DG shell boundary conditions

Since shell formalism only takes displacements into account, rotating boundary conditions are imposed though a DG formulation.

Materials

As for boundary condition elements, there is no material to associate to an element.

Elements

Since no material is required, the first stage consists in defining an ElementProperties:

prp = ElementProperties(typeEl)
prp.put(param1, value1)
prp.depend(param1, fct1, Lock1)) #facultatif
...

where

`typeEl`	desired type of element (for example `BoundaryDgShellFirstDegreeElement`)
`param1`	name of the property associated to the element (for example `STIFFMETHOD`)
`value1`	value of the corresponding property
`fct1`	function which characterizes the dependency of the property (optional: no fct if no dependency)
`Lock1`	Lock which defines the dependency variable of the property (compulsory if there is a dependency)

BoundaryDgShellFirstDegreeElement

DG interface element to insert on shell boundaries to provide BCs. These are 2-nodes linear lines, but they are interfering over all neighboring dofs.

By default, stresses are integrated over dim*2 integration points. The material used is dgShellMaterial.

BoundaryDgShellSecondDegreeElement

Same as BoundaryDgShellFirstDegreeElement, but 8-nodes second order shell element.

BoundaryDgShellNineNodeSecondDegreeElement

Same as BoundaryDgShellSecondDegreeElement, but 9-nodes second order shell element.

BoundaryDgShellSixteenNodeThirdDegreeElement

Same as BoundaryDgShellNineNodeSecondDegreeElement, but 16-nodes third order shell element.

Parameters of shell boundary conditions elements

Name	Metafor Code	Dependency
`MATERIAL`	Number of the material to consider	-
`STIFFMETHOD`	Method used to compute the stiffness matrix = `STIFF_ANALYTIC` : analytic matrix (default) = `STIFF_NUMERIC` : numerical matrix	-
`BENDING_NPG`	Number of integration points along one direction for bending solving = 2 classical solving (second order) = 3 EAS solving with 22 or 7 added modes (8 or 9-nodes second order) = 4 solving without EAS (16-nodes third order)	-
`NORMAL_PT1`	First point governing the element of the shell normal	-
`NORMAL_PT2`	First point governing the element of the shell normal	-

Interactions

Once created, the element is generated by a DgShellInteraction:

dgBound = DgShellInteraction(number)
dgBound.push(gObject1)
dgBound.push(gObject2)
...
dgBound.addProperty(prp)
interactionset.add(dgBound)  # the interaction is added in InteractionSet

or

dgBound = interactionset.add( DgShellInteraction(number) )
dgBound.push(gObject1)
dgBound.push(gObject2)
...
dgBound.addProperty(prp)

`number`	Number of the material to consider
`gObject1`, `gObject2`	mesh geometric entities
`prp`	Properties of the DG boundary condition elements to generate

Generally, entities are lines or groups of nodes on a line.

Table of Contents