- Mapdl.usrelem(nnodes='', ndim='', keyshape='', nreal='', nsavevars='', nrsltvar='', keyansmat='', nintpnts='', kestress='', keysym='', **kwargs)#
Specifies the characteristics of the user-defined element USER300.
APDL Command: USRELEM
The number of nodes.
The number of dimensions (of nodal coordinates). Valid values are 2 or 3.
One of the following element shape options:
- ANYSHAPE - Any shape (that is, no specified shape). This value is the default. (The ANSYS
MeshTool is unavailable.)
POINT - Point.
LINE - Straight line.
TRIAN - Triangle.
QUAD - Quadrilateral. This shape can be degenerated to a triangle.
TET - Tetrahedron.
BRICK - Brick. This shape can be degenerated to a wedge, pyramid, or tetrahedron.
The number of real constants.
The number of saved variables.
The number of variables saved in results files.
Key for element formulation control:
- 0 - Create your own material codes within the element formulation. In this case,
the real constants are available to input material properties. You can also input linear material properties via MP and MPDATA commands .
- 1 - Use ANSYS standard material routines or the USERMAT subroutine to form
structural material data. ANSYS material properties must be input in the standard way (as you would for non-user-defined elements). This value is invalid when KeyShape = ANYSHAPE.
The maximum number of integration points (used when KEYANSMAT = 1).
Key for the element stress state (used when KEYANSMAT = 1):
0 - Plane stress elements.
1 - Axisymmetric elements.
2 - Plane strain elements.
3 - 3-D solid elements.
4 - 3-D solid-shell elements.
5 - Generalized plane strain elements.
6 - Beam elements.
7 - Link/truss elements.
8 - 3-D shell elements.
9 - Axisymmetric shell elements.
Key for specifying whether element stiffness matrices are symmetric or unsymmetric:
0 - Symmetric.
1 - Unsymmetric.
The USRELEM command specifies the characteristics of the user-defined element USER300.
Although you can intersperse other commands as necessary for your analysis, issue the USRELEM command as part of the following general sequence of commands:
Issue the ET command for element USER300, followed by the related TYPE command.
Issue both the USRELEM and USRDOF commands (in either order).
Define your element using USER300.
The number of real constants (NREAL) can refer to geometry quantities, material quantities, or any parameters for element formulation.
ANSYS saves variables in the .esav file to preserve element data when you specify a positive NSAVEVARS value. When KEYANSMAT = 0, all variables of both material and kinematic formulation are saved. When KEYANSMAT = 1, only the variables for kinematic formulation (such as deformation gradient tensor) are saved; in this case, the material routine saves all necessary material data automatically.
Element data saved in results files (NRSLTVAR) are accessible only as nonsummable miscellaneous data. ANSYS saves stress and total strain data for structural elements in the .rst file automatically (as it does for equivalent variables such as thermal gradient and thermal flux in thermal elements); therefore, NRSLTVAR does not need to include stress and total strain data.
To learn more about creating user-defined elements, see Creating a New Element in the Programmer’s Reference.