# Axisymmetric Stress-Strain Script Modeling

Continuing on the previous post on axisymmetric modeling in FEATool, we will here take a look at how to model axisymmetric stress-strain from structural mechanics by entering and parsing the governing equations directly into FEATool using Matlab m-file scripting. The problem we will be looking at is a hollow sphere with is affected by a high uniform pressure from the inside. (Although this tutorial uses the Matlab m-script and custom equation approach to set up and run the model, the FEATool GUI with predefined axisymmetric physics modes can be used as well.)

First is to define the *fea* struct which will contain all modeling
and problem data. The space dimension coordinate names are chosen as
*r* and *z*, and their corresponding displacements as *u* and *w*. In
this case linear Lagrange finite element shape functions
`sflag1`

are used for the FEM
discretization.

```
fea.sdim = { 'r' 'z' };
fea.dvar = { 'u' 'w' };
fea.sfun = { 'sflag1' 'sflag1' };
```

Next, is to create the computational geometry and grid. By using
axisymmetry we are able to save a lot of computational cost by
reducing the geometry from three to two dimensions. Since we are
looking at a perfect symmetric spherical sphere or shell we can also
get away with only modeling a single quadrant of a ring. Such a grid
can be created with the help of the
`ringgrid`

function, as follows

```
r_i = 1;
r_o = 2;
fea.grid = ringgrid( 12, 72, r_i, r_o );
fea.grid = delcells( fea.grid, selcells( fea.grid, '(x<=eps) + (y<=eps)') );
```

The derivation of the axisymmetric stress strain equations is left to
the reader, but they are defined in two string equation variables for
the radial *r* and *z*-directions, respectively. The equations are
also parsed by `parseeqn`

to
generate the weak FEM formulation stored in the *fea.eqn* struct.

```
eqn_r = '- c1*( (1-nu)*ur_r + nu*wz_r + nu/r*( u_r - ur_t - wz_t ) - (1-nu)/r^2*u_t ) - c1*c2*( uz_z + wr_z ) = 2*pi*r*Fr';
eqn_z = '- c1*( nu*ur_z + nu/r*u_z + (1-nu)*wz_z ) - c1*c2*( uz_r + wr_r ) = 2*pi*r*Fz';
fea.eqn = parseeqn( { eqn_r eqn_z }, fea.dvar, fea.sdim );
```

Furthermore, equation coefficients and constants are defined in the
*fea.expr* field. The empty cells are simply placeholders for
coefficient string descriptions and names used by the FEATool GUI,
and not needed here

```
nu = 0.3;
E = 200e9;
c1 = E / ((1+nu)*(1-2*nu) );
c2 = (1-2*nu) / 2;
fea.expr = { 'c1' [] [] {[num2str(c1*2*pi),'*r']} ;
'c2' [] [] {c2} ;
'nu' [] [] {nu} ;
'Fr' [] [] {0} ;
'Fz' [] [] {0} };
```

Boundary conditions must also be prescribed. In this case a force
acting in the normal direction of the inner boundary (number 1), and
also zero normal displacements on the symmetry boundaries (3 and
4). (Note that one can use the
`plotbdr`

function to visualize and
see the boundary numbering).

```
p = 20e4;
fea.bdr.d = { [] [] [] [0] ;
[] [] [0] [] };
fea.bdr.n = { [num2str(p*2*pi),'*r*-nr'] [] [] [] ;
[num2str(p*2*pi),'*r*-nz'] [] [] [] };
```

Lastly the whole *fea* problem struct is checked and parsed and sent
to the static solver.

```
fea = parseprob( fea );
fea.sol.u = solvestat( fea );
```

The solution can be visualized, plotted, and compared to the expected analytical displacement of a hollow sphere.

```
n = 20;
r = linspace(r_i,r_o,n);
z = zeros(1,n);
u_ref = 1./(2*E*(r_o^3-r_i^3)*r.^2) .* (2*(p*r_i^3)*(1-2*nu)*r.^3+p*(1+nu)*r_o^3*r_i^3);
u = evalexpr( 'u', [r;z], fea );
subplot(1,2,1)
postplot( fea, 'surfexpr', 'sqrt(u^2+w^2)', 'arrowexpr', {'u' 'w'} )
title('computed displacement')
subplot(1,2,2), hold on
plot(u_ref,r,'r-')
plot(u,r,'b.')
title( 'radial displacement')
legend('exact solution','computed solution')
xlabel('r')
grid on
```

The complete FEATool m-script file is available for download from the link below together with a selection of other axisymmetric stress strain benchmark examples.

This post has shown how to implement the custom axisymmetric
stress-strain equation and structural mechanics model using a Matlab
m-script file. However, one could just as well do this using either
the *Custom Equation* or *Plane Stress/Strain* physics modes by
editing the corresponding equations in the FEATool Multiphysics GUI.