Download as PDF, PPTX
![12
Implementation in OpenFOAM
buoyantBoussinesqSimpleFoam.C
#include "fvCFD.H„ standard file for finite volume method
#include "singlePhaseTransportModel.H„ simple single-phase transport model based on viscosity-Model
#include "RASModel.H„ namespace for incompressible RAS turbulence models
#include "fvIOoptionList.H„ class for external objects or constraints on the case
#include "simpleControl.H„ checks for the simple loop
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
int main(int argc, char *argv[])
{
#include "setRootCase.H„ checks folder structure of the case
#include "createTime.H„ checks runtime according to the controlDict and initiates time variables
#include "createMesh.H„ defines mesh in the domain
#include "readGravitationalAcceleration.H„ reads value for g
#include "createFields.H„ creates the fields: T, U, 𝑃𝑟𝑔ℎ, rhok, kappat, gh, turbulence(k, ɛ, nut)
#include "createFvOptions.H„ creates related constraints according to fvOptions
#include "initContinuityErrs.H„ declare and initialise the cumulative continuity error](https://image.slidesharecdn.com/943e2705-4674-453e-af4e-d008ee3bd2a9-160210132604/85/buoyantBousinessqSimpleFoam-12-320.jpg)
Uploaded byMilad Sm
buoyantBousinessqSimpleFoam
This document provides an introduction to the buoyantBoussinesqSimpleFoam solver in OpenFOAM. It discusses the governing equations including the Boussinesq approximation and SIMPLE algorithm. It then describes the implementation in OpenFOAM, covering the files used, how the pressure, velocity, and temperature equations are solved. Finally, it summarizes the hotRoom tutorial case used to demonstrate natural convection in a room with a heat source.
buoyantBousinessqSimpleFoam
- 1. An Introduction toOpenFOAM Solver buoyantBoussinesqSimpleFoam CFD 2 Milad Salimi 16 July 2015 1
- 2. Outline Application Theoretical background GoverningEquations Boussinesq Approximation SIMPLE Algorithm Implementation in OF Pressure Shift U, T, P Equations Implementation hotRoom Tutorial 2
- 3. Application Steady-state solverfor buoyant, turbulent flow of incompressible fluids including Boussinesq approximation for stratified flow Useful for heat transfer cases with low temperature differences like ventilation problems Useful for natural convection problems due to buoyancy like flow around hot plates, radiators 3
- 4. Governing Equations 4 1) 𝛻.𝑢 = 0 Continuity Equation 2) 𝜌𝛻. 𝑢𝑢 = −𝛻𝑝 + 𝛻. 𝜇𝛻𝑢 + 𝜌𝑔 Momentum Equation 3) 𝛻. Tu = 𝑘 𝑒𝑓𝑓 𝛻2 𝑇 Temperature Equation where 𝑘 𝑒𝑓𝑓 = 𝑘 + 𝑘 𝑡 = 𝑣 𝑡 𝑃𝑟𝑡 + 𝑣0 𝑃𝑟 𝑃𝑟 = 𝑐 𝑝 𝜇0 𝑘 , 𝑃𝑟𝑡 = 𝑐 𝑝 𝜇 𝑡 𝑘 𝑡 𝑘 𝑡 − turbulent thermal conductivity
- 5. 5 • Density Variationis only important in the buoyancy term ρg • 𝜌 = 𝜌0 = 𝑐𝑜𝑛𝑠𝑡 for inertia terms • 𝜌 ≠ 𝑐𝑜𝑛𝑠𝑡 for gravitational term 𝜌𝑔 = 𝜌0 + ∆𝜌 𝑔 • Valid only when ∆𝜌 ≪ 𝜌0 • The density assumed to vary linearly with temperature ∆𝜌 = −𝜌0 𝛽 𝑇 − 𝑇𝑟𝑒𝑓 𝛽 − Coefficient of thermal expansion 1 𝐾 𝑇𝑟𝑒𝑓 − Reference Temperature 𝐾 Boussinesq Approximation
- 6. 6 Boussinesq Approximation • Momentumequation can be rewritten as: 𝜌0 𝛻. 𝑢𝑢 = −𝛻𝑝 + 𝛻. 𝜇𝛻𝑢 + 𝜌0 − 𝜌0 𝛽(𝑇 − 𝑇𝑟𝑒𝑓) 𝛻. 𝑢𝑢 = −𝛻𝑝 + 𝑣 𝑒𝑓𝑓 𝛻2 𝑢 + 𝜌 𝑘 𝑔 where 𝜌 𝑘 = 1 − 𝛽 𝑇 − 𝑇𝑟𝑒𝑓 , 𝜌 𝑘 ≪ 1 𝜌 𝑘 − effective kinematic density • Allows to solve the equations with methods for incompressible flow • Less than 1% error for temperature variations of 2K for water or 15K for air
- 7. 7 SIMPLE Algorithm • Asolution method for Incompressible Steady-State Navier Stokes Equations • SIMPLE (Semi-Implicit Method for Pressure-Linked Equations) • In incompressible flows 𝜌 = 𝑐𝑜𝑛𝑠𝑡 and not linked to pressure (no explicit eq. For p) • Pressure-Velocity coupling algorithms are used to derive equations for pressure from momentum and continuity equations • Why Semi-Implicit method? Because the discretized momentum equation and pressure correction equation are solved implicitly, where the velocity correction is solved explicitly
- 8.
