FEATool Multiphysics
v1.17.0
Finite Element Analysis Toolbox
|
OPENFOAM OpenFOAM CFD solver interface.
[ U, TLIST, VARS ] = OPENFOAM( FEA, VARARGIN ) Export, solves, and/or imports the solved problem described in the finite element problem struct FEA using the OpenFOAM CFD solver. Accepts the following property/value pairs.
Input Value/{Default} Description ----------------------------------------------------------------------------------- mode check, export, solve, import Command mode(s) to call (default all) casedir {tempdir/random} OpenFOAM case directory control logical {false} Show solver control panel. foamdir default OpenFOAM installation directory logfname default OpenFOAM log/output filename fid/logfid scalar {1/stdout} Log file/message output file handle
MODE is a string or cell array of strings selecting action(s) to perform. By default check, export, solve, and import are performed in sequence.
Returns the solution vector U (n_dof x n_timesteps), corresponding list of time steps TLIST, and additional solution variables in VARS.
Additional options are passed to the OPENFOAM_DATA, OPENFOAM_EXPORT, OPENFOAM_SOLVE, and OPENFOAM_IMPORT functions.
1) Laminar steady Hagen-Poiseuille flow in a channel. n = 20; rho = 1; miu = 1; uin = 1; fea.sdim = {'x', 'y'}; fea.geom.objects = {gobj_rectangle(0, 3, 0, 1)}; fea.grid = rectgrid(3*n, 1*n, [0, 3;0, 1]); fea = addphys(fea,@navierstokes); fea.phys.ns.eqn.coef{1,end} = {rho}; fea.phys.ns.eqn.coef{2,end} = {miu}; fea.phys.ns.eqn.coef{5,end} = {uin}; fea.phys.ns.bdr.sel(2) = 4; fea.phys.ns.bdr.sel(4) = 2; fea.phys.ns.bdr.coef{2,end}{1,4} = uin; fea = parsephys(fea); fea = parseprob(fea); fea.sol.u = openfoam(fea); subplot(2,1,1) postplot(fea, 'surfexpr', 'p', 'isoexpr', 'sqrt(u^2+v^2)', 'arrowexpr', {'u', 'v'}) subplot(2,1,2), hold on, grid on xlabel('Velocity profile at outlet'), ylabel('y') x = 3*ones(1, 100); y = linspace(0, 1, 100); U_ref = 6*uin*(y.*(1-y))./1^2; U = evalexpr('sqrt(u^2+v^2)', [x;y], fea); plot(U_ref, y, 'r--', 'linewidth', 3) plot(U, y, 'b-', 'linewidth', 2.5) legend('Analytic solution', 'Computed solution') 2) Axisymmetric turbulent flow in a pipe, showing solution convergence curves. Re = 1e5; rho = 1; miu = 1/Re; win = 1; fea.sdim = {'r', 'z'}; fea.geom.objects = {gobj_rectangle(0, .5, 0, 15)}; n_lev = 3; nx = 2^(n_lev-1) * 5; ny = 2^(n_lev-1) * 50; px = [.5, .49, .47, .44, .4, .2, 0]; px = interp1(linspace(0,0.5,length(px)), px, linspace(0,0.5,nx)); fea.grid = rectgrid(px, ny, [0, .5; 0, 15] ); fea = addphys(fea,{@navierstokes,true}); fea.phys.ns.eqn.coef{1,end} = {rho}; fea.phys.ns.eqn.coef{2,end} = {miu}; fea.phys.ns.eqn.coef{6,end} = {win}; fea.phys.ns.bdr.sel(1) = 2; fea.phys.ns.bdr.sel(2) = 1; fea.phys.ns.bdr.sel(3) = 4; fea.phys.ns.bdr.sel(4) = 5; fea.phys.ns.bdr.coef{2,end}{2,1} = win; fea = parsephys(fea); fea = parseprob(fea); turb.model = 'kEpsilon'; turb.inlet = [0.001, 0.00045]; turb.wallfcn = 1; fea.sol.u = openfoam(fea, 'turb', turb, 'hax', axes(), 'control', true, 'nproc', 1); figure,subplot(1,2,1) postplot(fea, 'surfexpr', 'sqrt(u^2+w^2)', 'isoexpr', 'sqrt(u^2+w^2)', 'arrowexpr', {'u' 'w'}) axis([0, .5, 14, 15]) subplot(1,2,2), hold on, grid on xlabel('Velocity profile at outlet'), ylabel('r') r = linspace(0, 0.5, 100); z = 15*ones(1, 100); U = evalexpr('sqrt(u^2+w^2)', [r;z], fea); plot(U, r, 'b-', 'linewidth', 2.5)
Further OpenFOAM supported script model examples can be found as EX_NAVIERSTOKES1-4/6-8/10-13/17, EX_COMPRESSIBLEEULER2-6, EX_HEATTRANSFER10.