====== Pressure and shear  (Metafor > v3593) ======
<note important>
This Documentation refers to Metafor version >= 3593.
for more informations on changes see [[https://gitlab.uliege.be/am-dept/MN2L/oo_meta/-/merge_requests/167|MR !167]] for technical informations). 

for a Metafor version < 3593, please refers to this [[pressure_shear_pre3593|page]].
</note>

Pressure and shear boundary conditions can be applied using special finite elements defined on the boundary of the mesh. The geometry of these elements are lines in 2D corresponding to the boundary edges of the elements of the 2D mesh.
In 3D, pressure elements are triangles or quads, depending of the shape of the facets of the elements of the mesh near the boundary.

As any finite element, their definition requires an ''[[doc:user:elements:general:def_element_properties|ElementProperties]]'' object and an ''Interaction'' (''LoadingInteraction'') and a ''Material''.

The ''[[doc:user:elements:general:def_element_properties|ElementProperties]]'' contains the type of element and integration parameters (number of integration points, stiffness computation method, ...).
The ''PressureMaterial'' contains the values for the pressure and the shear, as well as functions defining the time / space evolution of these values. 

These elements should not be mixed with [[doc:user:conditions:dead_loads|dead loads]]. In most cases, pressure elements should be chosen over dead loads because:

    * Pressure and shear are always defined in local axes, so the direction of the resulting force depends on the orientation of the boundary edge/face on which it is applied.
    * Pressure is distributed properly over all edges/faces on which the ''LoadingInteraction'' is applied. Consequently, the total applied force does not depend on the mesh. 

{{ doc:user:pressure.gif |Pressure Elements}}

===== Element =====

The first step consists in defining an ''[[doc:user:elements:general:def_element_properties|ElementProperties]]'', as

  prp = ElementProperties(typeEl)
  prp.put(param, value)
  
where
| ''typeEl'' | desired element (for example ''Pressure[2|3]DElement'' - see below)  |
| ''param'' | name of the property associated to the element (e.g. ''NIP'') |
| ''value'' | value of the corresponding property (e.g. the Number of Integration Points)  |
  
  mat = materset.define(no, PressureMaterial)
  mat.put(param, value)
  mat.depend(param, fct, lock)) # optional
  ...

where
| ''param'' | name of the property associated to the material (e.g. ''PRESSURE'') |
| ''value'' | value of the corresponding property (e.g. value for the pressure)  |


==== PressureMaterial ====
Material for Pressure Elements 
=== Parameters ===
^   Name                                          ^     Description       ^  Dependency ^
| ''PRESSURE''  | Pressure on the entity on which the propriety is applied | time (TM)  \\ position (TX/TY/TZ)  |
| ''SHEAR_KSI'' | Shear along $\xi$ (related to element) on the entity on which the propriety is applied | time (TM) \\ position (TX/TY/TZ)  |
| ''SHEAR_ETA'' | Shear along $\eta$ (related to element) on the entity on which the propriety is applied \\ only usefull for ''Pressure3DElement'' | time (TM) \\ position (TX/TY/TZ)  |


==== Pressure2DElement, Pressure3DElement ====

Pressure/shear element for a mesh made of triangles/quadrangles in 2D or hexahedra in 3D.

=== Parameters ===
^   Name                                          ^     Description       ^  Dependency ^
| ''STIFFMETHOD'' | Method used to compute the stiffness matrix\\ = ''STIFF_ANALYTIC'' : analytic matrix (default)\\ = ''STIFF_NUMERIC''  : numerical matrix  |  -  |
| ''MATERIAL''    | Number of the ''PressureMaterial''  to consider  |
| ''NIP''         | Number of integration points by direction (default : 2D 2 / 3D 2x2)    |  -  |



==== TrianglePressure3DElement ====

Pressure/shear element for a mesh made of tetrahedra

=== Parameters ===
^   Name                                          ^     Description       ^  Dependency ^
| ''STIFFMETHOD'' | Method used to compute the stiffness matrix\\= ''STIFF_ANALYTIC'' : analytic matrix (default)\\ = ''STIFF_NUMERIC''  : numerical matrix \\ Not applicable, only the numerical one exists ! |  -  |
| ''MATERIAL''    | Number of the ''PressureMaterial''  to consider  |
| ''NIP''         | Total number of integration points (default : 1)    |  -  |


==== ContactPressure2DElement, ContactPressure3DElement ====

Derivations of ''Pressure2DElement'' and ''Pressure3DElement'' with the possibility to set the pressure/shear force of a node to zero, when this node is in contact within a specified contact interaction.  
To determine the contact status, the contact flag of the previous time step is used.

=== Parameters ===

The same than in Traction2DElement and Traction3DElement, with the following additional parameters:

^  Name  ^  Description  ^  Dependency  ^
| ''NUM_CONTACT_INTERACTION''   | Number of the contact interaction, which is tested for the contact status |  -  |
| ''TRACTION_AT_TRANSITION_ON'' | If ''True'' (default), the traction of a node belonging to an element at the transition from contact to no contact is not set equal to zero, although the node is in contact  |  -  |

{{ :doc:user:elements:boundaries:tractionattransition.png?600 |}}



===== Interaction =====

The interaction used for pressure/shear element is a ''LoadingInteraction''. It is defined as:

  load = LoadingInteraction(no)
  load.push(gObject1)
  load.push(gObject2)
  ...
  load.addProperty(prp)
  interactionset.add(load)

where

| ''no''                      | number of the ''Interaction''  | 
| ''gObject1'', ''gObject2''  | meshed geometric entity where the boundary conditions are applied (one part of the boundary of the mesh)  | 
| ''prp''                     | [[doc:user:elements:general:def_element_properties|Properties]] of [[#Element|boundary condition elements]] to be generated  |