- 9. 9 SIMPLE Algorithm C –Coefficient array r – explicit source terms A – Diagonal matrix of C H – off-diagonal matrix of C
- 10. 10 SIMPLE Algorithm • InSIMPLE algorithm under-relaxation is required due to the neglect of u*’ • Used to increase the stability of calculations but may slow down speed of convergence • Too small values of 𝛼 will significantly slow down the convergence • Improved versions of SIMPLE algorithm are: SIMPLER (SIMPLE Revised) SIMPLEC (SIMPLE Consistent) PISO (Pressure Implicit with Splitting of Operators)
- 11. 11 Implementation in OpenFOAM Filescan be found in $FOAM_SOLVERS/heatTransfer/buoyantBoussinesqSimpleFoam buoyantBoussinesqSimpleFoam.C main source code createFields.H creates the fields readTransportProperties.H read transport properties: 𝑣, 𝛽, 𝑇𝑟𝑒𝑓, 𝑃𝑟, 𝑃𝑟𝑡 UEqn.H solve momentum equation TEqn.H solve temperature equation pEqn.H solves the pressure, corrects the momentum velocities according to the new pressure field and adjusts the pressure level to obey overall mass continuity
- 12. 12 Implementation in OpenFOAM buoyantBoussinesqSimpleFoam.C #include"fvCFD.H„ standard file for finite volume method #include "singlePhaseTransportModel.H„ simple single-phase transport model based on viscosity-Model #include "RASModel.H„ namespace for incompressible RAS turbulence models #include "fvIOoptionList.H„ class for external objects or constraints on the case #include "simpleControl.H„ checks for the simple loop // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // int main(int argc, char *argv[]) { #include "setRootCase.H„ checks folder structure of the case #include "createTime.H„ checks runtime according to the controlDict and initiates time variables #include "createMesh.H„ defines mesh in the domain #include "readGravitationalAcceleration.H„ reads value for g #include "createFields.H„ creates the fields: T, U, 𝑃𝑟𝑔ℎ, rhok, kappat, gh, turbulence(k, ɛ, nut) #include "createFvOptions.H„ creates related constraints according to fvOptions #include "initContinuityErrs.H„ declare and initialise the cumulative continuity error
