This option is used to introduce a linear or a general user-defined element. It must precede any reference to this user element on an *ELEMENT option.
Product: ABAQUS/Standard
Type: Model data
Level: Part Part Instance Model
Set this parameter equal to the name of the results file (with no extension) from which the data are to be read. See “Input syntax rules,” Section 1.2.1 of the ABAQUS Analysis User's Manual, for the syntax of such file names.
This parameter can be used only if the user-defined element type is linear and its stiffness and/or mass matrices are to be read from the ABAQUS/Standard results file of a previous analysis (in which they were written by using the *ELEMENT MATRIX OUTPUT or *SUBSTRUCTURE MATRIX OUTPUT options). When this parameter is used, all values are taken from the results file. For example, if the stiffness or mass being read from the results file is not symmetric, the UNSYMM parameter will be invoked automatically.
If this parameter is omitted, the data will be read from a standard input file.
Set this parameter equal to the element number that was assigned to the element whose matrices are being read. This parameter can also be set to a substructure identifier to read a substructure matrix from an ABAQUS/Standard results file.
Set this parameter equal to the step number in which the element matrix was written. This parameter is not required if using a substructure whose matrix was output during its generation.
Set this parameter equal to the increment number in which the element matrix was written. This parameter is not required if using a substructure whose matrix was output during its generation.
Include this parameter to indicate that the behavior of the element type is linear and is defined by a stiffness matrix and/or a mass matrix. The *MATRIX option is required to define the element's behavior.
Set this parameter equal to the number of nodes associated with an element of this type.
ABAQUS/Standard assigns space to store the coordinate values at each node in user subroutine UEL. The default number of coordinate values is equal to the largest active degree of freedom of the user element with a maximum of 3. Use the COORDINATES parameter to increase the number of coordinate values.
Include this parameter if the element matrices are not symmetric. This parameter will cause ABAQUS/Standard to use its unsymmetric equation solution capability.
The presence or absence of this parameter determines the form in which the matrices must be provided for reading.
First line:
Enter the list of active degrees of freedom at the first node of the element (as determined by the connectivity list). The rule in “Conventions,” Section 1.2.2 of the ABAQUS Analysis User's Manual, regarding which degrees of freedom can be used for displacement, rotation, temperature, etc. must be conformed to.
Second line if the active degrees of freedom are different at subsequent nodes:
Enter the position in the connectivity list (node position on the element) where the new list of active degrees of freedom first applies.
Enter the new list of active degrees of freedom.
Repeat the second data line as often as necessary.
Set this parameter equal to the number of nodes associated with an element of this type.
Set this parameter equal to the maximum number of coordinates needed in user subroutine UEL at any node point of the element. ABAQUS/Standard assigns space to store the coordinate values at all the nodes associated with elements of this type. The default is COORDINATES=1.
ABAQUS/Standard will change the value of COORDINATES to be the maximum of the user-specified value of the COORDINATES parameter or the value of the largest active degree of freedom of the user element that is less than or equal to 3. For example, if COORDINATES=1 and the active degrees of freedom of the user element are 2, 3, and 6, the value of COORDINATES will be changed to 3. If COORDINATES=2 and the active degrees of freedom of the user element are 11 and 12, the value of COORDINATES will remain as 2.
Set this parameter equal to the number of integer property values needed as data in user subroutine UEL to define such an element. The default is I PROPERTIES=0.
Set this parameter equal to the number of real (floating point) property values needed as data in user subroutine UEL to define such an element. The default is PROPERTIES=0.
Include this parameter if the element matrices are not symmetric. This parameter will cause ABAQUS/Standard to use its unsymmetric equation solution capability.
Set this parameter equal to the number of solution-dependent state variables that must be stored within the element. Its value must be greater than 0 and less than 1000. The default is VARIABLES=1.
First line:
Enter the list of active degrees of freedom at the first node of the element (as determined by the connectivity list). The rule in “Conventions,” Section 1.2.2 of the ABAQUS Analysis User's Manual, regarding which degrees of freedom can be used for displacement, rotation, temperature, etc. must be conformed to.
Second line if the active degrees of freedom are different at subsequent nodes:
Enter the position in the connectivity list (node position on the element) where the new list of active degrees of freedom first applies.
Enter the new list of active degrees of freedom.
Repeat the second data line as often as necessary.