| Abaqus Keywords Reference Guide |
|
| How to find keyword examples |
| Abaqus Keywords Reference Guide |
|
| How to find keyword examples |
This option is used to provide tabular printed output of element variables (stresses, strains, etc.).
Product: Abaqus/Standard
Type: History data
Level: Step
Set this parameter equal to the name of the element set for which this output request is being made. If this parameter is omitted, the output will be printed for all elements in the model.
Set this parameter equal to the output frequency, in increments. The output will always be printed at the last increment of each step unless FREQUENCY=0. The default is FREQUENCY=1. Set FREQUENCY=0 to suppress the output.
This parameter is useful only during eigenvalue extraction for natural frequencies (“Natural frequency extraction,” Section 6.3.5 of the Abaqus Analysis User's Guide), complex eigenvalue extraction (“Complex eigenvalue extraction,” Section 6.3.6 of the Abaqus Analysis User's Guide), and for eigenvalue buckling estimation (“Eigenvalue buckling prediction,” Section 6.2.3 of the Abaqus Analysis User's Guide). Set this parameter equal to the highest mode number for which output is required.
The default value is LAST MODE=N, where N is the number of modes extracted. If the MODE parameter is used, the default value is LAST MODE=M, where M is the value of the MODE parameter.
This parameter is useful only during natural frequency extraction, complex eigenvalue extraction, and eigenvalue buckling estimation. Set this parameter equal to the first mode number for which output is required. The default is MODE=1. When performing a SIM-based *FREQUENCY analysis (EIGENSOLVER=AMS, EIGENSOLVER=LANCZOS, SIM, or EIGENSOLVER=SUBSPACE, SIM) eigenvectors are always mass normalized. Otherwise, the normalization will follow the format set by the NORMALIZATION parameter, with DISPLACEMENT as the default.
Set POSITION=AVERAGED AT NODES if the values being printed are the averages of values extrapolated to the nodes of the elements in the set. Since variables may be discontinuous between elements with different properties, Abaqus/Standard breaks the output into separate tables for different element property definitions within the element set specified. Abaqus/Standard will also output elements of differing types separately. Thus, averaging will occur only over elements that contribute to a node that have the same type.
Set POSITION=CENTROIDAL if values are being printed at the centroid of the element (the centroid of the reference surface of a shell element, the midpoint between the end nodes of a beam element).
Set POSITION=INTEGRATION POINTS (default) if values are being printed at the integration points at which the variables are actually calculated.
Set POSITION=NODES if the values being written are extrapolated to the nodes of each element in the set but not averaged at the nodes.
This parameter can be used to obtain output only for the rebar in the element set specified; output for the matrix material will not be given. It can be used with or without a value. If it is used without a value, the output will be given for all rebar in the element set. Its value can be set to the name assigned to the rebar on the *REBAR option to specify output for that particular rebar in the element set.
If this parameter is omitted in a model that includes rebar, the output requests govern the output for the matrix material only (except for section forces, when the forces in the rebar are included in the force calculation).
Rebar output can be obtained only at the integration points in continuum and beam elements. In shell and membrane elements rebar output can be obtained at the integration points and at the centroid of the element.
Set SUMMARY=YES (default) to obtain a summary and the locations of the maximum and minimum values in each column of the table.
Set SUMMARY=NO to suppress this summary.
Set TOTALS=YES to print the total of each column in the table. This is useful, for example, to sum the energies of a set of elements. The default is TOTALS=NO.
First line (optional, and relevant only if integration point variables are being printed for shell, beam, or layered solid elements):
Give a list of the section points in the beam, shell, or layered solid at which variables should be printed. If this line is omitted, the variables are printed at the default output points defined in Part VI, “Elements,” of the Abaqus Analysis User's Guide. For section points on a meshed beam cross-section, specify a list of user-defined section point labels. If this data line is omitted, all available section points will be printed. A maximum number of 16 section points can be specified. Repeat the *EL PRINT option as often as needed if output at additional points is required.
Second line:
Give the identifying keys for the variables to be printed in a table for this element set. The keys are defined in “Abaqus/Standard output variable identifiers,” Section 4.2.1 of the Abaqus Analysis User's Guide. All of the variables in each table must be of the same type (integration point, section point, or whole element variables).
Repeat the second data line as often as necessary: each line defines a table. If this line is omitted, no element output will be printed to the data file.