FEATool  v1.7.1
Finite Element Analysis Toolbox
 All Files Functions Pages
ex_planestress1.m File Reference

Description

EX_PLANESTRESS1 Example for plane stress for hole in plate.

[ FEA, OUT ] = EX_PLANESTRESS1( VARARGIN ) Example to calculate displacements and stresses for a hole in plate configuration under plane stress assumption.

Accepts the following property/value pairs.

Input       Value/{Default}        Description
-----------------------------------------------------------------------------------
E           scalar {210e9}         Modulus of elasticity
nu          scalar {0.3}           Poissons ratio
diam        scalar {0.01}          Diameter of hole
thick       scalar {0.001}         Plate thickness
force       scalar {1000}          Load force
sx_ref      scalar {3e7}           Reference stress in x-direction
hmax        scalar {0.00125}       Max grid cell size
sfun        string {sflag1}        Shape function for displacements
iphys       scalar 0/{1}           Use physics mode to define problem (=1)
iplot       scalar 0/{1}           Plot solution (=1)
                                                                                  .
Output      Value/(Size)           Description
-----------------------------------------------------------------------------------
fea         struct                 Problem definition struct
out         struct                 Output struct

Code listing

 cOptDef = { ...
   'E',        210e9; ...
   'nu',       0.3; ...
   'diam',     0.01; ...
   'thick',    0.001; ...
   'force',    1000; ...
   'sx_ref',   3e7; ...
   'hmax',     0.00125; ...
   'sfun',     'sflag1'; ...
   'iphys',    1; ...
   'iplot',    1; ...
   'tol',      0.05; ...
   'fid',      1 };
 [got,opt] = parseopt(cOptDef,varargin{:});
 fid       = opt.fid;


% Model, geometry, and grid parameters.
 h         = 0.05;            % Height of 1/4 rectangular domain.
 l         = 0.05;            % Length of 1/4 rectangular domain.
 xc        = 0;               % x-coordinate of hole center.
 yc        = 0;               % y-coordinate of hole center.
 area      = 2*h*opt.thick;   % Area on which load force is applied.


% Geometry definition.
 gobj1 = gobj_rectangle( 0, l, 0, h, 'R1' );
 gobj2 = gobj_circle( [0 0], opt.diam/2, 'C1' );
 fea.geom.objects = { gobj1 gobj2 };
 fea = geom_apply_formula( fea, 'R1-C1' );
 fea.sdim = { 'x' 'y' };   % Coordinate names.


% Grid generation.
 fea.grid = gridgen(fea,'hmax',opt.hmax,'fid',fid);
 n_bdr    = max(fea.grid.b(3,:));        % Number of boundaries.


% Boundary conditions.
 dtol  = opt.diam/10;
 lbdr  = findbdr( fea, ['x<=',num2str(dtol)] );     % Left boundary number.
 rbdr  = findbdr( fea, ['x>=',num2str(l-dtol)] );   % Right boundary number.
 lobdr = findbdr( fea, ['y<=',num2str(dtol)] );     % Lower boundary number.


% Problem definition.
 E11 = opt.E/(1-opt.nu^2);
 E12 = opt.nu*E11;
 E22 = E11;
 E33 = opt.E/(1+opt.nu)/2;

 if ( opt.iphys==1 )

   fea = addphys(fea,@planestress);      % Add plane stress physics mode.
   fea.phys.pss.eqn.coef{1,end} = { opt.nu };
   fea.phys.pss.eqn.coef{2,end} = { opt.E  };
   fea.phys.pss.sfun            = { opt.sfun opt.sfun };   % Set shape functions.

   bctype = mat2cell( zeros(2,n_bdr), [1 1], ones(1,n_bdr) );
   bctype{1,lbdr}  = 1;
   bctype{2,lobdr} = 1;
   fea.phys.pss.bdr.coef{1,5}   = bctype;
   bccoef = mat2cell( zeros(2,n_bdr), [1 1], ones(1,n_bdr) );
   bccoef{1,rbdr} = opt.force/area;
   fea.phys.pss.bdr.coef{1,end} = bccoef;

   fea = parsephys(fea);                 % Check and parse physics modes.

 else

   fea.dvar  = { 'u' 'v' };                  % Dependent variable names.
   fea.sfun  = { opt.sfun opt.sfun };        % Shape functions.

% Define equation system.
   fea.eqn.a.form = { [2 3;2 3] [3 2;2 3];   ...
                      [3 2;2 3] [2 3;2 3] }; ...
   fea.eqn.a.coef = { {E11 E33} {E12 E33};   ...
                      {E33 E12} {E33 E11} };
   fea.eqn.f.form = { 1 1 };
   fea.eqn.f.coef = { 0 0 };

% Define boundary conditions.
   fea.bdr.d     = cell(2,n_bdr);
   fea.bdr.n     = cell(2,n_bdr);
  [fea.bdr.n{:}] = deal(0);              % Assign zero to all Neumann boundaries.

   fea.bdr.n{1,rbdr}  = opt.force/area;  % Set horizontal load force on right boundary.

   fea.bdr.d{1,lbdr}  = 0;               % Set zero horizontal displacement on left boundary.

   fea.bdr.d{2,lobdr} = 0;               % Set zero vertical displacement on lower boundary.

 end


% Parse and solve problem.
 fea       = parseprob(fea);             % Check and parse problem struct.
 fea.sol.u = solvestat(fea,'fid',fid);   % Call to stationary solver.


% Postprocessing.
 s_sx = [num2str(E11),'*ux+',num2str(E12),'*vy'];
 if ( opt.iplot>0 )
   figure
   postplot(fea,'surfexpr',s_sx,'isoexpr',s_sx,'evaltype','exact')
   title('Stress, x-component')
 end


% Error checking.
 [~,sx_max] = minmaxsubd( s_sx, fea );
 out.sx_max = sx_max;
 out.err    = opt.sx_ref-sx_max;
 out.pass   = (sx_max>(opt.sx_ref*(1-opt.tol)))&&(sx_max<(opt.sx_ref*(1+opt.tol)));


 if ( nargout==0 )
   clear fea out
 end