Step actions

Step actions define actions run during a simulation. They are defined within a *step definition, line by line, by specifying their name and a list of option=value, for example

*step, jobName=myJob,
    dirichlet, name=bottom,   nSet=bottom,   field=displacement, 2=0, 1=0
    dirichlet, name=rightTop, nSet=rightTop, field=displacement, 2=0,
    distributedload, name=dload1, surface=top,  type=pressure, magnitude=10, f(t)=t*2
    distributedload, name=dload2, surface=left, type=pressure, magnitude=50, f(t)=t

`bodyforce` - Bodyforce loads

Relevant module: edelweissfe.stepactions.bodyforce

Options:
Option	Description
`forceVector`	The force vector
`delta`	In subsequent steps only: define the updated force vector incrementally
`f(t)`	(Optional) define an amplitude in the step progress interval [0…1]

Example: testfiles/BodyForce3D/test.inp

*include, input=mesh.inp

*material, name=linearelastic, id=le
30000.0, 0.15

*section, name=section1, material=le, type=solid
all

*job, name=c3d8job, domain=3d
*solver, solver=NIST, name=theSolver

*fieldOutput
create=perNode, name=displacement, elSet=all, field=displacement, result=U, name=displacement
create=perElement, name=stress, elSet=all, result=stress, quadraturePoint=1
create=perElement, name=strain, elSet=all, result=strain, quadraturePoint=1
create=perNode, name=RF, nSet=top, result=P, field=displacement

*output, type=ensight, name=ensightExport
create=perNode,    fieldOutput=displacement
create=perElement, fieldOutput=stress
create=perElement, fieldOutput=strain
configuration, overwrite=yes

*output, type=monitor, name=myNodeSetMonitor
fieldOutput=RF, f(x)='sum(x[:,0])', name=ForceX
fieldOutput=RF, f(x)='sum(x[:,1])', name=ForceY
fieldOutput=RF, f(x)='sum(x[:,2])', name=ForceZ

*step, solver=theSolver, maxInc=1e-1, minInc=1e-5, maxNumInc=1000, maxIter=25, stepLength=1
options, category=NISTSolver, extrapolation=linear
dirichlet, name=top,  nSet=top,   field=displacement, 1=0.0, 2=0.0, 3=.0
bodyforce, name=bforce, elSet=all, forceVector='0.0, 10.0, 20.0', f(t)=t

`dirichlet` - Standard dirichlet BC

Relevant module: edelweissfe.stepactions.dirichlet

Options:
Option	Description
`nSet`	The node set for application of the BC
`1,2,3,...`	Prescribed values for components of the physical field
`components`	Prescribed values using a np.ndarray for representation; use ‘x’ for ignored values
`field`	Field for which the boundary condition is active
`analyticalField`	(Optional) scales the defined boundary condition
`f(t)`	(Optional) define an amplitude in the step progress interval [0…1]

`distributedload` - Distributed surface loads

Relevant module: edelweissfe.stepactions.distributedload

Options:
Option	Description
`surface`	Surface for application of the distributed load
`magnitude`	Magnitude of the distributed load
`delta`	In subsequent steps only: define the new magnitude incrementally
`f(t)`	(Optional) define an amplitude in the step progress interval [0…1]
`type`	The load type, e.g., pressure or surface traction; Must be supported by the element type

Example: testfiles/DLoad/test.inp

*modelGenerator, generator=planeRectQuad, name=gen
elType=CPE4
nX=20
nY=5
l=100
h=25

*elSet, elSet=loadEls
100,95,90,85,80

*surface, type=element, name=surfaceLoad
**elset, faceID
loadEls, 3


*section, name=section1, thickness=1.0, material=mat, type=plane
all
*material, name=VonMises, id=mat
210000, 0.3, 550, 1000, 200, 1400

*job, name=cpe4job, domain=2d
*solver, solver=NIST, name=theSolver

*fieldOutput
create=perNode, name=displacement, elSet=all, field=displacement, result=U, name=displacement
create=perNode, name=displacement, nSet=gen_left, field=displacement, result=P, name=RF
create=perElement, name=stress, elSet=all, result=stress, quadraturePoint=1
create=perElement, name=strain, elSet=all, result=strain, quadraturePoint=1

*output, type=monitor, name=ensightExport
fieldOutput = RF, f(x) = 'sum ( x[:, 1])'

*output, type=ensight, name=ensightExport
create=perNode,    fieldOutput=displacement
create=perElement, fieldOutput=stress
create=perElement, fieldOutput=strain
configuration, overwrite=yes
*step, solver=theSolver, maxInc=1e-1, minInc=1e-5, maxNumInc=1000, maxIter=25, stepLength=1
options, category=NISTSolver, extrapolation=linear
dirichlet, name=left,  nSet=gen_left,   field=displacement, 1=0.0, 2=0.0
distributedload, name=dload, surface=gen_top, type=pressure, magnitude=0.15, f(t)=t

