Constraints

Constraints are defined globally, and may be used for introducing additional scalar equations into the global equation system.

Example syntax:

*constraint, type=rigidbody, name=myRigigBody
    nSet=right
    referencePoint=rBottom

equalvaluelagrangian - Constrain nodal values to equal values

Module edelweissfe.constraints.equalvaluelagrangian

Options:

Option

Description
field

The field this constraint acts on.
component

The component of the field.
nSet

The node set to be constrained.
Example: testfiles/EqualValueLagrangianConstraint/test.inp
*modelGenerator, generator=planeRectQuad, name=gen
elType=CPS8R
nX=20
nY=20
l=100
h=100

*constraint, type=equalValueLagrangian, name=myConstraint
nSet=gen_top
field=displacement
component=1

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

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

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

*fieldOutput
create=perNode, name=displacement, elSet=all, field=displacement, result=U,
create=perNode, name=RF, nSet=gen_bottom, field=displacement, result=P,
create=perElement, name=stress, elSet=all, result=stress, quadraturePoint=0:4, f(x)='mean(x, axis=1)'
create=perElement, name=strain, elSet=all, result=strain, quadraturePoint=0:4, f(x)='mean(x, axis=1)'

*output, type=monitor, name=theMonitor
fieldOutput = RF, f(x) = 'sum ( x, axis=0)'

*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=bottom, nSet=gen_bottom, field=displacement, 1=0.0, 2=0.0
dirichlet, name=load, nSet=gen_rightTop, field=displacement, 1=5.0, 2=5.0

equalvaluepenalty - Constrain nodal values to equal values

Module edelweissfe.constraints.equalvaluepenalty

Options:

Option

Description
field

The field this constraint acts on.
component

The component of the field.
penalty

The numerical penalty value.
nSet

The node set to be constrained.
Example: testfiles/EqualValuePenaltyConstraint/test.inp
*modelGenerator, generator=planeRectQuad, name=gen
elType=CPS8R
nX=20
nY=20
l=100
h=100

*constraint, type=equalValuePenalty, name=myConstraint
nSet=gen_top
field=displacement
component=1
penalty=1e8

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

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

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

*fieldOutput
create=perNode, name=displacement, elSet=all, field=displacement, result=U,
create=perNode, name=RF, nSet=gen_bottom, field=displacement, result=P,
create=perElement, name=stress, elSet=all, result=stress, quadraturePoint=0:4, f(x)='mean(x, axis=1)'
create=perElement, name=strain, elSet=all, result=strain, quadraturePoint=0:4, f(x)='mean(x, axis=1)'

*output, type=monitor, name=theMonitor
fieldOutput = RF, f(x) = 'sum ( x, axis=0)'

*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=bottom, nSet=gen_bottom, field=displacement, 1=0.0, 2=0.0
dirichlet, name=load, nSet=gen_rightTop, field=displacement, 1=5.0, 2=5.0

linearizedrigidbody - Linearized rigid body constraints

Module edelweissfe.constraints.linearizedrigidbody

Options:

Option

Description
nSet

(Slave) node set, which is constrained to the reference point
referencePoint

(Master) reference point
Example 2D: testfiles/LinearizedRigidBodyConstraint/test.inp
*modelGenerator, generator=planeRectQuad, name=gen
l=100
h=10
nX=15
nY=5
elType=CPS4

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

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

*job, name=cps4job, domain=2d
*solver, solver=NIST, name=theSolver
*fieldOutput
create=perNode, name=load,  nSet=gen_left, field=displacement, result=P, f(x)='sum(x[:,1])'
create=perNode, name=displacement, elSet=all, field=displacement, result=U, name=displacement


*output, type=monitor
fieldOutput=load

*constraint, type=linearizedRigidBody, name=rb1
nSet=gen_right
referencePoint=gen_rightTop

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

*step, solver=theSolver, maxInc=1e-1, minInc=1e-4, maxNumInc=1000, maxIter=4
options, category=NISTSolver, extrapolation=linear
dirichlet, name=leftCorner,  nSet=gen_leftBottom, field=displacement, 1=0.0, 2=0.0
dirichlet, name=rotRP,  nSet=gen_rightTop,   field=rotation, 1=0.05
dirichlet, name=movRP,  nSet=gen_rightTop,   field=displacement, 2=0.00
Example 2D: testfiles/LinearizedRigidBodyConstraint2D/test.inp
*modelGenerator, generator=planeRectQuad, name=gen
l=100
h=10
nX=15
nY=5
elType=CPS4