- 13. 13 Implementation in OpenFOAM •In the momentum equation we have in direction of buoyancy, the terms − 𝑑𝑝 𝑑𝑧 + 𝜌𝑔 • To make sure that in the pressure correction of the simple algorithm also the buoyancy term 𝜌𝑔ℎ is taken into account, the pressure and the buoyancy are expressed as one term: 𝑃𝑟𝑔ℎ = 𝑝 − 𝜌𝑔ℎ • Computing the derivative of 𝑃𝑟𝑔ℎ we have: − 𝑑𝑃 𝑟𝑔ℎ 𝑑𝑧 = − 𝑑𝑝 𝑑𝑧 + 𝜌𝑔 + 𝑔ℎ 𝑑𝜌 𝑑𝑧 • The term 𝑔ℎ 𝑑𝜌 𝑑𝑧 is extra and substracted via the code - ghf *fvc::snGrad(rhok) in UEqn Pressure shift due to buoyancy
- 14. 14 UEqn.H 𝛻. (𝑢𝑢) IncompressiblekOmega code (−𝑔ℎ 𝑑𝜌 𝑑𝑧 − 𝛻𝑃𝑟𝑔ℎ) * surface area over all of cell faces reconstructs a volume field from a face flux field applies relaxation factor
- 15. 15 TEqn.HSetting up 𝑘𝑡 TEqn.H Setting up 𝑘 𝑒𝑓𝑓 = 𝑘 + 𝑘 𝑡 𝜌 𝑘 is updated based on the new T s𝑜𝑙𝑣𝑒𝑠 𝑡ℎ𝑒 𝑡𝑒𝑚𝑝𝑒𝑟𝑎𝑡𝑢𝑟𝑒 𝑒𝑞𝑢𝑎𝑡𝑖𝑜𝑛 matrix
- 16. 16 pEqn.H Setting up variables rAU=𝐴−1 invertionof A rAUf=𝐴−1 𝑓 interpolatation of A to faces defining a vector field HbyA=𝐴−1 𝐻 contribution to the corrected velocity excluding pressure and gravity 𝑝ℎ𝑖𝑔 = −(𝐴−1 𝑔ℎ 𝑑𝜌 𝑑𝑛 ). 𝑆𝑓 𝑝ℎ𝑖𝐻𝑏𝑦𝐴 = 𝐴−1 𝐻 𝑓. 𝑆𝑓 defining a scalar field 𝑝ℎ𝑖𝐻𝑏𝑦𝐴 𝑝ℎ𝑖𝐻𝑏𝑦𝐴 = 𝐴−1 𝐻 𝑓. 𝑆𝑓 −(𝐴−1 𝑔ℎ 𝑑𝜌 𝑑𝑛 ). 𝑆𝑓 𝑠𝑒𝑡𝑡𝑖𝑛𝑔 𝑝𝑟𝑒𝑠𝑠𝑢𝑟𝑒 𝑐𝑜𝑟𝑒𝑐𝑡𝑖𝑜𝑛 𝑒𝑞𝑢𝑎𝑡𝑖𝑜𝑛 ∇2 𝐴−1 𝑃′ 𝑟𝑔ℎ = ∇. (𝐴−1 𝐻 − 𝐴−1 𝑔ℎ 𝑑𝜌 𝑑𝑛 ). 𝑆𝑓 𝑐𝑎𝑙𝑐𝑢𝑙𝑎𝑡𝑒𝑠 𝑃′ 𝑟𝑔ℎ
- 17. 17 pEqn.H for velocity corrector𝒖′ 𝑢𝑝𝑑𝑎𝑡𝑒𝑠 𝑡ℎ𝑒 𝑝𝑟𝑒𝑠𝑠𝑢𝑟𝑒: 𝑃 𝑛+1 𝑟𝑔ℎ = 𝑃 𝑛 𝑟𝑔ℎ + 𝛼 𝑝 𝑃′ 𝑟𝑔ℎ 𝑈 = 𝐴−1 𝐻 − 𝐴−1 𝑔ℎ 𝑑𝜌 𝑑𝑛 − 𝐴−1 ∇𝑃 𝑛+1 𝑟𝑔ℎ
- 18. 18 hotRoom Tutorial Shows howconstant temperature point heat source influences the behavior of a static volume of air Natural convection occurs K-epsilon turbulence model used
- 19. 19 hotRoom Tutorial • Acube with size 10 × 5 × 10 𝑚3 • Number of cells in each direction (20 10 20) with no grading Total 4000 cells • 6 wall patches (floor, ceiling, 4 fixed walls) • A heat source with T=600K located at floor patch (setFieldsDict)
- 20. 20 Boundary Conditions Field patchtype value U all fixedValue 0 P_rgh All fixedFluxPressure 0 T floor fixedValue 300 ceiling fixedValue 300 fixedWalls zerogradient - alphat All alphatJayatillekeWallFunction 0 P All calculated k All kqRWallFunction 0.1 epsilon All epsilonWallFunction 0.01
- 21.
- 22.
- 23.
- 24. 24 References www.openfoamwiki.net www.cfd-online.com https://github.com/OpenFOAM/OpenFOAM-2.2.x http://freefoam.sourceforge.net www.comsol.de/multiphysics/boussinesq-approximation www.bakker.org/dartmouth06/engs150/05-solv.ppt web.stanford.edu/class/me469b/handouts/incompressible.pdf www.training.prace-ri.eu/uploads/tx_pracetmo/OpenFOAMselectedSolver-1.pdf
- 25.