Description

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.

Examples

  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.

See also: openfoam_data, openfoam_export, openfoam_solve, openfoam_import