Create or edit a fully coupled thermal-electrochemical structural procedure
-
Display the Edit Step dialog box following the
procedure outlined in Creating a step
(Procedure type:
General; Coupled
thermal-electrochemical-structural), 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.
- Optional:
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.
-
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.
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 might 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.
|