Create or edit a coupled temperature-displacement procedure using
explicit integration
-
Display the Edit Step dialog box following the
procedure outlined in
Creating a step
(Procedure type:
General; Dynamic,
Temp-disp, Explicit ), or
Editing a step.
-
On the Basic,
Incrementation, Mass scaling, and
Other tabbed pages, configure settings such as the time
period for the step, the increment size, mass scaling definitions, and bulk
viscosity parameters 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.
-
In the Time period field, enter the time period
of the step.
-
Select an Nlgeom option:
-
Toggle Nlgeom Off to
perform a geometrically linear analysis during the current step.
-
Toggle Nlgeom On to
indicate that
Abaqus/Explicit
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.
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 to allow
Abaqus/Explicit
to determine the time incrementation automatically. For more information, see
Automatic Time Incrementation.
-
Choose Fixed to use a fixed time
incrementation scheme. The fixed time increment size is determined either by
the initial element stability estimate for the step or by a user-specified time
increment. For more information, see
Fixed Time Incrementation.
-
If you selected Automatic time incrementation,
perform the following steps:
-
Choose a Stable increment estimator option:
-
Choose Global to allow the global
estimator to determine the stability limit as the step proceeds. The adaptive,
global estimation algorithm determines the maximum frequency of the entire
model using the current dilatational wave speed. This algorithm continuously
updates the estimate for the maximum frequency. The global estimator will
usually allow time increments that exceed the element-by-element values.
-
Choose Element-by-element to allow
Abaqus/Explicit
to determine an element-by-element estimate using the current dilatational wave
speed in each element.
The element-by-element estimate is conservative; it will give
a smaller stable time increment than the true stability limit that is based
upon the maximum frequency of the entire model. In general, constraints such as
boundary conditions and kinematic contact have the effect of compressing the
eigenvalue spectrum, and the element-by-element estimates do not take this into
account.
-
By default, the "improved" method to estimate the element stable
time increment for three-dimensional continuum elements and elements with plane
stress formulations is used. This method usually results in a larger element
stable time increment than a more traditional method. Toggle off
Improved Dt Method to deactivate the "improved" method.
-
Choose a Max. time increment option:
For more information, see
Automatic Time Incrementation.
-
If you selected Fixed time incrementation, choose
an option for determining increment size:
-
Choose User-defined time increment to specify
a time increment size directly. Enter that time increment size in the field
provided.
-
Choose Use element-by-element time increment
estimator to use time increments the size of the initial
element-by-element stability limit throughout the step. The dilatational wave
speed in each element at the beginning of the step is used to compute the fixed
time increment size.
For more information, see
Fixed Time Incrementation.
-
If desired, enter a Time scaling factor to adjust
the stable time increment computed by
Abaqus/Explicit.
(This option is unavailable if you have specified a User-defined time
increment for the Fixed time incrementation
scheme.) For more information, see
Scaling the Time Increment.
Configure settings on the Mass scaling tabbed
page
-
In the Edit Step dialog box, display the
Mass scaling tabbed page. For background information on
mass scaling, see
Mass Scaling.
(For information on displaying the Edit Step
dialog box, see
Creating a step,
or
Editing a step.)
-
Choose one of the following options for specifying mass scaling:
-
Choose Use scaled mass and “throughout step” definitions
from the previous step if you want mass scaling definitions from the
previous step to propagate through the current step. If you choose this option,
you can skip the remaining steps in this procedure.
-
Choose Use scaling definitions below to
create one or more new mass scaling definitions for this step. If you choose
this option, complete the remaining steps in this procedure.
-
At the bottom of the Data table, click
Create.
An Edit mass scaling dialog box appears.
-
Specify which type of mass scaling definition you want to create:
-
Choose Semi-automatic mass scaling to define
mass scaling for any type of analysis except bulk metal rolling.
-
Choose Automatic mass scaling to define mass
scaling for a bulk metal rolling analysis. For more information, see
Automatic Mass Scaling for Analysis of Bulk Metal Rolling.
-
Choose Reinitialize mass to reinitialize
masses of elements to their original values. This option allows you to prevent
the scaled mass from a previous step from being used in the current step. For
more information, see
Reverting the Mass Matrix to the Original State.