`geostatic` - Geostatic stress states

Relevant module: edelweissfe.stepactions.geostatic

Initialize materials to an geostatic stress state

Options:
Option	Description
`p1`	sig_x=sig_y=sig_z in first point
`h1`	y coordinate of first point, default=1.0
`p2`	s11=s22=s33 in second point, default=p1
`h2`	y coordinate of second point, default=-1.0
`xLateral`	ratio of sig_x/sig_y, default=1.0
`zLateral`	ratio of sig_z/sig_y, default=1.0

Example: testfiles/GeoStatic/test.inp

*modelGenerator, generator=planeRectQuad, name=gen
l=50
h=150
nX=10
nY=30
elType=CPE4

*material, name=linearElastic, id=le
210000, 0.3

*section, name=section1, thickness=1.0, material=le, type=plane
all

*job, name=cpe4job, domain=2d
*solver, solver=NIST, name=theSolver
*fieldOutput
create=perNode, name=dispTop, nSet=gen_top,       field=displacement, result=U, f(x)='mean(x[:,1])'
create=perNode, name=RFBottom, nSet=gen_bottom,    field=displacement, result=P, f(x)='sum(x[:,1])'
create=perNode, elSet=all,  field=displacement, result=U, name=displacement
create=perElement, elSet=all,  result=stress,  name=S11,  quadraturePoint=1, f(x)='x[:,0]'
create=perElement, elSet=all,  result=stress,  name=S22,  quadraturePoint=1, f(x)='x[:,1]'
create=perElement, elSet=all,  result=stress,  name=S33,  quadraturePoint=1, f(x)='x[:,2]'

*output, type=monitor
fieldOutput=dispTop
*output, type=monitor
fieldOutput=RFBottom

*output, type=ensight, name=ensightExport
create=perNode, fieldOutput=displacement
create=perElement, fieldOutput=S11
create=perElement, fieldOutput=S22
create=perElement, fieldOutput=S33
configuration, overwrite=yes


*step, solver=theSolver, maxInc=0.5
dirichlet, name=left,   nSet=gen_left,   field=displacement, 1=0.0,
dirichlet, name=right,  nSet=gen_right,   field=displacement, 1=0.0
dirichlet, name=bottom, nSet=gen_bottom,   field=displacement, 2=0.0,
geostatic, name=geo, elSet=all, p1=-10, h1=150, p2=-5, h2=0, xLateral=1.0, zLateral=1.0
distributedload, name=dlTop, surface=gen_top, magnitude=10, f(t)=1, type=pressure

*step, solver=theSolver, maxInc=1e-1,
distributedload, name=dlTop, delta=-10.0, f(t)=t

`indirectcontrol` - Indirect displacement control

Relevant module: edelweissfe.stepactions.indirectcontrol

Options:
Option	Description
`dof1`	Degree of freedom for the constraint ( model access expression )
`dof2`	Degree of freedom for the constraint ( model access expression )
`L`	Final distance (e.g. crack opening)

Example: testfiles/IndirectDisplacementControl/test.inp

*job, name=job, domain=3d

*solver, solver=NISTPArcLength, name=NISTPArcLen

*modelGenerator, generator=boxGen, name=gen
lX     = 100
lY     = 1
lZ     = 1
nX     = 9
nY     = 1
nZ     = 1
elType = GC3D8

*material, name=gcdp, id=concrete
**E         nu      fcy         fcu         fbu         ftu         Df          Ah
100.0,      0.00,   10,         30,         35,         3.00,       0.85,       0.12,
**Bh        Ch      Dh          As          softmod     l           m           omegaMax
0.003,      2.0,    1e-6,       15.0,       .1,         2,          1.05,       1,
**derivativeMethod, dTThresholdElasticStiffness
1,                  1e-8

*section, name=concrete, material=concrete, type=solid
all

*modelGenerator, generator=findClosestNode, name=closestN1, executeAfterManualGeneration=True
location='40, 0, 0'
storeIn=IDC1

*modelGenerator, generator=findClosestNode, name=closestN2, executeAfterManualGeneration=True
location='60, 0, 0'
storeIn=IDC2

*step, maxInc=1, minInc=1, maxNumInc=100000, maxIter=25, stepLength=1, solver=NISTPArcLen
setfield,   name=omegaIni,  fieldOutput=alphaDWeak, value=1e-2, type=uniform

