Creating finite element meshes

Relevant module edelweissfe.generators.abqmodelconstructor

The default way to create finite element meshes is using the keywords

• *node

• *element

• *nset

• *elset

• *surface

employing an Abaqus-like syntax.

Example: testfiles/LinearElasticIsotropic/test.inp

*node
** Our  nodes
** ID   coordinates
0,  0,       0,      0
1,  0.100,   0,      0
2,  0.100,   0.100,  0
3,  0,       0.100,  0
4,  0,       0,      0.100
5,  0.100,   0,      0.100
6,  0.100,   0.100,  0.100
7,  0,       0.100,  0.100

*element, type=C3D8, provider=marmot
** We create a single hex8 element
** ID       node IDs
1,      0,1,2,3,4,5,6,7

*nSet, nSet=left
0,1,4,5
*nSet, nSet=bottomleft
1
*nSet, nSet=bottomback
0

*elSet, elSet=theOnlyElement
1

*material, name=LinearElastic, id=myMaterial
**Isotropic
**E   | nu |
1.8e4, 0.22

*section, name=section1, material=myMaterial, type=solid
** element set 'all' is automatically created
** we could also use the set 'theOnlyElement'
all

*surface, type=element, name=surfaceRight
** Elset,   faceID
all,        4

*job, name=mySingleElementJob, domain=3d
*solver, solver=NIST, name=theSolver

*step, solver=theSolver, maxInc=1e0, minInc=1e0, maxNumInc=100, maxIter=25, stepLength=1
** The first step: set the BCs
dirichlet, name=1, nSet=left,       field=displacement, 2=0
dirichlet, name=2, nSet=bottomback, field=displacement, 1=0,3=0
dirichlet, name=3, nSet=bottomleft, field=displacement, 3=0

*step, solver=theSolver, maxInc=1e0, minInc=1e0, maxNumInc=10, maxIter=25, stepLength=1
** The second step: apply the load
distributedload, name=dload, surface=surfaceRight, type=pressure, magnitude=0.15, f(t)='t**2'

*fieldOutput
** The results we are interested in
create=perElement, name=strain,       elSet=all, result=strain, quadraturePoint=0:8, f(x)='np.mean(x,axis=1)'
create=perElement, name=stress,       elSet=all, result=stress, quadraturePoint=0:8, f(x)='np.mean(x,axis=1)'
create=perNode, name=RF_left,      nSet=left, field=displacement, result=P, f(x)='np.sum(x[:,1])'
create=perNode, name=displacement, elSet=theOnlyElement, field=displacement, result=U

*output, type=ensight, name=myEnsightOutput
** For visualization in Paraview etc.
create=perNode, fieldOutput=displacement
create=perElement, fieldOutput=stress
create=perElement, fieldOutput=strain
configuration, overwrite=yes

*output, type=monitor, name=myMonitor
** Directly print to the terminal
fieldOutput=RF_left