-
Choose Disable mass scaling thoughout step to
disable in this step all variable mass scaling definitions from previous steps.
For more information, see
Continuous Mass Matrix with No Further Scaling.
-
If you selected Semi-automatic mass scaling,
Automatic mass scaling, or Reinitialize
mass, indicate the region to which you want the mass scaling
definition applied:
-
Choose Whole model to apply the mass scaling
definition to all elements in the model.
-
Choose Set to apply the mass scaling
definition to a particular set of elements. Click the arrow to the right of the
Set field, and select the set name of interest.
-
If you selected Semi-automatic mass scaling,
indicate when, during the step, you want
Abaqus/Explicit
to scale the element masses:
-
Choose At beginning of step to perform fixed
mass scaling only at the beginning of the step. For more information, see
Fixed Mass Scaling.
-
Choose Throughout step to scale the mass of
elements periodically during the step. For more information, see
Variable Mass Scaling.
-
If you selected Semi-automatic mass scaling,
indicate how you want
Abaqus/Explicit
to scale the element masses:
-
Toggle on Scale by factor to scale the
elements once at the beginning of the step by the value you enter in the field
provided. For more information, see
Defining a Scale Factor Directly.
-
Toggle on Scale to target time increment of
n to enter a desired element stable time
increment in the field provided. Click the arrow to the right of the
Scale element mass field, and select how you want
Abaqus/Explicit
to apply that target time increment:
-
Select Uniformly to satisfy target to
scale the masses of the elements equally so that the smallest element stable
time increment of the scaled elements equals the target value.
-
Select If below minimum target to scale
the masses of only the elements whose element stable time increments are less
than the target value.
-
Select Nonuniformly to equal target to
scale the masses of all elements so that they all have the same element stable
time increment equal to the target value.
For more information, see
Defining a Desired Element-by-Element Stable Time Increment.
If you toggle on both Scale by factor and
Scale to target time increment,
Abaqus/Explicit
first scales the masses by the factor value that you enter and then possibly
scales them again, depending on the value you enter for target time increment
and the option you select for applying that target.
-
If you selected Automatic mass scaling, enter the
following values:
-
In the Feed rate field, enter the estimated
average velocity of the workpiece in the rolling direction at steady-state
conditions.
-
In the Extruded element length field, enter
the average element length in the rolling direction.
-
In the Nodes in cross-section field, enter
the number of nodes in the cross-section of the workpiece. Increasing this
value decreases the amount of mass scaling.
For more information, see
Automatic Mass Scaling for Analysis of Bulk Metal Rolling.
-
If you selected Semi-automatic mass scaling
throughout the step or Automatic mass scaling, specify
when, during the step, you want
Abaqus/Explicit
to perform mass scaling calculations:
-
Choose Every n
increments to specify the frequency, in increments, at which
Abaqus/Explicit
is to perform mass scaling calculations. Enter the desired frequency in the
field provided.
For example, if you enter a value of 5,
Abaqus/Explicit
scales the mass at the beginning of the step and at increments 5, 10, 15, etc.
-
Choose At n equal
intervals to specify the number of intervals during the step at
which
Abaqus/Explicit
is to perform mass scaling calculations. Enter the desired value in the field
provided.
For example, if you enter a value of 2,
Abaqus/Explicit
scales the mass at the beginning of the step, the increment immediately
following the half-way point in the step, and the final increment in the step.
-
Click OK to close the Edit mass
scaling dialog box and return to the Mass
scaling tabbed page of the Edit Step dialog
box.
The mass scaling definition that you have just created appears in the
Data table.
-
If desired, repeat Steps 3 to 10 to create additional mass scaling
definitions.
-
Once you have created one or more mass scaling definitions, you can
edit or delete them if desired. Select a particular mass scaling definition in
the Data table, and click Edit or
Delete at the bottom of the Data
table.
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.)
-
Enter a value for the Linear bulk viscosity
parameter. Linear bulk viscosity is included by default in
Abaqus/Explicit.
-
Enter a value for the Quadratic bulk viscosity
parameter. This form of bulk viscosity pressure is found only in
solid continuum element and is applied only if the volumetric strain rate is
compressive.
For more information, see
Bulk Viscosity.
When you have finished configuring settings for the step, click
OK to close the Edit Step dialog
box.
|