Convective Heat transfer in a vertical slot for the course CFD with OpenSource Software

Transcription

1 for the course CFD with OpenSource Software Applied Mechanics/Fluid Dynamics, Chalmers University of Technology, Gothenburg, Sweden December 10, 2016 December 10, /

2 Contents 1 Introduction 2 buoyantboussinesqsimplefoam Solver Description Viscosity Models New viscosity Model Test case 3 buoyantsimplefoam Solver Description Test case December 10, /

3 Natural Convection 2D Natural convection in a vertical slot with two walls at different temperatures. The fluid rises along hot wall, turns at top, sinks down along cold wall and turns again. This forms unicellular motion In the current project, simulations are carried out on the vertical slot of dimensions 300mm high and 15mm wide. December 10, /

4 Overview Description of solver buoyantboussinesqsimplefoam. Description of Viscosity Models. Implementation of new Viscosity model. Test Case using buoyantboussinesqsimplefoam and new viscosity model. Description of buoyantsimplefoam solver. Test case using buoyantsimplefoam. December 10, /

5 buoyantboussinesqsimplefoam-solver Description Solver Organization The solver has following directories buoyantboussinesqsimplefoam.c createfields.h Make files options peqn.h readtransportproperties.h TEqn.H UEqn.H December 10, /

6 buoyantboussinesqsimplefoam-solver Description buoyantboussinesqsimplefoam.c while (simple.loop()) { { #include "UEqn.H" #include "TEqn.H" #include "peqn.h" } laminartransport.correct(); turbulence->correct(); runtime.write(); } December 10, /

7 buoyantboussinesqsimplefoam-solver Description createfields.h Creates Pressure(P rgh ), Velocity(U) and Temperature(T) fields Transport and turbulence properties. Density treated as ρ = 1 β(t T ref ). Turbulent thermal diffusivity (alphat). Dynamic Pressure is treated as p = ρ.g + p rgh Acceleration due to gravity(g) and body force(gh). December 10, /

8 buoyantboussinesqsimplefoam-solver Description UEqn.H: (φu) + U t.(ν eff U).(ν eff ( U)T ) = ( ρ)gh p rgh where ν eff = ν + ν t TEqn.H:.(φT ).α eff T = S radiation + S T Where, α eff = νt pr t + ν pr, S radiation and S T are source terms due to radiation and user defined source term respectively. December 10, /

9 buoyantboussinesqsimplefoam-solver Description PEqn.H: The boundary flux is solved as: φ g = rauf gh ρ Using the boundary flux, the pressure is solved using equation:.rauf p rgh =.φ g Where rauf is 1/U.Eqn.A() interpolated from volume field to face field. The pressure is then calculated as p = p rgh + ρ k gh. Finally velocity is corrected using the updated flux and relaxed pressure. December 10, /

10 Viscosity Model Viscosity models in OpenFoam viscositymodel is a base class. There are five models as derived classes. BirdCarreu CrossPowerLaw HerschelBulkley Newtonian powerlaw December 10, /

11 Viscosity Model Link between transportmodel, turbulencemodel and viscositymodel TransportModel class is the base class for all the turbulence models. singlephasetransportmodel reads the viscosity nu, corrects it and fetches it when it is called in the turbulencemodel class singlephasetransportmodel is a derived class of +viscositymodel. It has a pointer viscositymodelptr which is private member data. class singlephasetransportmodel : public IOdictionary, public transportmodel { // Private Data autoptr<viscositymodel> viscositymodelptr_; December 10, /

12 Viscosity Model The member function nu returns the value of viscosity read from viscositymodel and the member function correct corrects the viscosity Foam::tmp<Foam::volScalarField> Foam::singlePhaseTransportModel::nu() const { return viscositymodelptr_->nu(); } void Foam::singlePhaseTransportModel::correct() { viscositymodelptr_->correct(); } The class turbulencemodel has a private member data transportmodel which returns the value of nu as a volume scalar field. December 10, /

13 New Viscosity Model New Viscosity model Viscosity is function of strain rate in non Newtonian fluids. OpenFoam has four non Newtonian viscosity models. Newtonian model assumes constant viscosity. But viscosity is function of temperature in Newtonian fluids. New model is based on power law. It can be applied to both Newtonian and non Newtonian fluids. Temperature dependency of viscosity has been added based on Vogel s law. ν = k. γ (n 1) = exp(a + For Newtonian fluids, n = 1. B T + C ) γ(n 1) December 10, /

14 New Viscosity Model Steps for new viscosity model Copy powerlaw folder from $FOAM_SRC/transportModels/incompressible/viscosityModels. Copy Make from $FOAM_SRC/transportModels/incompressible/Make Modify the name and path of the library in the files directory and add necessary lninclude files in options directory Include temperature based viscosity law in powerlaw.c Add additional private data members in powerlaw.h Replace powerlaw by new name templaw in all the above files and also rename the.c and.h files. Compile by wmake libso December 10, /

15 Test Case Test Case The already available tutorial hotroom is used to implement the case of verticalslot. M esh Generation: The blockmeshdict file in system directory has to be modified as per required geometry. blockmesh command is used for mesh generation. The mesh has four patches of type wall namely hot, cold and topandbottom. The frontandback has the empty patches. December 10, /

