FEATool  v1.8
Finite Element Analysis Toolbox
 All Files Functions Pages
ex_spanner.m File Reference

Description

EX_SPANNER Gmsh grid import and stress calculation of a spanner.

[ FEA, OUT ] = EX_SPANNER( VARARGIN ) Example to import a Gmsh grid and calculate displacements on a fixed spanner. The load force may be distributed in the tangential load direction with the force fraction parameter FRAC.

Accepts the following property/value pairs.

Input       Value/{Default}        Description
-----------------------------------------------------------------------------------
E           scalar {190e3}         Modulus of elasticity [N/mm^2]
nu          scalar {0.29}          Poissons ratio
force       scalar {1000}          Load force [N]
frac        scalar {0}             Fraction of stress against pulling direction
sfun        string {sflag1}        Shape function for displacements
iplot       scalar 0/{1}           Plot solution (=1)
                                                                                  .
Output      Value/(Size)           Description
-----------------------------------------------------------------------------------
fea         struct                 Problem definition struct
out         struct                 Output struct

Code listing

 cOptDef = { 'E',        190e3;
             'nu',       0.29;
             'force',    1000;
             'frac',     0;
             'sfun',     'sflag1';
             'iplot',    1;
             'fid',      1 };
 [got,opt] = parseopt(cOptDef,varargin{:});


% Define scaling factor m to mm.
 USE_METERS = true;
 s = double( ~USE_METERS + USE_METERS*1e-3 );


% Import (and scale) grid.
 fea.sdim = {'x','y','z'};
 fea.grid = impexp_gmsh( 'spanner.msh', 'import', [], [], opt.fid );
 fea.grid.p = fea.grid.p*s;


% Add linear elasticity physics mode and define material parameters.
 fea = addphys( fea, @linearelasticity );
 fea.phys.el.sfun            = { opt.sfun opt.sfun opt.sfun };
 fea.phys.el.eqn.coef{1,end} = { opt.nu };
 fea.phys.el.eqn.coef{2,end} = { opt.E/s^2 };


% Set all boundaries to no load per default.
 n_bdr  = max(fea.grid.b(3,:));
 bc_sel = cell(3,n_bdr);
 [bc_sel{:}] = deal(0);


% Fix all displacements on boundaries 11 and 14.
 i_fix = [11 14];
 [bc_sel{:,i_fix}] = deal(1);
 fea.phys.el.bdr.coef{5} = bc_sel;


% Apply force for x > 140 mm.
 i_force = [1 4];
 force = opt.force/(6*s*80*s);
 fea.phys.el.bdr.coef{7}{1,i_force(1)} = ['-',num2str((1-opt.frac)*force),'*(y>140*',num2str(s),')'];
 fea.phys.el.bdr.coef{7}{3,i_force(2)} = [num2str(opt.frac*force),'*(y>140*',num2str(s),')'];


% Parse and solve problem.
 fea = parsephys(fea);
 fea = parseprob(fea);
 fea.sol.u = solvestat( fea, 'fid', opt.fid, 'icub', 1+str2num(strrep(opt.sfun,'sflag','')) );


% Postprocessing.
 if( opt.iplot>0 )
   subplot(1,2,1)
   postplot( fea, 'surfexpr', ['sqrt(u^2+v^2+w^2)/',num2str(s)] )
   view([30 20])
   title('Total displacement (mm)')

   subplot(1,2,2)
   DSCALE = 5;
   dp = zeros(size(fea.grid.p));
   for i=1:3
     dp(i,:) = DSCALE*evalexpr( fea.dvar{i}, fea.grid.p, fea );
   end
   fea_disp.grid   = fea.grid;
   fea_disp.grid.p = fea_disp.grid.p + dp;
   plotgrid( fea_disp )
   title(['Displacement plot'])
   view([30 20])
 end


% Error checking.
 u = fea.sol.u(unique(fea.eqn.dofm{1}(:)))/s;
 v = fea.sol.u(unique(fea.eqn.ndof(1)+fea.eqn.dofm{2}(:)))/s;
 w = fea.sol.u(unique(sum(fea.eqn.ndof(1:2))+fea.eqn.dofm{3}(:)))/s;
 out.disp = sqrt( u.^2 + v.^2 + w.^2 );
 out.pass = nan;
 if( ~(got.frac || got.E || got.nu || got.force) )
   out.pass = abs( max(out.disp) - 2.5 )/2.5 < 0.1;
 end


 if( nargout==0 )
   clear fea out
 end