**deformation

Description

This boundary condition imposes the displacement vector \(\vect v\) of a node by the following formula:

(31)\[\vect u = \ten \varepsilon \vect r\]

where \(\ten \varepsilon\) is a symmetric tensor, and \(\vect r\) the position vector of the node considered. The origin of \(\vect r\) may be a fixed point or a node of the mesh.

For the case where the origin is a fixed point the node set considered must be given, as well as the position of the origin point in the form of a vector, and the components of the tensor \(\bf \varepsilon\). In 1D \(\varepsilon_{11}\) and \(\varepsilon_{22}\) may be imposed; in 2D \(\varepsilon_{12}\) may be added; in 3D the remaining \(\varepsilon_{33}\), \(\varepsilon_{13}\), and \(\varepsilon_{23}\) terms may be added. The tensor components are respectively named E11, E22, E12, E33, E13, and E23. If a component is not defined its value is set to zero. The values may be set by using a table for all of the components, or a table for each individual component (only for non-zero components).

Syntax

**deformation  [ node ] \(~\,~\,\) nset_name (vec | num_node) \(~\,~\,\) compos_name value [ table ] … compos_name value \(~\,\) [ table ]

node

is an optional keyword indicating that the origin of \(\vect r\) is a node of the mesh.

nset_name

Character name of the nset group upon which the displacement will be imposed.

vec

Position of the origin point in the form of a vector. This is in the case where the center is not a node of the mesh. Recall the vector form is 2 or three real values enclosed in parenthesis such as ( 1. 0. 0. ).

num_mode

Integer number of a node in the case where the node keyword was given.

compos_name value

Character string giving the name of a component of the \(\ten \varepsilon\) tensor as defined above, followed by a real giving the components value. Any number of these components may be given in any order thereby specifying the deformation tensor.

table

character name of the table(s) used to describe the field amplitude. See the command ***table.

Example

This example shows a simple uniform deformation field to an initially square multi-element mesh. The required BC input data is the following (see test deform in $Z7PATH/TESTS/Static_test/):

**deformation
  boundary (0. 0.) E22 0.1  E11 0.1 E12 .3 tab

where tab is a unit table definition given after. The resulting deformed structure is displayed below. This type of condition is useful for testing the mechanical behavior of materials under complex strain loadings.

Another imposed strain field is given below:

**deformation node
   nsetdef 2 E11 2. E33 4. tab