Create or edit a coupled temperature-displacement procedure
-
Display the Edit Step dialog box following the
procedure outlined in
Creating a step
(Procedure type:
General; Coupled
temp-displacement ), or
Editing a step.
-
On the Basic,
Incrementation, and Other tabbed
pages, configure settings such as the time period for the step, increment size,
and solution technique preferences as described in the following procedures.
Configure settings on the Basic tabbed page
-
In the Edit Step dialog box, display the
Basic tabbed page.
-
In the Description field, enter a short
description of the analysis step.
Abaqus
stores the text that you enter in the output database, and the text is
displayed in the state block by the Visualization module.
-
Indicate whether you want Steady-state or
Transient response. See the following sections for more
information:
Note:
After you have selected a Response option, a
message appears informing you that
Abaqus/Standard
has selected the Default load variation with time option
(located on the Other tabbed page) that corresponds to
your Response selection. Click
Dismiss to close the message dialog box.
-
In the Time period field, enter the time period
of the step.
-
Choose an Nlgeom option:
-
Toggle Nlgeom Off to
perform a geometrically linear analysis during the current step.
-
Toggle Nlgeom On to
indicate that
Abaqus/Standard
should account for geometric nonlinearity during the step. Once you have
toggled Nlgeom on, it will be active during all subsequent
steps in the analysis.
For more information, see
Linear and nonlinear procedures.
-
Select an automatic stabilization method if you expect the problem to
have local instabilities such as surface wrinkling, material instability, or
local buckling.
Abaqus/Standard
can stabilize this class of problems by applying damping throughout the model.
For more information, see
Unstable Problems, and
Automatic Stabilization of Static Problems with a Constant Damping Factor.
Click the arrow to the right of Automatic
stabilization, and select a method for defining the damping factor:
-
Select Specify dissipated energy fraction to
allow
Abaqus/Standard
to calculate the damping factor from a dissipated energy fraction that you
provide. Enter a value for the dissipated energy fraction in the adjacent field
(the default is 2.0 × 10−4). For more information, see
Calculating the Damping Factor Based on the Dissipated Energy Fraction.
-
Select Specify damping factor to enter the
damping factor directly. Enter a value for the damping factor in the adjacent
field. For more information, see
Directly Specifying the Damping Factor.
-
Select Use damping factors from previous general
step to use the damping factors at the end of the previous step as
the initial factors in the current step's variable damping scheme. These
factors override any initial damping factors that are calculated or specified
directly in the current step. If there are no damping factors associated with
the previous general step (for example, if the previous step does not use any
stabilization or the current step is the first step of the analysis),
Abaqus
uses adaptive stabilization to determine the required damping factors.
-
When using automatic stabilization,
Abaqus
can use the same damping factor over the course of a step, or it can vary the
damping factor spatially and temporally during a step based on the convergence
history and the ratio of the energy dissipated by damping to the total strain
energy. For more information, see
Adaptive Automatic Stabilization Scheme.
If you selected Specify dissipated energy fraction,
adaptive stabilization is optional and turned on by default. If you selected
Specify damping factor, adaptive stabilization is optional
and turned off by default. If you selected Use damping factors from
previous general step, adaptive stabilization is required.
To use adaptive stabilization, toggle on Use adaptive
stabilization with max. ratio of stabilization to strain energy (if
necessary), and enter a value in the adjacent field for the allowable accuracy
tolerance for the ratio of energy dissipated by damping to total strain energy
in each increment. The default value of 0.05 should be suitable in most cases.
-
If desired, toggle on Include creep/swelling/viscoelastic
behavior. If you leave this option toggled off, you indicate that
there is no creep or viscoelastic response occurring during this step even if
creep or viscoelastic material properties have been defined.
Configure settings on the Incrementation tabbed
page
-
In the Edit Step dialog box, display the
Incrementation tabbed page.
(For information on displaying the Edit Step
dialog box, see
Creating a step,
or
Editing a step.)
-
Choose a Type option:
-
Choose Automatic if you want
Abaqus/Standard
to determine suitable time increment sizes.
-
Choose Fixed to specify direct user control
of the incrementation.
Abaqus/Standard
uses an increment size that you specify as the constant increment size
throughout the step.
-
In the Maximum number of increments field, enter
the upper limit to the number of increments in the step. The analysis stops if
this maximum is exceeded before
Abaqus/Standard
arrives at the complete solution for the step.
-
If you selected Automatic in Step 2, enter values
for Increment size:
-
In the Initial field, enter the initial time
increment.
Abaqus/Standard
modifies this value as required throughout the step.
