How can I run a crack cohesive model in Mofem?

[Arthur Álax de Araujo Albuquerque]

Are there any documantation that explain How I can run a crack cohesive model in Mofem?

[zahur.ullah1]

The theoretical background of the cohesive crack model can be found in our recent paper: 

http://www.sciencedirect.com/science/article/pii/S0263822316318104

The way the cohesive user module works and how it should run is given in: 

build_mofem/user_modules/cohesive_interface/README

And examples meshes can be found in the source code: 

mofem-cephas/mofem/users_modules/basic_finite_elements/cohesive_interface/

[Lukasz Kaczmraczyk]

Arthur, you can have a go and try to run peel test problem. Mesh is in application directory. In the case of any difficulty, just ask.

If you like to change model, to bilinear or exponential softening, we guide you how to do this.

Regards,

Lukasz

[Lukasz Kaczmraczyk]

Go to directory,

cd $HOME/mofem_installation/users_modules/basic_finite_elements/cohesive_interface/

Run code,

mpirun -np 4 ./arc_length_interface \
-my_file PeelTestHalfCrack.h5m \
-my_order 2 -ksp_type fgmres \
-pc_type lu -pc_factor_mat_solver_package mumps -ksp_monitor \
-ksp_atol 1e-10 -ksp_rtol 1e-10 \
-snes_monitor -snes_type newtonls -snes_linesearch_type l2 -snes_linesearch_monitor \
-snes_max_it 16 -snes_atol 1e-8 -snes_rtol 1e-8 -my_sr 1e-1 -my_ms 3 \
-snes_converged_reason 2>&1| tee log

Note only 3 steps, -my_ms 3, you have to have more if you like to see something interesting. I recommend to use higher order appriximation for test, -my_order 2, you can run analysis whet higher order and see diffrence. This mesh is very corse, so you will see big improvement with higher orders.

No you can convert output files to VTK,

../nonlinear_elasticity/do_vtk.sh out_values_*.h5m

Now you can open data in preview,

paraview --data=out_values_*.vtk

Regards,

Lukasz

[Lukasz Kaczmraczyk]

You can use this mesh for tests,  load it to cubit and save cub file, which can use 

-my_file PeelTest.cub

reset


brick x 10 y 2 z 1
webcut volume 1 with plane yplane imprint merge


create Displacement  on surface 16 9  dof 1 dof 2 dof 3 fix 0
create force  on surface 13  vector 0 1 0 0 0 0
create force  on surface 11  vector 0 -1 0 0 0 0
create cfd_bc interface on surface 7


set duplicate block elements on
block 1 volume all
block 1 name "MAT_ELASTIC"
block 1 attribute count 2
block 1 attribute index 1 1
block 1 attribute index 2 0.0
block 2 surface 7
block 2 name "MAT_INTERF"
block 2 attribute count 4
block 2 attribute index 1 1
block 2 attribute index 2 0
block 2 attribute index 3 1
block 2 attribute index 4 1


nodeset 4 vertex 5
nodeset 4 name "LoadPath"


volume all scheme Tetmesh
volume all size auto factor 7
mesh volume all

Nodset "LoadPath" is used to print displacements (and load factor) on the specific for specific node (or nodes).  Displacements and load factor printed as well to file "load_disp.txt". You can use this to plot load displacement path.