*node, nSet=RP
999999, 150, 5

*material, name=linearElastic, id=myMaterial
30000.0, 0.15

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

*job, name=myJob, domain=2d

*solver, solver=NIST, name=theSolver

*fieldOutput
create=perNode, name=load,  nSet=gen_left, field=displacement, result=P, f(x)='sum(x[:,1])'
create=perNode, name=displacement, elSet=all, field=displacement, result=U, name=displacement

*output, type=monitor
fieldOutput=load

*constraint, type=linearizedRigidBody, name=fixedSupport
nSet=gen_left
referencePoint=gen_leftTop

*constraint, type=linearizedRigidBody, name=pinnedSupport
nSet=gen_right
referencePoint=RP

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

*step, solver=theSolver, maxInc=1e-1, minInc=1e-4, maxNumInc=1000, maxIter=4
options, category=NISTSolver, extrapolation=linear
dirichlet, name=rotFixedSupport,  nSet=gen_leftTop,   field=rotation, 1=0
dirichlet, name=movFixedSupport,  nSet=gen_leftTop,   field=displacement, 1=0, 2=0
dirichlet, name=movPinnedSupport,  nSet=RP,   field=displacement, 1=0, 2=0

*step, solver=theSolver, maxInc=1e-1, minInc=1e-4, maxNumInc=1000, maxIter=4
options, category=NISTSolver, extrapolation=linear
distributedload, name=loadTop, surface=gen_top, type=pressure,  magnitude=10.0, f(t)=1
Example 3D: testfiles/LinearizedRigidBodyConstraint3D/test.inp
*modelGenerator, generator=boxGen, name=gen
lX=100
lY=10
lZ=10
nX=15
nY=5
nZ=5
elType=C3D8

*node, nSet=RP
999999, 150, 5, 5

*material, name=linearElastic, id=myMaterial
30000.0, 0.15

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

*job, name=myJob, domain=3d

*solver, solver=NIST, name=theSolver

*fieldOutput
create=perNode, name=load,  nSet=gen_left, field=displacement, result=P, f(x)='sum(x[:,1])'
create=perNode, name=displacement, elSet=all, field=displacement, result=U, name=displacement

*output, type=monitor
fieldOutput=load

*constraint, type=linearizedRigidBody, name=fixedSupport
nSet=gen_left
referencePoint=gen_topLeftBack

*constraint, type=linearizedRigidBody, name=pinnedSupport
nSet=gen_right
referencePoint=RP

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

*step, solver=theSolver, maxInc=1e-1, minInc=1e-4, maxNumInc=1000, maxIter=4
options, category=NISTSolver, extrapolation=linear
dirichlet, name=rotFixedSupport,  nSet=gen_topLeftBack,   field=rotation, 1=0, 2=0, 3=0
dirichlet, name=movFixedSupport,  nSet=gen_topLeftBack,   field=displacement, 1=0, 2=0, 3=0
dirichlet, name=movPinnedSupport,  nSet=RP,   field=displacement, 1=0, 2=0, 3=0

*step, solver=theSolver, maxInc=1e-1, minInc=1e-4, maxNumInc=1000, maxIter=4
options, category=NISTSolver, extrapolation=linear
distributedload, name=loadTop, surface=gen_top, type=pressure,  magnitude=10.0, f(t)=1
dirichlet, name=rotation,  nSet=RP,   field=rotation, 2=0.1

rigidbody - Geometrically exact rigid body constraints in 3D

Module edelweissfe.constraints.rigidbody

Options

Option

Description
nSet

(slave) node set, which is constrained to the reference point
referencePoint

(master) reference point
Example: testfiles/RigidBodyConstraintLargeDeformations3D/test.inp
*include, input=mesh.inp

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

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

*job, name=c3d8job, domain=3d
*solver, solver=NISTParallel, name=theSolver
*fieldOutput
create=perNode, name=displacement, elSet=all, field=displacement, result=U, name=displacement
create=perElement, name=stress, elSet=all, result=stress, f(x)=' mean(x, axis=1) ', quadraturePoint=0:8

*constraint, type=rigidbody, name=rb1
nSet=right
referencePoint=rBottom

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

*step, solver=theSolver, maxInc=2e-1, minInc=1e-4, maxNumInc=1000, maxIter=10
options, category=NISTSolver, extrapolation=linear
dirichlet, name=left,  nSet=left,         field=displacement, 1=0.0, 2=0, 3=0
dirichlet, name=rotRP,  nSet=rBottom,   field=rotation, 1=3.141,

penaltyindirectcontrol - Penalty based indirect control

Module edelweissfe.constraints.penaltyindirectcontrol

Options

Option

Description
field

The field this constraint acts on
cVector

The projection vector for the constrained nodes (e.g., CMOD)
constrainedNSet

The node set for determining the constraint (e.g., CMOD)
loadNSet

The node set for application of the controlled load
loadVector

The vector (in correct) dimensions and tensorial order determining the load
length

