double-edge notched specimen

The double edge notched specimen was investigated by Nooru-Mohamed (1992).

This example is taken from the thesis. The details of the model can be seen in Section 6.3.

The model can be downloaded here.

Model Setup

The definitions of nodes and elements can be seen in element_f.supan and node_f.supan.

To ease the work of defining boundary conditions and load, some node groups can be defined first.

In total four edges will be used, here the generatebypoint command is used to find all relevant nodes.

# find all nodes on the line segment defined by (0,0) and (200,0)
generatebypoint nodegroup 1 0. 0. 200. 0.

# find all nodes on the line segment defined by (200,0) and (200,100)
generatebypoint nodegroup 2 200. 0. 200. 100.

# find all nodes on the line segment defined by (0,200) and (200,200)
generatebypoint nodegroup 3 0. 200. 200. 200.

# find all nodes on the line segment defined by (0,100) and (0,200)
generatebypoint nodegroup 4 0. 100. 0. 200.

The boundary conditions are explicitly assigned to the corresponding node groups.

# for all four edges, the drilling DoFs are constrained
grouppenaltybc 1 3 1 2 3 4

# constrain horizontal movement of edge 2
grouppenaltybc 2 1 2
# constrain vertical movement of edge 1
grouppenaltybc 3 2 1

Two displacement loads are applied. Two files h and v are used to define the amplitudes.

# horizontal dispalcement to generate a 5kN total horizontal tension force
amplitude Tabular 1 h
groupdisplacement 1 1 -16.5E-3 1 4

amplitude Tabular 2 v
groupdisplacement 2 2 .1 2 3

If VTK is enabled, it is possible to record the distribution of tension damage at each converged substep.

hdf5recorder 1 Visualisation DT width 3 scale 0

Since we are not interested in the displacement, scale is simply set to zero. The output file are automatically numbered with a total width of four. It is changed to three in this example. The generated visualisation files can be loaded into ParaView as a group to generate animations.

The analysis has a duration of two seconds. In the first second, the horizontal tension is applied, then the vertical load is applied.

step static 1 2
set fixed_step_size 1
set ini_step_size 5E-3

converger RelIncreDisp 1 1E-4 20 1

Results

Results are shown as follows, which agree with experimental results.

tension damage distribution

the first principal stress distribution

Element Deletion

It is possible to further define a criterion so that for elements that exceed a certain value of $d_t$, they are removed from the model. This is an approach adopted widely to simulate crack propagation.

criterion MaxHistory 1 DT .8

The animation of crack development is shown as follows.

crack development

Performance

See a typical profiling.