*step, maxInc=1e-2, startInc=1e-2, minInc=1e-6, maxNumInc=100000, maxIter=25, stepLength=1, solver=NISTPArcLen
options, category=Ensight, intermediateSaveInterval=1, minDTForOutput=0
options, category=NISTArcLength, arcLengthController=indirectcontrol, stopCondition='fieldOutputs["I1pMax"] > 0.01'

indirectcontrol, dof1='model.nodeSets["IDC1"][0].fields["displacement"]', cVector1='[-1,0,0]', dof2='model.nodeSets["IDC2"][0].fields["displacement"]', cVector2='[1,0,0]', L=1.,

dirichlet, name=leftX, nSet=gen_left,  field=displacement, 1=0.
dirichlet, name=leftY, nSet=gen_left,  field=displacement, 2=0.
dirichlet, name=leftZ, nSet=gen_left,  field=displacement, 3=0.
dirichlet, name=right, nSet=gen_right, field=displacement, 1=1.

*fieldOutput
name=displacement,    create=perNode, elSet=all, field=displacement, result=U
name=nonlocal_damage, create=perNode, elSet=all, field=nonlocal damage, result=U

name=strain, create=perElement, elSet=all, result=strain, quadraturePoint=0:8, f(x)='np.mean(x,axis=1)'
name=stress, create=perElement, elSet=all, result=stress, quadraturePoint=0:8, f(x)='np.mean(x,axis=1)'
name=omega,  create=perElement, elSet=all, result=omega,  quadraturePoint=0:8, f(x)='np.mean(x,axis=1)'
name=alphaP, create=perElement, elSet=all, result=alphaP, quadraturePoint=0:8, f(x)='np.mean(x,axis=1)'
name=alphaD, create=perElement, elSet=all, result=alphaD, quadraturePoint=0:8, f(x)='np.mean(x,axis=1)'
name=I1p,    create=perElement, elSet=all, result=I1p,    quadraturePoint=0:8, f(x)='np.mean(x,axis=1)'

name=I1pMax,    create=perElement, elSet=all, result=I1p,    quadraturePoint=0:8, f(x)='np.max(x)', saveHistory=true
name=alphaDMax, create=perElement, elSet=all, result=alphaD, quadraturePoint=0:8, f(x)='np.max(x)', saveHistory=true
name=omegaMax,  create=perElement, elSet=all, result=omega,  quadraturePoint=0:8, f(x)='np.max(x)', saveHistory=true

name=alphaDWeak, create=perElement, elSet=gen_centerSliceX, result=alphaD, quadraturePoint=0:8

name=U1,  create=perNode, nSet=gen_right, field=displacement, result=U, f(x)='mean(x[:,0])', saveHistory=true, export=U
name=RF1, create=perNode, nSet=gen_right, field=displacement, result=P, f(x)='sum(x[:,0])', saveHistory=true, export=RF

*output, type=ensight, name=test
create=perNode, fieldOutput=displacement
create=perNode, fieldOutput=nonlocal_damage
create=perElement, fieldOutput=omega
create=perElement, fieldOutput=I1p
create=perElement, fieldOutput=alphaP
create=perElement, fieldOutput=alphaD
create=perElement, fieldOutput=stress
create=perElement, fieldOutput=strain
configuration, overwrite=yes

*output, type=meshPlot
figure=1, axSpec=111, create=xyData, x=U1, y=RF1

`indirectcontractioncontrol` - Indirect displacement – contraction ring control

Relevant module: edelweissfe.stepactions.indirectcontrol

Options:
Option	Description
`contractionNSet`	The node set defining the contraction ring
`L`	Final distance (e.g. crack opening)
`exportCVector`	(Optional) file to export the computed c vector

`initializematerial` - Initialize materials

Relevant module: edelweissfe.stepactions.initializematerial

Let materials initialize themselves (e.g., state vars depending on material parameters…) !

`modelupdate` - Update the model

Relevant module: edelweissfe.stepactions.modelupdate

Options:
Option	Description
`update`	Model accessible, executable expression

`nodeforces` - Concentrated node forces

Relevant module: edelweissfe.stepactions.nodeforces

Options:
Option	Description
`nSet`	Node set for application of the boundary condition
`1,2,3,...`	Prescribed values for components of the physical field
`components`	Prescribed values using a np.ndarray for representation; use ‘x’ for ignored values
`field`	Field for which the boundary condition is active
`f(t)`	(Optional) define an amplitude in the step progress interval [0…1]

Example: testfiles/NodeForces/test.inp

*material, name=VonMises, id=mat
210000, 0.3, 550, 1000, 200, 1400

*section, name=section1, thickness=1.0, material=mat, type=plane
all

*job, name=cps4job, domain=2d
*solver, solver=NIST, name=theSolver

*modelGenerator, generator=planeRectQuad, name=gen
x0=0, l=50
y0=0, h=100
elType=CPS4
nX=10
nY=10

