You must configure a fully coupled temperature-displacement analysis when the stress analysis is dependent on the temperature distribution and the temperature distribution depends on the stress solution. For such cases the thermal and mechanical solutions must be obtained simultaneously rather than sequentially. In ABAQUS/Explicit a fully coupled thermal-stress analysis includes inertia effects and models transient thermal response. For more information, see “Fully coupled thermal-stress analysis in ABAQUS/Explicit” in “Fully coupled thermal-stress analysis,” Section 6.5.4 of the ABAQUS Analysis User's Manual.
When you configure a dynamic temperature-displacement procedure, the step editor displays the Basic, Incrementation, Mass scaling, and Other tabs. Settings you can configure with these tabbed pages include the time period for the step, the increment size, mass scaling definitions, and bulk viscosity parameters.
To configure settings on the Basic tabbed page:
In the Edit Step dialog box, display the Basic tabbed page.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
In the Description field, enter a short description of what occurs during this 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 a time scale for the analysis.
Select an Nlgeom option:
Turn Nlgeom Off to perform a geometrically linear analysis during the current step.
Turn Nlgeom On to indicate that ABAQUS/Explicit should account for geometric nonlinearity during the step. Once you have turned Nlgeom on, it will be active during all subsequent steps in the analysis.
To 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,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Select a Type option:
Select Automatic to allow ABAQUS/Explicit to determine the time incrementation automatically. For more information, see “Automatic time incrementation” in “Fully coupled thermal-stress analysis,” Section 6.5.4 of the ABAQUS Analysis User's Manual.
Select 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” in “Fully coupled thermal-stress analysis,” Section 6.5.4 of the ABAQUS Analysis User's Manual.
If you selected Automatic time incrementation, perform the following steps:
Select a Stable increment estimator option:
Select 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.
Select 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.
Select a Max. time increment option:
Select Unlimited if you do not want to impose an upper limit to time incrementation.
Select Value to enter a value for the maximum time increment allowed. Then enter the value in the field provided.
If you selected Fixed time incrementation, select an option for determining increment size:
Select User-defined time increment to specify a time increment size directly. Then enter that time increment size in the field provided.
Select 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.
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” in “Fully coupled thermal-stress analysis,” Section 6.5.4 of the ABAQUS Analysis User's Manual.
To 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,” Section 11.7.1 of the ABAQUS Analysis User's Manual.
(For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
Select one of the following options for specifying mass scaling:
Select 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 select this option, you can skip the remaining steps in this procedure.
Select Use scaling definitions below to create one or more new mass scaling definitions for this step. If you select 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:
Select Semi-automatic mass scaling to define mass scaling for any type of analysis except bulk metal rolling.
Select 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” in “Mass scaling,” Section 11.7.1 of the ABAQUS Analysis User's Manual.
Select 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 “Reinitializing the mass” in “Mass scaling,” Section 11.7.1 of the ABAQUS Analysis User's Manual.
Select Disable mass scaling thoughout step to disable in this step all variable mass scaling definitions from previous steps. For more information, see “Removing mass scaling definitions” in “Mass scaling,” Section 11.7.1 of the ABAQUS Analysis User's Manual.
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:
Select Whole model to apply the mass scaling definition to all elements in the model.
Select Set to apply the mass scaling definition to a particular set of elements. Then 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:
Select At beginning of step to perform fixed mass scaling only at the beginning of the step. For more information, see “Fixed mass scaling” in “Mass scaling,” Section 11.7.1 of the ABAQUS Analysis User's Manual.
Select Throughout step to scale the mass of elements periodically during the step. For more information, see “Variable mass scaling” in “Mass scaling,” Section 11.7.1 of the ABAQUS Analysis User's Manual.
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” in “Mass scaling,” Section 11.7.1 of the ABAQUS Analysis User's Manual.
Toggle on Scale to target time increment of n to enter a desired element stable time increment in the field provided. Then, 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.
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.
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:
Select Every n increments to specify the frequency, in increments, at which ABAQUS/Explicit is to perform mass scaling calculations. Then 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.
Select At n equal intervals to specify the number of intervals during the step at which ABAQUS/Explicit is to perform mass scaling calculations. Then 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 then click Edit or Delete at the bottom of the Data table.
To 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,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)
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” in “Explicit dynamic analysis,” Section 6.3.3 of the ABAQUS Analysis User's Manual.
Once you have finished configuring settings for the step, click OK to close the Edit Step dialog box.