Perform Analyses - Run Simulation

Check Model

Before performing an analysis, it is recommended that you perform a check on the model. This is done by clicking the Analysis Analysis Check Model command. The purpose of checking the model is so that the user can confirm that the FEA model is as intended. There are no holes, no missing boundary conditions, and so on. The checking is done in the Results environment.

Notes:

The date and time when the model was last Checked and last analyzed are stored. If a change is made to the model that would affect the results, such as changing the mesh, material properties, element definition, analysis parameters, loads, or constraints; then the Checked date is updated. When the Checked date is newer than the analyzed date, the following warning message is given whenever you try to display the model in the Results environment:
The results are out-of-date as the model has changed.

Do you wish to see the old results anyway?

If the model has truly changed, the old results should not be used.
If the model has been changed, or if a different version of the software is being used (which could result in different node or element numbering), it is possible that the existing results will not match the current FEA model. If you proceed to use the existing results, check the validity of the results carefully. Alternatively, re-analyze the model to be certain that the results are for the current model. Changes to the model include any geometry changes which can either be deliberate (for example, deleting lines and redrawing them) or transparent (for example, transferring to PV/Designer).
This message appears when doing a restart analysis for those analysis types that show the results while the analysis is running. This behavior is expected.

The geometry decoder checks that all the lines in the model are connected in such a way that valid elements can be formed out of those lines. If there are lines present in the model that cannot be used to form legitimate elements or other decoding problems, a warning dialog will appear. This dialog will allow the user to review the warnings in a text file.

Depending on the severity of the geometry warnings the program will proceed to the Results environment or not, according to the following list:

Clean Model: No warnings, and the model appears in the Results environment. After inspecting the model, go to back to the FEA Editor environment.
Minor Warnings: A warning file is produced, but the model appears in the Results environment. Use the warnings in the text file and Results environment to determine the cause of the problem. The sources of this kind of error are:
- Some of the lines in a part do not form elements as defined in that part. Consequently, nodes are generated, but they are not used to form elements. The warning indicates that nodes were dropped, and usually you will see holes or voids in the model.
Severe Warnings: A warning file is produced. No model is produced, so the Results environment does not appear. Use the text in the warning file to determine the problem, then return to the Interface to fix them. The sources of this kind of error are as follows:
- No combination of lines in a part can form elements. For example, when a part is defined to contain brick elements, but no brick elements can be formed out of the lines in that part, then the geometry translator reports an error.
- Improper material properties.

Run Simulations

Once the model is set up, you can perform the analysis using one of the following two methods:

Method 1: Click Analysis Analysis Run Simulation. This command runs the current design scenario only. Alternatively, right-click the appropriate Design Scenario heading in the browser and choose Run Simulation from the context menu. Initially, the solver used to run the simulation is dependent upon the Default Processor settings in the Processors tab of the application options. To override the default processor choice, expand the Run Simulation command (by clicking the bottom half of the ribbon button). Then, choose one of the following two sub-commands:
- Run with SimMech: Run the simulation using the native Simulation Mechanical solver.
- Run with Nastran: Run the simulation using the Autodesk Nastran solver.
These two commands are also available from the context menu that appears when you right-click a Design Scenario heading in the browser.

If you override the default processor, the Run Simulation command continues to call the most recently executed processor (when you re-analyze the same design scenario). It does not change the default processor for other design scenarios or future models. For example, assume that the default processor is SimMech but you choose to execute the Run with Nastran command. When you subsequently click the Run Simulation command to re-analyze this design scenario, the Nastran solver will be used again.

Note: Autodesk Nastran processors are available for solving particular analysis types only. The Run with Nastran command and the Default Processor option are available for the following linear, nonlinear, and thermal analysis types:
- Static Stress with Linear Material Models
- Natural Frequency (Modal)
- Natural Frequency (Modal) with Load Stiffening
- Critical Buckling Load
- Static Stress with Nonlinear Material Models
- Steady-State Heat Transfer
Method 2: Click Analysis Analysis Solver Manager. This command can be used to solve multiple design scenarios, schedule analyses, and to set up other analysis options. See the Solver Manager page for more information.

Regardless of which method you use to run the simulation, the Simulation Job Manager is used to manage and to monitor the solution tasks.

Regardless of whether you are using the SimMech or Nastran solvers, you can view the progress of the analysis by clicking the Details tab of the Output Bar at the bottom of the screen. You can view either the Solve Log file, the Summary file, or the Check Log file.

Note: The previous results are deleted when the analysis begins, except when doing a restart analysis. Some results that are common to all analysis types, such as Weight and Center of Gravity volume results and log files, may need to be recreated to see those results.

Real-Time Monitoring of Analysis Progress

Some analysis types display the model in the Results environment during the analysis (automatic monitoring). This capability exists regardless of which processor you choose (SimMech or Nastran). With automatic monitoring during the solution phase, you can verify that the model behavior is as expected. If not, the analysis can be canceled and the model setup adjusted accordingly. All of the normal features of the Results environment can be used while the analysis is continuing. The analysis types that provide automatic monitoring include:

Nonlinear Structural Analyses (Mechanical Event Simulation, Static Stress with Nonlinear Material Models, and MES Riks)
Thermal (Steady-State and Transient Heat Transfer)

Note: The time step displayed in the Results environment advances automatically as each step converges. If you change the displayed load case or time step in the Results environment while the analysis is ongoing, then the automatic time step advancement is disabled. To re-enable automatic time step advancement, click Results Contours Load Case Options Automatic Advance. This command functions as a feature toggle. When disabled, the display will remain at the currently displayed time step. When enabled, the time steps advance automatically.

Analysis types without real-time monitoring:

For other analysis type (linear, electrostatic, and natural frequency with nonlinear materials), the software remains in the FEA Editor while the solution is running. Once the analysis is complete, the model is displayed in the Results environment.