Restarting Abaqus analyses

You can restart Abaqus solutions. For example, you can solve a solution that uses saved data from a previous analysis of the same finite element model. For complex solutions that contain multiple steps, you want to run the analysis in stages rather than analyze all steps within a lengthy, single solve. Running an analysis in stages allows you to examine the results and confirm that the solution is proceeding as you expected before you continue with the next step.

Note:

When you restart a solution, you cannot change any of the basic model definition data associated with that solution, such as the mesh or the associated materials.

Required files for a restart

If you want to later restart an analysis, you must request that the files that Abaqus requires for a restart be written when you first solve a solution. These restart files allow you to complete an analysis to a certain point in the solve and then restart and continue the analysis in a subsequent solve. You can control the amount of data written to the restart files. You can change this amount from step to step if you include a Restart modeling object in each step.

Abaqus requires the following files for a restart:

• Restart file (.res)

• Analysis database (.mdl and .stt)

• Part (.prt)

• Output database (.odb)

• Linear dynamics and substructure database (.sim)

Writing out the necessary information to later perform a restart

Use the Restart Output Control options on the Output tab in the Solution Step dialog box to write out restart information for a given step. You can choose to do the following:

• Indicate that the restart output is the same as restart data requested in a previous step

• Discontinue writing restart data.

• Apply a specific Restart modeling object request to the step.

Use the Restart modeling object to define the options that control the restart of an analysis. These options include:

• The amount of data written to the restart files.Note: You can change this amount from step to step if you include a Restart modeling object in each step.

• The frequency with which restart data is written.

You can write out restart information from Thermal analyses and the following types of Abaqus Structural steps:

• General

• Frequency Perturbation

• Visco

• Implicit Dynamics

• Direct Cyclic

• