- Field output
-
Abaqus
generates field output from data that are spatially distributed over the entire
model or over a portion of it. In most cases you use
the Visualization module
to view field output data using deformed shape, contour, or symbol plots. The
amount of field output generated by
Abaqus
during an analysis is often large. As a result, you typically request that
Abaqus
write field data to the output database at a low rate; for example, after every
step or at the end of the analysis.
When you create a field output request, you can specify the output frequency
in equally spaced time intervals or every time a particular length of time
elapses. For an
Abaqus/Standard
analysis procedure, you can alternatively specify the output frequency in
increments, request output after the last increment of each step, or request
output according to a set of time points. For an
Abaqus/Explicit
analysis procedure, you can alternatively request field output for every time
increment or according to a set of time points.
When you create a field output request,
Abaqus
writes every component of the selected variables to the output database. For
example, if you were using solid elements to model a cantilever beam with a
load at the tip, you could request the stress (all six components) and the
displacement (all six components) data from the entire model after the last
increment of the loading step. You could then use
the Visualization module
to view a contour plot of stresses and deflections in the final loaded state.
- History
output
-
Abaqus
generates history output from data at specific points in a model. In most cases
you use
the Visualization module
to display history output using X–Y plots. The rate
of output depends on how you want to use the data that are generated by the
analysis, and the rate can be very high. For example, data generated for
diagnostic purposes may be written to the output database after every
increment. You can also use history output for data that relate to the model or
a portion of the model as a whole; for example, whole model energies.
When you create a history output request, you can specify the output
frequency in equally spaced time intervals or every time a particular length of
time elapses. For an
Abaqus/Standard
analysis procedure, you can alternatively specify the output frequency in
increments, request output after the last increment of each step, or request
output according to a set of time points. For an
Abaqus/Explicit
analysis procedure, you can alternatively request history output in time
increments.
When you create a history output request, you can specify the individual
components of the variables that
Abaqus/CAE
will write to the output database. For example, if you model the response of a
cantilever beam with a load applied to the tip, you might request the following
output after each increment of the loading step:
You could then use
the Visualization module
to view an X–Y plot of stress at the root versus
displacement at the tip with increasing load.
|