Configuring a dynamic, explicit procedure

1. Display the Edit Step dialog box following the procedure outlined in Creating a step (Procedure type: General; Dynamic, Explicit), or Editing a step.

2. On the Basic, Incrementation, Mass scaling, and Other tabbed pages, configure settings such as the time period for the step, the maximum time increment, the increment size, mass scaling definitions, and bulk viscosity parameters as described in the following procedures.

1. In the Edit Step dialog box, display the Basic tabbed page.

2. 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.

3. In the Time period field, enter the time period of the step.

4. 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.

5. Toggle on Include adiabatic heating effects if you are performing an adiabatic stress analysis. This option is relevant only for metal plasticity. For more information, see Adiabatic analysis.

1. 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.)

2. 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.

3. If you selected Automatic time incrementation, perform the following steps:

   1. 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.

   2. Choose a Max. time increment option:

      • Choose Unlimited if you do not want to impose an upper limit to time incrementation.

      • Choose Value to enter a value for the maximum time increment allowed. Enter the value in the field provided.

   For more information, see Automatic time incrementation.

4. 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.

5. 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.

1. 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.)

2. 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.

3. At the bottom of the Data table, click Create.

   An Edit mass scaling dialog box appears.

4. 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.

5. 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. Enter the set name in the field provided.

6. 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.

7. 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.

8. 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.

9. 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.

10. 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.

11. If desired, repeat Steps 3 to 10 to create additional mass scaling definitions.

12. 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.

1. 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.)

2. Enter a value for the Linear bulk viscosity parameter. Linear bulk viscosity is included by default in Abaqus/Explicit.

3. 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 dynamic, explicit step, click OK to close the Edit Step dialog box.