16 Test Case Boundary Conditions : The 0/ directory has eight directories. alphat, k, epsilon, nut, p_rgh, p, U and T. These files have to be modified since the patches of our mesh is different from that of the default tutorial. Internal Field uniform (0,0,0) boundaryfield hot noslip Velocity Boundary condition cold noslip frontandback empty topandbottom noslip December 10, /

17 Test Case Temperature Boundary condition Internal Field fixedvalue 298 boundaryfield hot 323 cold 273 frontandback empty topandbottom zerogradient Two additional files v2 and f have to be created for implementing v2f turbulence model. The dimensions of v2 is m 2 /s 2 and f is 1/s and v2wallfunction and fwallfunction are used at walls respectively. December 10, /

18 Test Case constant/transportproperties transportmodel templaw; templawcoeffs { m m [ ] 1; A A [ ] -2.2; B B [ ] 812.9; C C [ ] -140; n n [ ] 1; numin numin [ ] 5e-6; numax numax [ ] 5.5e-5; } The turbulence model has to be changed from kepsilon to v2f in constant/turbulenceproperties. December 10, /

19 Test Case Solution Control Add the following in system/controldict libs ( "libusertemplaw.so" ); Add the following in divschemes in system/fvschemes div(phi,v2) div(phi,f) bounded Gauss upwind; bounded Gauss upwind; December 10, /

20 Test Case Solution Control Adding a solver for f under solvers section in system/fvsolution f { } solver PCG; preconditioner DIC; tolerance 1e-5; reltol 0.1; Replace (k epsilon R) as (k epsilon v2 f) under SIMPLE and relaxationfactor in system/fvsolution. December 10, /

21 Test Case Results The case can be run using buoyantboussinesqsimplefoam. The results can be checked using parafoam. Temperature Viscosity December 10, /

22 Test Case Results Velocity December 10, /

23 Solver Description buoyantsimplefoam /buoyantsimplefoam buoyantsimplefoam.c createfieldrefs.h createfields.h EEqn.H Make files options peqn.h UEqn.H December 10, /

24 Solver Description CreateFields.H In createfields, class rhothermo.h is used which is a thermophysical model belonging to thermophysical model library. The temperature is not solved directly, thus it is not created as a filed in createfields.h. Instead enthalpy or internal energy are considered based on energy model chosen. Since the density change is being accounted, it is created as field in createfields.h. December 10, /

25 Solver Description Governing Equations UEqn.H: (φu) + ρu t EEqn.H:.(µ eff U).(µ eff ( U)T ) = ( ρ) p rgh.(φh e ) +.(φ(0.5 U + p ρ )).α eff T = S radiation + S h Where S radiation and S h are radiation and user defined source terms respectively. December 10, /

26 Solver Description PEqn.H The flux at boundaries are calculated and then equation for pressure is solved and relaxed. φ g = ρ.rauf.g.h ρ.ρrauf p rgh =.φ g Velocity is corrected based on boundary flux and pressure relaxation. December 10, /

27 Solver Description Thermophysical properties The solver accesses thermophysicalproperties dictionary to get all the thermophysical properties. The thermophysical models available in OpenFoam are psithermo, rhothermo, rhoreactionthermo psiureactionthermo, rhoreactionthermo, multiphasereactiont buoyantsimplefoam uses rhothermo to access the thermophysical properties. It is a density based model. December 10, /

28 Solver Description Thermophysical properties thermotype { type herhothermo; mixture puremixture; transport constant; thermo hconst; equationofstate perfectgas; specie specie; energy sensibleenthalpy; } Mixture specifies mixture composition. puremixture is used to specify a mixture without any reaction. December 10, /

29 Solver Description Thermophysical properties transport specifies the transport model to be used. The transport model evaluate properties like dynamic viscosity, thermal conductivity and thermal diffusivity. thermo specifies the type of thermodynamic model used. hthermo assumes contant cp. The equations of state available in the thermophysical library are rhoconst, perfectgas, incompressibleperfectgas, perfectfluid etc. Density is calculated based on these equations. The form of energy used in specified through this. sensibleenthalpy and sensibleinternalenergy are few examples. December 10, /

30 Test Case Test Case The tutorial buoyantcavity is used as a base for this case. The mesh for this case is similar to that used in the previous case. Same blockmeshdict file is used. The boundary conditions used for this case is similar to previous case. Except that the wall function used for alphat is compressible::alphatwallfunction;. Also v2 and f files are added to implement v2f turbulence model. December 10, /

31 Test Case ThermophysicalProperties In constant/thermophysicalproperties, mixture specie { nmoles 1; molweight ; } thermodynamics { Cp 1600; Hf 0; } transport { mu 5e-05; Pr 0.9; } December 10, /

32 Test Case Solution Control The fvschemes and fvsolution directories in system are modified similarly as done in previous case to add v2 and f. The case is run using buoyantsimplefoam and results can be checked using parafoam. December 10, /

33 Test Case Results Temperature Velocity December 10, /

34 Test Case Questions?? Thank You December 10, 2016 /