a Moving Mesh using sprayDyMFoam

Andreas Nygren

Chalmers University of Technology

Division of Combustion

8-9th of December

OpenFoam Course

Andreas Nygren OpenFoam Course - December 8-9 2015

Introduction Motivation

• To properly resolve the physics, fine meshes are needed in

regions of interest.

• It is computationally expensive to make the whole mesh very

fine.

• For automotive applications moving meshes are used to model

piston movement.

Andreas Nygren OpenFoam Course - December 8-9 2015

Introduction Learning Outcomes

Today you will learn how to:

• How to combine the dynamicRefineFvMesh class with

thedynamicMotionSolverFvMesh class

• Modify sprayDyMFoam to calculate and output the gradient
• f the velocity field to be used as basis for the adaptive mesh

refinement.

• How to set-up a case with mesh motion and on-line adaptive

mesh refinement.

Andreas Nygren OpenFoam Course - December 8-9 2015

Introduction Dynamic Mesh Libraries in OpenFOAM

dynamicFvMesh

• dynamicMotionSolverFvMesh
• dynamicRefineFvMesh
• solidBodyMotionFvMesh
• dynamicInkJetFvMesh

topoChangerFvMesh

• linearValveFvMesh
• linearValveLayersFvMesh
• mixerFvMesh
• movingConeTopoFvMesh
• rawTopoChangerFvMesh

Andreas Nygren OpenFoam Course - December 8-9 2015

Introduction Dynamic Mesh Libraries in OpenFOAM

dynamicFvMesh

• dynamicMotionSolverFvMesh
• dynamicRefineFvMesh
• solidBodyMotionFvMesh
• dynamicInkJetFvMesh

topoChangerFvMesh

• linearValveFvMesh
• linearValveLayersFvMesh
• mixerFvMesh
• movingConeTopoFvMesh
• rawTopoChangerFvMesh

Focus on simple mesh motion with mesh refinement!

Andreas Nygren OpenFoam Course - December 8-9 2015

Mesh Refinement with Motion First off!

• Combine dynamicRefineFvMesh and

dynamicMotionSolverFvMesh

• Create a library for both mesh motion and refinement

Andreas Nygren OpenFoam Course - December 8-9 2015

Mesh Refinement with Motion Copy and rename

Start by copying dynamicRefineFvMesh to your own folder OF30x mkdir -p $FOAM_RUN/../src/motionRefinementFvMesh/ cd $FOAM_RUN/../src/motionRefinementFvMesh/ cp -r $FOAM_SRC/dynamicFvMesh/dynamicRefineFvMesh . mv dynamicRefineFvMesh dynamicMotionSolverRefineFvMesh cd dynamicMotionSolverRefineFvMesh mv dynamicRefineFvMesh.C dynamicMotionSolverRefineFvMesh.C mv dynamicRefineFvMesh.H dynamicMotionSolverRefineFvMesh.H

Andreas Nygren OpenFoam Course - December 8-9 2015

Mesh Refinement with Motion Renaming Inside Files

• Function calls and includes etc need to be renamed to the

new class name

• Use the sed command!

sed command

sed -i s/dynamicRefineFvMesh/dynamicMotionSolverRefineFvMesh/g dynamicMotionSolverRefineFvMesh.C sed -i s/dynamicRefineFvMesh/dynamicMotionSolverRefineFvMesh/g dynamicMotionSolverRefineFvMesh.H

• A Convenient and safe way to change the name

Andreas Nygren OpenFoam Course - December 8-9 2015

Mesh Refinement with Motion Edit dynamicMotionSolverRefineFvMesh.H

Class Declaration for motionSolver

namespace Foam { // Add Class Declaration for the Motion Solver Class class motionSolver;

Declare a pointer to the motionSolver

class dynamicMotionSolverRefineFvMesh : public dynamicFvMesh { //Add declaration for pointer to Motion Solver autoPtr<motionSolver> motionPtr_; protected:

