| Abaqus Keywords Reference Guide |
|
| How to find keyword examples |
| Abaqus Keywords Reference Guide |
|
| How to find keyword examples |
This option is used to define an element directly by specifying its nodes.
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE
Type: Model data
Level: Part, Part instance, Assembly
Abaqus/CAE: Mesh module
Set this parameter equal to the element type, as defined in Part VI, “Elements,” of the Abaqus Analysis User's Guide.
For user elements specify the Un type identification (see “User-defined elements,” Section 32.17.1 of the Abaqus Analysis User's Guide). The *USER ELEMENT option must also appear in the same input file.
For substructures specify the Zn type identification (see “Using substructures,” Section 10.1.1 of the Abaqus Analysis User's Guide).
Set this parameter equal to the name of the element set to which these elements will be assigned.
This parameter applies only to Abaqus/Standard analyses.
This parameter is meaningful only for substructures. Set this parameter equal to the name (with no extension) of the substructure library on which the substructure resides. See “Input syntax rules,” Section 1.2.1 of the Abaqus Analysis User's Guide, for the syntax of such library names. If no name is specified, the default name is used (see “Using substructures,” Section 10.1.1 of the Abaqus Analysis User's Guide).
Set this parameter equal to the name of the alternate input file containing the data lines for this option. See “Input syntax rules,” Section 1.2.1 of the Abaqus Analysis User's Guide, for the syntax of such file names. If this parameter is omitted, it is assumed that the data follow the keyword line.
When the *ELEMENT option is used to define the connectivity of axisymmetric elements with asymmetric deformation in Abaqus/Standard, set this parameter equal to a positive offset number for use in specifying the additional nodes needed in the connectivity (see “Element definition,” Section 2.2.1 of the Abaqus Analysis User's Guide, for more information). The default is OFFSET=100000.
When the *ELEMENT option is used to define the connectivity of gasket elements in Abaqus/Standard or cohesive elements, set the OFFSET parameter equal to a positive offset number for use in defining the remaining nodes of the element when only part of the element nodes are defined explicitly. If this parameter is omitted, the connectivity of the entire gasket or cohesive element must be specified on the data lines (see “Defining the gasket element's initial geometry,” Section 32.6.4 of the Abaqus Analysis User's Guide, and “Defining the cohesive element's initial geometry,” Section 32.5.4 of the Abaqus Analysis User's Guide).
This parameter applies only to Abaqus/Standard analyses.
This parameter can be used only when the *ELEMENT option is used to define gasket elements. Use this parameter to specify the connectivity of gasket elements using the node ordering of an equivalent solid element. Set it equal to the face number of the equivalent solid element that corresponds to the first face (SNEG) of the gasket element. If no value is assigned to this parameter, it is assumed that the first face (S1) of the solid element corresponds to the first face of the gasket element.
First line:
Element number.
First node number forming the element.
Second node number forming the element.
Etc., up to 15 node numbers on this line.
The order of nodes for each element type (the element's connectivity) is given in Part VI, “Elements,” of the Abaqus Analysis User's Guide.
Continuation lines (only needed if the previous line ends with a comma):
Node numbers forming the element.
Repeat this set of data lines as often as necessary, with up to 16 integer values per line (maximum 80 characters).