## *REFINE MESH

Keyword type: step

With this keyword a user-defined part of the input mesh consisting of C3D4 and C3D10 elements is refined according to certain criteria and the calculation is automatically restarted with the refined mesh. Temperatures, volumetric distributed loading (e.g. centrifugal forces), point loads and single point constraints are automatically modified. This does not apply to facial distributed loads and multiple point constraints. These should not be applied to the part of the mesh to be refined. To determine the temperatures in the new mesh interpolation based on the unrefined mesh is done. For the point forces and single point constraints the definition in the unrefined mesh is kept and multiple point constraints are constructed between the concerned nodes in the old mesh and the tetrahedrons in the new mesh within which they are located.

The refinement is done in the step in which *REFINE MESH is used and is based on the results calculated in that step. The keyword should occur at most once in the complete input deck.

For the refinement the available criteria are the size of the displacements (label U), the velocity (label V), the stress (label S), the total strain (label E), the mechanical strain (label ME), the equivalent plastic strain (label PEEQ), the energy density (label ENER), the heat flux (label HFL), the gradient based error estimator (label ERR) or a user-defined function (user subroutine ucalculateh.f). The size is defined as the absolute value if it concerns a scalar quantity and the norm if it concerns a vector or tensor.

There is one required parameter LIMIT and two optional parameters ELSET and USER.

With the parameter LIMIT the user defines a positive value above which refinement is requested. For instance, if the limit is 50. and the value of the selected criterion is 200. a refinement by a factor of 4 is aimed at. The refinement is done iteratively (5 times), and each iteration induces a maximum refinement by a factor of 2.

The parameter ELSET allows the user to define an element set (which should consist of C3D4 and/or C3D10 elements only) to be refined. All other elements (no matter whether tetrahedral or not) are not changed. Notice that the interface between the part of the mesh to be refined and its complement is not changed, so multiple point constraints describing this interface still work after refinement. The element set name should not be longer than 60 characters.

With the parameter USER a new criterion for the refinement can be coded in user subroutine ucalculateh.f.

If the tetrahedral mesh in the input deck contains at least one quadratic element, the refined mesh contains C3D10 elements only, else it is a pure C3D4 mesh.

First line:

• *REFINE MESH.
• enter the required parameter LIMIT and its value and any other optional parameter.

Second line:

• the label of the selected criterion.

Example:

*REFINE MESH,LIMIT=50.
S


requests a refinement based on the size of the stress and a limit of 50.

Example files: circ10p.