**positive_displacement

Description

This boundary condition is used to ensure \(U.v \ge 0\), where \(v\) is the direction along which the positive displacement must be verified. This is very similar to a contact problem, and it works by creating a node-to-rigid contact element, as described in the PhD thesis of M. Barboteu.

“Contact, frottement et techniques de calcul parallèle”, M. Barboteu, Université de Montpellier, France, March 1st, 1999 (see pages 24–26).

The additional DOFs are named PD.

Note that one has to use the extended convergence info, since this BC involves additional degrees of freedom which are forces (and not displacement). This boundary conditions only works in 2D.

Syntax

The syntax required to positive_displacement is:

**positive_displacement \(~\,~\,\) nset_name  dir

nset_name

is the name of the nset on which the boundary condition is to be imposed.

dir

is the direction along which the positive displacement is imposed.

Example

This example assumes that a mesh with nsets ligament, lip and top have previously been created. It simulates a cracked plate under tension. The crack lip is denoted as lip. This positive displacement is imposed on the nset lip to avoid the crack to close and subsequent mesh inter-penetration in the crack lip region.

 ***mesh plane_stress
[...]
 ***resolution
  **sequence
   *time 600.
   *increment 1000
   *algorithm p1p2p3
   *ratio (U:.05   absolu EZ:1.e-6   PD:1.e-8)

  ***bc
   **impose_nodal_dof
     ligament U2 0.
   **pressure
     top 400. load_cycle
   **positive_displacement lip 0. 1.

In this example, the DOF PD is attached to the positive displacement BC, and EZ appears because of the plane_stress formulation.