====== Shells======

===== Materials =====

The definition of shell finite elements follows the same logic as volume elements. First, a material is defined: 

  materialno = materialset.define (number, type)
  materialno = materialset(number)
  materialno.put(param, value)
  materialno.depend(param, fct, Key(Lock)))
  ...

|''number'' | material number (must be unique with respect to all elements in ''materialset'', not to shells) |
|''type'' | shell type (for example ''LinearShellMaterial'') |
|''param'' | name of the shell parameter (for example ''ELASTIC_MODULUS'') |
|''value'' | value of the corresponding parameter ''param''|
|''fct'' | function which characterizes the dependency of the property (optional: no fct if no dependency) |
|''Lock'' | [[doc:user:general:locks|Lock]] which defines the dependency variable of the property (compulsory if there is a dependency) |


====  LinearShellMaterial ====

=== Description ===

Simple linear elastic law (small strains and displacements).

=== Parameters ===
^   Name                                          ^     Metafor Code     ^  Dependency ^
| Density                                         |   ''MASS_DENSITY''    |              |
| Young modulus                                   |  ''ELASTIC_MODULUS''  |              |
| Poisson ratio                                   |   ''POISSON_RATIO''   |              |

===== Elements =====

After defining the [[#Materials|material]], it must be associated to an ''[[doc:user:elements:general:def_element_properties|ElementProperties]]'':

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

where

|''typeEl'' | desired element (for example ''LinearShellFirstDegreeElement'')|
|''param1''| name of the property associated to the element (for example ''MATERIAL'' to associate the desired material)|
|''value1''| value of the corresponding property |
|''fct1''| function which characterizes the dependency of the property (optional: no fct if no dependency) |
|''Lock1''| [[doc:user:general:locks|Lock]] which defines the dependency variable of the property (compulsory if there is a dependency) |

====  LinearShellFirstDegreeElement ====

Linear shell elements (small strains small displacements). 4-nodes linear quadrangles.

By default, stresses are integrated of ''dim*2'' integration points. 

A thickness must be defined, see table below.


====  LinearShellSecondDegreeElement ====

Same as ''LinearShellFirstDegreeElement'' but based on a second order mesh ([[doc:user:geometry:mesh:2d]]).

The membrane part can be integrated over ''dim*3'' integration points, considering EAS modes, see table below.
The bending part can be integrated over ''dim*3'' integration points, considering EAS modes, see table below.



====  LinearShellNineNodeSecondDegreeElement ====

Same as ''LinearShellSecondDegreeElement'' but based on a 9-nodes second order mesh ([[doc:user:geometry:mesh:2d]]).

The membrane part can be integrated over ''dim*3'' integration points, considering EAS modes, see table below.
The bending part can be integrated over ''dim*3'' integration points, considering EAS modes, see table below.


====  LinearShellSixteenNodeThirdDegreeElement ====

Same as ''LinearShellNineNodeSecondDegreeElement'' but based on a 16-nodes third order mesh ([[doc:user:geometry:mesh:2d]]).

The membrane part can be integrated over ''dim*4'' integration points, without EAS modes (no locking), see table below.
The bending part can be integrated over ''dim*4'' integration points, without EAS modes (no locking), see table below.


=== Parameters ===
^   Name                                             ^     Metafor Code     ^  Dependency ^
| ''MATERIAL''    | Number of the shell material to consider             |  -  |
| ''STIFFMETHOD'' | Method used to compute the stiffness matrix \\ = ''STIFF_ANALYTIC'' : analytic matrix (default) \\ = ''STIFF_NUMERIC''  : numerical matrix           |  -  |
| ''GRAVITY_X'' / ''GRAVITY_Y'' / ''GRAVITY_Z'' | gravity  |  time |
| ''THICKNESS'' | initial thickness  |  -  |
| ''MEMBRANE_NPG'' | Number of integration points along one direction for membrane solving \\ = 2 classical solving  (second order)\\ = 3 EAS solving with 11 or 13 added modes (8 or 9-nodes second order)\\ = 4 solving without EAS (16-nodes third order)  |  -  |
| ''BENDING_NPG''  | Number of integration points along one direction for membrane 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)  |  -  |

===== Interactions =====

Shell elements are then generated as [[doc:user:elements:volumes:volumeelement|volume elements]], using a ''FieldApplicator'' interaction. Then, they must be completed with a [[doc:user:elements:shells:interface|DG interface element]] to be consistent.

  app = FieldApplicator(no)
  app.push(gObject1)
  app.push(gObject2)
  ...
  app.addProperty(prp)        # association of an ElementProperties
  interactionset.add(app)     #  the interaction is added in InteractionSet 

or

  app = interactionset.add(FieldApplicator(no)) #add returns a reference
  app.push(gObject1)
  app.push(gObject2)
  ...
  app.addProperty(prp)        # association of an ElementProperties


where 
| ''no''  | number of the ''Interaction'' (which is to say the ''FieldApplicator'') | 
|''gObject1''  | mesh geometric entity where the finite elements are applied |
| ''prp'' | [[doc:user:elements:general:def_element_properties|Properties]] of shell elements to generate.|