Tutorial 1: A simple patch test

This part is taken from Section 2.6 of

The implementation of a finite element simulation under displacement control is demonstrated by means of a patch test. Patch tests are simple finite element simulations which are intended to demonstrate that an element possesses some basic requirements, such as the ability to represent a uniform stress state. The following patch test is taken from MacNeal and Harder (1985).

We consider a rectangular domain, shown in Figure 2.9. The domain is discretised by five quadrilateral elements. The positions of the nodes are chosen such that all elements are skewed and are mildly distorted. The positions of the internal nodes 4, 5, 6, and 7 are given in the figure. The displacements a = (ax, ay) of the external nodes 0, 1, 2, and 3 are prescribed according to the relations:

Node	x	y
4	0.04	0.02
5	0.18	0.03
6	0.16	0.08
7	0.08	0.08

In order to test whether everything is installed properly, the following two simulations can be run.

Simple example

In the directory ‘’examples/ch02’’ the script ‘’PatchTest.py’’ can be executed from a terminal (or DOS-shell) by typing:

python PatchTest.py

In Windows, this script can also be executed by double-clicking the icon.

PyFEM example

The full finite element code PyFEM can be run by typing ‘’pyfem’’ in the terminal. In directory ‘’examples/ch04’’ for example, the input file ‘’ShallowTrussRiks.pro’’ is processed by typing:

pyfem ShallowTrussRiks.pro

Here, ‘’ShallowTrussRiks.pro’’ is the input file, which by definition ends with ‘’.pro’’. When it is opened in a text editor, it looks as follows:

input = "ShallowTrussRiks.dat";

TrussElem  =
{
  ....
};

SpringElem =
{
  ....
};

solver =
{
  ....
};

outputModules = ["graph"];

graph =
{
  ....
};

The dots indicate lines that have been omitted in this example. The first argument in the ‘’.pro’’-file specifies the input file, which contains the positions of the nodes, the element connectivity and the boundary conditions. The structure of this file, which normally has the extension ‘’.dat’’, is as follows:

<Nodes>
  1   0.0 0.0 ;
  2 -10.0 0.0 ;
  3  10.0 0.0 ;
  4   0.0 0.5 ;
</Nodes>

<Elements>
  1 'TrussElem' 2 4 ;
  2 'TrussElem' 3 4 ;
  3 'SpringElem' 1 4 ;
</Elements>

<NodeConstraints>
  u[1] = 0.0;
  u[2] = 0.0;
  u[3] = 0.0;

  v[1] = 0.0;
  v[2] = 0.0;
  v[3] = 0.0;
</NodeConstraints>

<ExternalForces>
  v[4] = -100.0 ;
</ExternalForces>

The nodes are defined between the labels ‘’<Nodes>’’ and ‘’</Nodes>’’. The first number indicates the node identification number. The remaining numbers denote the coordinates in x-, y-, and in the case of a three dimensional simulation, the z-direction. For example, node 2 has the x and y coordinates (-10,0).

The element connectivity is given after the tag ‘’<Elements>’’. The first number indicates the element ID number. The string refers to the name of the element model this element belongs to. The remaining numbers are the nodes that are used to construct the element. In this example, the first element is of the type ‘’TrussElem’’ and is supported by nodes 2 and 4.

The boundary conditions and applied loads are specified next. The node constraints are given after the label texttt{<NodeConstraints>}. In this example, the displacement components ‘’u’’ and ‘’v’’ of nodes 1,2 and 3 have a prescribed value of 0.0. The external forces are specified in a similar manner in the field ‘’<ExternalForces>’’. Here, a unit external force with magnitude -100.0 is added to node number 4 in the direction that corresponds to the ‘’v’’ displacement. Hence, this force is acting in the negative y-direction.

The parameters of the finite element model are specified in the ‘’.pro’’ file, in the fields ‘’TrussElem’’ and ‘’SpringElem’’, which refer to the labels used in the element connectivity description:

TrussElem  =
{
  type = "Truss";
  E    = 5e6;
  Area = 1.0;
};

SpringElem =
{
  type = "Spring";
  k    = 100.0;
};

The elements denoted by the label ‘’TrussElem’’ are of the type ‘’Truss’’. This model requires two additional parameters, the Young’s modulus of the material ‘’E’’ and the area of the cross-section texttt{Area}. The label ‘’SpringElem’’ denote elements of the type ‘’Spring’’. Here, one additional parameter is required: the spring stiffness ‘’k’’. A detailed overview of the element types and the corresponding parameters can be found in Section of this manual.

The parameters of the solver are defined next:

solver =
{
  type = 'RiksSolver';

  fixedStep = true;
  maxLam    = 10.0;
};

The solver is of the type ‘’RikSolver’’. The two additional parameters specify that the magnitude of the path-parameter is constant (‘’fixedStep = true’’) and that the simulation is stopped when the load parameter $lambda$ reaches a value of 10.0. A detailed overview of available solver types and their parameters is given in Section xx.

Finally, the results of the simulation can be stored and visualised in several ways. To this end, a chain of output modules can be specified. In this example, the results are stored in a load-displacement curve in the module ‘’GraphWriter’’:

outputModules = ["graph"];

graph =
{
  type     = "GraphWriter";
  onScreen = true;

  columns = [ "disp" , "load" ];

  disp =
  {
    type   = "state";
    node   = 4;
    dof    = 'v';
    factor = -1.0;
  };

  load =
  {
    type = "fint";
    node = 4;
    dof  = 'v';
  };
};

In this example, two colums are stored: ‘’disp’’, the displacement (‘’state’’) of node 4 in the vertical direction and ‘’load’’, the corresponding internal force. The parameter ‘’onScreen = true’’ is used to show the load-displacement curve on the screen during the simulation. By default, the results will be stored in a file called ‘’ShallowTrussRiks.out’’. A description of all available output modules can be found in Section xx.