Andreas Nygren OpenFoam Course - December 8-9 2015

Mesh Refinement with Motion Edit dynamicMotionSolverRefineFvMesh.C

Includes for the Motion Solver

#include "dynamicMotionSolverRefineFvMesh.H" #include "addToRunTimeSelectionTable.H" #include "surfaceInterpolate.H" #include "volFields.H" #include "polyTopoChange.H" #include "surfaceFields.H" #include "syncTools.H" #include "pointFields.H" #include "sigFpe.H" #include "cellSet.H" // Add the Following Includes to the Header: #include "motionSolver.H" #include "mapPolyMesh.H" #include "pointField.H" Andreas Nygren OpenFoam Course - December 8-9 2015

Mesh Refinement with Motion Edit dynamicMotionSolverRefineFvMesh.C

Pointer to the motionSolver object in the Constructor

dynamicFvMesh(io), //define a pointer to the motionSolver Object in the Constructor: motionPtr_(motionSolver::New(*this)), meshCutter_(*this), dumpLevel_(false), nRefinementIterations_(0), protectedCell_(nCells(), 0)

function call to move points

bool Foam::dynamicMotionSolverRefineFvMesh::update() { // Add a function call to the motionSolver // to move points before refinement. dynamicFvMesh::movePoints(motionPtr_->newPoints());

Andreas Nygren OpenFoam Course - December 8-9 2015

Mesh Refinement with Motion Create a Make folder

Copy the Make folder from dynamicFvMesh

cd .. cp -r $FOAM_SRC/dynamicFvMesh/Make .

Edit Make/files

dynamicMotionSolverRefineFvMesh/dynamicMotionSolverRefineFvMesh.C LIB = $(FOAM_USER_LIBBIN)/libmotionRefinementFvMesh

Andreas Nygren OpenFoam Course - December 8-9 2015

Mesh Refinement with Motion

Make/options link with dynamicFvMesh

EXE_INC = \

• I$(LIB_SRC)/triSurface/lnInclude \
• I$(LIB_SRC)/meshTools/lnInclude \
• I$(LIB_SRC)/dynamicMesh/lnInclude \
• I$(LIB_SRC)/dynamicFvMesh/lnInclude \
• I$(LIB_SRC)/finiteVolume/lnInclude

LIB_LIBS = \

• ltriSurface \
• lmeshTools \
• ldynamicMesh \
• ldynamicFvMesh \
• lfiniteVolume

Andreas Nygren OpenFoam Course - December 8-9 2015

Mesh Refinement with Motion Clean and Compile!

Make

wclean wmake

Andreas Nygren OpenFoam Course - December 8-9 2015

Mesh Refinement Based on a Gradient

• It is known that the mesh should be refined where the

gradient of a field is high.

• We can base our mesh refinement on the gradient of a field

rather than the field itself.

• We just need to calculate the gradient of the field every time

step

• An easy way of doing this is to just modify the solver

Andreas Nygren OpenFoam Course - December 8-9 2015

Mesh Refinement Based on a Gradient Copying The Files

Copy and rename sprayDyMFoam

mkdir -p $FOAM_RUN/../applications/solvers/mySprayDyMFoam cd $FOAM_RUN/../applications/solvers/mySprayDyMFoam cp $FOAM_SOLVERS/lagrangian/sprayFoam/createClouds.H . cp $FOAM_SOLVERS/lagrangian/sprayFoam/createFields.H . cp $FOAM_SOLVERS/lagrangian/sprayFoam/rhoEqn.H . cp $FOAM_SOLVERS/lagrangian/sprayFoam/UEqn.H . cp $FOAM_SOLVERS/lagrangian/sprayFoam/sprayDyMFoam/pEqn.H . cp $FOAM_SOLVERS/lagrangian/sprayFoam/sprayDyMFoam/sprayDyMFoam.C . cp -r $FOAM_SOLVERS/lagrangian/sprayFoam/sprayDyMFoam/Make . mv sprayDyMFoam.C mySprayDyMFoam.C

Andreas Nygren OpenFoam Course - December 8-9 2015

Mesh Refinement Based on a Gradient Initialize The Gradient Field

Add to createFields.H

// Initialize After U! volScalarField UGrad ( IOobject ( "UGrad", runTime.timeName(), mesh, IOobject::READ_IF_PRESENT, IOobject::AUTO_WRITE ), mag(fvc::grad(U)) );

