Next: Beam Section Types
Up: Element Types
Previous: One-node mass element (MASS)
Contents
The user can define his/her own elements. In order to do so he/she has to:
- Give a name to the element. The name has to start with ``U'' followed by
maximal 4 characters. Any character from the ASCII character set can be
taken, but please note that lower case characters are converted into upper
case by CalculiX. Consequently, ``Ubeam'' and ``UBEam'' are the same
name. This reduces the character set from 256 to 230 characters.
- specify the number of integration points within the element, the number
of nodes belonging to the element and the number of degrees of freedom in
each node by using the *USER ELEMENT keyword card.
- write a FORTRAN subroutine resultsmech_uxxxx.f calculating the secondary
variables (usually strains, stresses, internal forces) from the primary
variables (= the solution of the equation system, usually displacements,
rotations....). Add a call to this routine in resultsmech_u.f
- write a FORTRAN subroutine e_c3d_uxxxx.f calculating the element stiffness
matrix and the element external force vector (and possibly the element mass
matrix). Add a call to this routine in e_c3d_u.f
- write a FORTRAN subroutine extrapolate_uxxxx.f calculating the value of
the secondary variables (usually strains, stresses..) at the nodes based on
their values at the integration points within the element. Add a call to
this routine in extrapolate_u.f
An example for a 3D Timoshenko beam element (for static linear elastic
calculations and small deformations) according to [79] is
implemented as element ``U1'' in CalculiX. It is used in example userbeam.inp
in the test suite. The reader is referred to files resultsmech_u1.f,
e_c3d_u1.f and extrapolate_u1.f for details on how a user elements is coded.
Next: Beam Section Types
Up: Element Types
Previous: One-node mass element (MASS)
Contents
guido dhondt
2017-10-08