-
In the Minimum field, enter the minimum time
increment allowed. If
Abaqus/Standard
needs a smaller time increment than this value, it terminates the analysis.
-
In the Maximum field, enter the maximum time
increment allowed.
-
If you selected Fixed in Step 2, enter a value
for the constant time increment in the Increment size
field.
-
If you selected Automatic in Step 2 and if you
selected Transient response on the
Basic tabbed page, do the following:
-
Enter a value for the Max. allowable temperature change
per increment.
Abaqus/Standard
restricts the time step to ensure that this value is not exceeded at any node
during any increment of the step.
-
If you toggled on Include creep/swelling/viscoelastic
behavior on the Basic tabbed page, toggle on
Creep/swelling/viscoelastic strain error tolerance to
enter the maximum difference in the creep strain increment calculated from the
creep strain rates at the beginning and at the end of the increment. This value
controls the accuracy of the creep integration. For more information, see
Automatic Incrementation Controlled by the Creep Response.
-
If you toggled on Include creep/swelling/viscoelastic
behavior on the Basic tabbed page, choose a
Creep/swelling/viscoelastic integration option:
-
Choose Explicit/Implicit if you want to allow
Abaqus/Standard
to invoke the implicit integration scheme. For most coupled thermal-stress
analyses, the unconditional stability of the backward difference operator
(implicit method) is desirable.
-
Choose Explicit if you want to restrict
Abaqus/Standard
to using explicit integration. Explicit integration can be less expensive
computationally and simplifies implementation of user-defined creep laws in
user subroutine
CREEP.
For more information, see
Automatic Incrementation Controlled by the Creep Response.
Configure settings on the Other tabbed page
-
In the Edit Step dialog box, display the
Other tabbed page.
(For information on displaying the Edit Step
dialog box, see
Creating a step,
or
Editing a step.)
-
Choose a Matrix storage option:
-
Choose Use solver default to allow
Abaqus/Standard
to decide whether a symmetric or unsymmetric matrix storage and solution scheme
is needed.
-
Choose Unsymmetric to restrict
Abaqus/Standard
to the unsymmetric storage and solution scheme. (This is the only matrix
storage option available if you choose the Full Newton
solution technique.)
-
Choose Symmetric to restrict
Abaqus/Standard
to the symmetric storage and solution scheme.
For more information on matrix storage, see
Matrix Storage and Solution Scheme in Abaqus/Standard.
-
Choose a Solution technique:
-
Choose Full Newton to use Newton's method as
a numerical technique for solving nonlinear equilibrium equations. For more
information, see
Nonlinear solution methods in Abaqus/Standard.
-
Choose Separated to specify that linearized
equations for the individual fields in the fully coupled procedure are to be
decoupled and solved separately for each field. This option provides a less
costly solution for an analysis that is fully coupled in the sense that the
mechanical and thermal solutions evolve simultaneously, but with a weak
coupling between the two solutions. For more information, see
Approximate Implementation.
-
Click the arrow to the right of the Convert severe
discontinuity iterations field, and select an option for dealing
with severe discontinuities during nonlinear analysis:
-
Select Off to force a new iteration if severe
discontinuities occur during an iteration, regardless of the magnitude of the
penetration and force errors. This option also changes some time incrementation
parameters and uses different criteria to determine whether to do another
iteration or to make a new attempt with a smaller increment size.
-
Select On to use local convergence criteria
to determine whether a new iteration is needed.
Abaqus/Standard
will determine the maximum penetration and estimated force errors associated
with severe discontinuities and check whether these errors are within the
tolerances. Hence, a solution may converge if the severe discontinuities are
small.
-
Select Propagate from previous step to use
the value specified in the previous general analysis step. This value appears
in parentheses to the right of the field.
For more information on severe discontinuities, see
Severe Discontinuities in Abaqus/Standard.
-
Abaqus/Standard
automatically selects the Default load variation with time
option that corresponds to your Response selection on the
Basic tabbed page. It is recommended that you leave the
Default load variation with time selection unchanged.
-
Click the arrow to the right of the Extrapolation of
previous state at start of each increment field, and select a method
for determining the first guess to the incremental solution:
-
Select Linear to indicate that the process is
essentially monotonic and
Abaqus/Standard
should use a 100% linear extrapolation, in time, of the previous incremental
solution to begin the nonlinear equation solution for the current increment.
-
Select Parabolic to indicate that the process
should use a quadratic extrapolation, in time, of the previous two incremental
solutions to begin the nonlinear equation solution for the current increment.
-
Select None to suppress any extrapolation.
For more information, see
Extrapolation of the Solution.
When you have finished configuring settings for the step, click
OK to close the Edit Step dialog
box.
|