The value of the constraint (e.g., CMOD)
penaltyStiffness

The stiffness for formulating the constraint
offset

(Optional) a correction value for the computation of the constraint (e.g, initial displacement)
normalizeLoad

(Optional) normalize the applied force per node wrt. the number of nodes, i.e., apply a load irrespective of the total number of nodes in ``loadNSet``
Example: testfiles/PenaltyBasedIndirectControl/test.inp
*material, name=LinearElastic, id=myMaterial
**Isotropic
**E    nu
1000, 0.2

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

*modelGenerator, generator=planerectquad, name=gen
nX      =5
nY      =5
l      =20
h      =50
elType  = CPE4

*section, name=section1, material=myMaterial, type=plane, thickness=1
all

*fieldOutput
create=perNode, elSet=all, field=displacement, result=U, name=displacement
create=perNode, nSet=gen_top, field=displacement, result=U, name=disp_top
create=perNode, nSet=gen_bottom, field=displacement, result=P, name=RF
create=perElement, elSet=all, result=strain, name=strain, quadraturePoint=0:4, f(x)='np.mean(x,axis=1)'
create=perElement, elSet=all, result=stress, name=stress, quadraturePoint=0:4, f(x)='np.mean(x,axis=1)'

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

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

*nset, nset=measurement_nodes
gen_leftBottom
gen_leftTop

*constraint, type=penaltyindirectcontrol, name=pc1
field=displacement
cVector='0, 1, 0, -1'
constrainedNSet=measurement_nodes
loadNSet=gen_rightTop
loadVector='0, -1'
length=-1
penaltyStiffness=1e8
offset=0

*step, solver=theSolver, maxInc=1e0, minInc=1e0, maxNumInc=100, maxIter=25, stepLength=1
modelupdate, update='model.constraints["pc1"].active=False'
dirichlet,  name=fix_bottom, nSet=gen_bottom, field=displacement, 1=0, 2=0

*step, solver=theSolver, maxInc=2e-2, minInc=1e-6, maxNumInc=1000, maxIter=25, stepLength=1
modelupdate, update='model.constraints["pc1"].active=True'

Implementing your own constraints

Subclass from the constraint base class in module edelweissfe.constraints.base.constraintbase

class edelweissfe.constraints.base.constraintbase.ConstraintBase(name, options, model)[source]

The constraint base class.

Constraints can act on nodal variables, and scalar variables. If scalar variables are required, the can be created on demand by defining getNumberOfAdditionalNeededScalarVariables() and assignAdditionalScalarVariables(), which are called at the beginning of an analysis.

If scalar variables are used, EdelweissFE expects the layout of the external load vector PExt (and the stiffness) to be of the form

[ node 1 - dofs field 1,
  node 1 - dofs field 2,
  node 1 - ... ,
  node 1 - dofs field n,
  node 2 - dofs field 1,
  ... ,
  node N - dofs field n,
  scalar variable 1,
  scalar variable 2,
  ... ,
  scalar variable J ].
Parameters

  • name (str) – The name of the constraint.

  • options (dict) – A dictionary containing the options for the constraint.

  • model (FEModel) – A dictionary containing the model tree.

Attributes
fieldsOnNodes

The fields on the nodes this constraint is acting on.

nDof

The total number of degrees of freedom this constraint is associated with.

nodes

The nodes this constraint is acting on.

Methods

applyConstraint(U_np, dU, PExt, V, timeStep)

Apply the constraint.

assignAdditionalScalarVariables(scalarVariables)

Assign a list of scalar variables associated with this constraint.

getNumberOfAdditionalNeededScalarVariables()

This method is called to determine the additional number of scalar variables this Constraint needs.
abstract applyConstraint(U_np, dU, PExt, V, timeStep)[source]

Apply the constraint. Add the contributions to the external load vector and the system matrix.

Parameters

  • U_np (ndarray) – The current total solution vector.

  • dU (ndarray) – The current increment since the last time the constraint was applied.

  • PExt (ndarray) – The external load vector.

  • K – The system (stiffness) matrix.

  • dT – The time increment.

  • time – The current step and total time.

  • V (ndarray) –

  • timeStep (TimeStep) –

assignAdditionalScalarVariables(scalarVariables)[source]

Assign a list of scalar variables associated with this constraint.

Parameters
getNumberOfAdditionalNeededScalarVariables()[source]

This method is called to determine the additional number of scalar variables this Constraint needs.

Returns

Number of ScalarVariables required.

Return type

int

abstract property fieldsOnNodes: list

The fields on the nodes this constraint is acting on.

abstract property nDof: int

The total number of degrees of freedom this constraint is associated with.

abstract property nodes: list

The nodes this constraint is acting on.