*fieldOutput
create=perNode, nSet=gen_bottom, result=P, field=displacement, name=RF
create=perNode, elSet=all, field=displacement, result=U, name=displacement

*output, type=monitor
fieldOutput=RF, f(x)='mean(x[:,1])'

*output, type=ensight, name=esExport
create=perNode, fieldOutput=displacement
configuration, overwrite=yes

*step, maxInc=1e-1, minInc=1e-8, maxNumInc=50, maxIter=25, stepLength=100, solver=theSolver
dirichlet, name=bottom, nSet=gen_bottom,  field=displacement, 2=0, 1=0
nodeforces, name=cloadTop, nSet=gen_top, field=displacement, 2=-50
*step, maxInc=1e-1, minInc=1e-8, maxNumInc=1000, maxIter=25, stepLength=100, solver=theSolver
nodeforces, name=cloadTop, nSet=gen_top, 2=-10, f(t)=sin(t*2*pi)
*step, maxInc=1e-1, minInc=1e-8, maxNumInc=1000, maxIter=25, stepLength=100, solver=theSolver
nodeforces, name=cloadTop, nSet=gen_top, 2=+50, f(t)=t

`setfield` - Set a field to a prescribed value

Relevant module: edelweissfe.stepactions.setfield

Options:
Option	Description
`fieldOutput`	Field output to be set
`type`	‘Const’ or ‘analyticalField’
`value`	Scalar value if type ‘const’; name of analyticalField if type ‘analyticalField’

`setinitialconditions` - Set initial conditions to elements

Relevant module: edelweissfe.stepactions.setinitialconditions

Pass initial conditions to elements.

Options:
Option	Description
`property`	The name of the property to be initialized
`values`	The property values
`elSet`	(Optional) the element set for which the initaliziation is performed

Implementing your own step actions

Subclass from the step action base class in module edelweissfe.stepactions.base.stepactionbase

class edelweissfe.stepactions.base.stepactionbase.StepActionBase(name, definition, jobInfo, model, fieldOutputController, dofmanager, journal)[source]

This is the abase class for all step actions. User defined step actions can override the methods.

Parameters

name (str) – The name of this step action.
definition (dict) – A dictionary containing the options for this step action.
jobInfo (dict) – A dictionary containing the information about the job.
model (FEModel) – A dictionary containing the model tree.
fieldOutputController (FieldOutputController) – The fieldput controlling object.
journal (Journal) – The journal object for logging.

Methods

`applyAtIncrementStart`(model, timeStep)	Is called when a step increment starts.
`applyAtStepEnd`(model)	Is called when a step successfully finished.
`applyAtStepStart`(model)	Is called when a step starts.
`updateStepAction`(definition, jobInfo, model, ...)	Is called when an updated definition is present for a new step.

applyAtIncrementStart(model, timeStep)[source]

Is called when a step increment starts.

Parameters

U_n – The current converged solution vector at start of the increment.
P – The current reaction force vector.
increment – The defintion of the time increment.
timeStep (TimeStep) –

applyAtStepEnd(model)[source]

Is called when a step successfully finished.

Parameters

U – The current solution vector.
P – The current reaction force vector.

applyAtStepStart(model)[source]

Is called when a step starts.

Parameters

U – The current solution vector.
P – The current reaction force vector.

updateStepAction(definition, jobInfo, model, fieldOutputController, dofmanager, journal)[source]

Is called when an updated definition is present for a new step.

Parameters

name – The name of this step action.
definition (dict) – A dictionary containing the options for this step action.
jobInfo (dict) – A dictionary containing the information about the job.
model (FEModel) – A dictionary containing the model tree.
fieldOutputController (FieldOutputController) – The fieldput controlling object.
journal (Journal) – The journal object for logging.

Step actions

bodyforce - Bodyforce loads

dirichlet - Standard dirichlet BC

distributedload - Distributed surface loads

geostatic - Geostatic stress states

indirectcontrol - Indirect displacement control

indirectcontractioncontrol - Indirect displacement – contraction ring control

initializematerial - Initialize materials

modelupdate - Update the model

nodeforces - Concentrated node forces

setfield - Set a field to a prescribed value

setinitialconditions - Set initial conditions to elements

Implementing your own step actions

`bodyforce` - Bodyforce loads

`dirichlet` - Standard dirichlet BC

`distributedload` - Distributed surface loads

`geostatic` - Geostatic stress states

`indirectcontrol` - Indirect displacement control

`indirectcontractioncontrol` - Indirect displacement – contraction ring control

`initializematerial` - Initialize materials

`modelupdate` - Update the model

`nodeforces` - Concentrated node forces

`setfield` - Set a field to a prescribed value

`setinitialconditions` - Set initial conditions to elements