Andreas Nygren OpenFoam Course - December 8-9 2015

Mesh Refinement Based on a Gradient Modify the Solver

Add gradient calculation

// Store momentum to set rhoUf for introduced faces. volVectorField rhoU("rhoU", rho*U); // Add the calculation of the velocity // gradient before the mesh changes UGrad = mag(fvc::grad(U)); // Do any mesh changes mesh.update();

Andreas Nygren OpenFoam Course - December 8-9 2015

Mesh Refinement Based on a Gradient Create Make/files, Make/options and compile

Make/files - Change Name

mySprayDyMFoam.C EXE = $(FOAM_USER_APPBIN)/mySprayDyMFoam

Make/options - Change the Path to Two Folders

• I$(FOAM_SOLVERS)/lagrangian/reactingParcelFoam \
• I$(FOAM_SOLVERS)/compressible/rhoPimpleFoam/rhoPimpleDyMFoam \

Clean and Compile!

wclean wmake

Andreas Nygren OpenFoam Course - December 8-9 2015

Case Set-Up Aachen-Bomb case

• Static Spray combustion

chamber

• sprayFoam tutorial case
• We can modify it to run

with dynamicMotionSolver- RefineFvMesh

Andreas Nygren OpenFoam Course - December 8-9 2015

Case Set-Up

• Download the aachenBombMotionRefine case.
• It has been modified so that the spray chamber will shrink

during run-time.

• It serve to illustrate the simultaneous mesh motion and

refinement.

• This is not a ”real spray simulation”. The mesh is to coarse.
• We will now go through the modifications and then run the

case.

Andreas Nygren OpenFoam Course - December 8-9 2015

Case Set-Up Add patches for movingWall

patches ( wall walls ( (2 6 5 1) (0 4 7 3) (0 1 5 4) (7 6 2 3) ) wall fixedWall ( (4 5 6 7) ) wall movingWall ( (0 1 2 3) ) );

Andreas Nygren OpenFoam Course - December 8-9 2015

Case Set-Up Modify inital files to correspond to new patches

boundaryField { walls { type zeroGradient; } fixedWall { type zeroGradient; } movingWall { type zeroGradient; } }

Andreas Nygren OpenFoam Course - December 8-9 2015

Case Set-Up Moving Wall velocity for U

movingWall { type movingWallVelocity; value uniform (0 0 0); }

Andreas Nygren OpenFoam Course - December 8-9 2015

Case Set-Up pointMotion

dimensions [ 0 1 -1 0 0 0 0 ]; internalField uniform 0; boundaryField { movingWall { type uniformFixedValue; uniformValue 1; value uniform 1; } walls { type slip; } fixedWall { type uniformFixedValue; uniformValue 0; value uniform 0; } }

• Special Inital File
• Prescribe velocity for mesh

points at movingWall

Andreas Nygren OpenFoam Course - December 8-9 2015

Case Set-Up dynamicMeshDict - Motion Coeffs

dynamicFvMesh dynamicMotionSolverRefineFvMesh; motionSolverLibs ( "libfvMotionSolvers.so" ); solver velocityComponentLaplacian; velocityComponentLaplacianCoeffs { component y; diffusivity inverseDistance (movingWall); }

Andreas Nygren OpenFoam Course - December 8-9 2015

Case Set-Up dynamicMeshDict - Refinement Coeffs

dynamicMotionSolverRefineFvMeshCoeffs //dynamicRefineFvMeshCoeffs { // How often to refine refineInterval 1; // Field to be refinement on field UGrad; // Refine field inbetween lower..upper lowerRefineLevel 10000; upperRefineLevel 70000; // If value < unrefineLevel unrefine unrefineLevel 1; // Have slower than 2:1 refinement nBufferLayers 1; // Refine cells only up to maxRefinement levels maxRefinement 2; // Stop refinement if maxCells reached maxCells 160000; // Flux field and corresponding velocity field. Fluxes on changed // faces get recalculated by interpolating the velocity. Use none // on surfaceScalarFields that do not need to be reinterpolated. correctFluxes ( (phi_0 U_0) (phi U)

Andreas Nygren OpenFoam Course - December 8-9 2015

Results

Figure: Inital Temperature Field and Mesh Figure: Temperature Field and Mesh after 0.006 seconds Andreas Nygren OpenFoam Course - December 8-9 2015