ABAQUS Volume II: I–Z - Manual (Page 479)

*STEP
NAME
Set this parameter equal to a label that will be used to refer to the step on the output database. Step
names in the same input file must be unique. Step names from the original input file can be reused
in a restart input file.
NLGEOM
Omit this parameter or set NLGEOM=NO to perform a geometrically linear analysis during the
current step. Include this parameter or set NLGEOM=YES to indicate that geometric nonlinearity
should be accounted for during the step (stress analysis and fully coupled thermal-stress analysis
only). Once the NLGEOM option has been switched on, it will be active during all subsequent steps
in the analysis.
PERTURBATION
Include this parameter to indicate that this is a linear perturbation step. For this type of analysis
ABAQUS/Standard expects that load, boundary, and temperature changes should be given and that
the results will be changes relative to the previous step. Please read the discussions in “General and
linear perturbation procedures,” Section 6.1.2 of the ABAQUS Analysis User’s Manual, “Mesh-to-
mesh solution mapping,” Section 12.4.1 of the ABAQUS Analysis User’s Manual, and “Applying
loads: overview,” Section 27.4.1 of the ABAQUS Analysis User’s Manual, before using this option.
SOLVER
Set SOLVER=DDM to use the domain decomposition iterative linear equation solver. Please read
the discussion in “Iterative linear equation solver,” Section 6.1.5 of the ABAQUS Analysis User’s
Manual, before using this option.
If this parameter is omitted, the default direct sparse solver is used.
This parameter cannot be used in conjunction with the UNSYMM parameter or the DSA
parameter.
UNSYMM
Set UNSYMM=YES to indicate that unsymmetric matrix storage and solution should be used.
Set UNSYMM=NO to indicate that symmetric storage and solution should be used.
The default value for this parameter depends on the model and procedure options used. The
user is allowed to change the default value only in certain cases. If the UNSYMM parameter is not
used in such cases, ABAQUS/Standard will use the value specified in the previous general analysis
step. See “Procedures: overview,” Section 6.1.1 of the ABAQUS Analysis User’s Manual, for a
more detailed discussion of the use of this parameter.
Optional data lines:
First line:
1. Subheading for this step.
The subheading can be several lines long, but only the first 80 characters of the first line will be saved
and printed as a subheading.
18.36–3
ABAQUS Version 6.1 Module: ID:
Printed on: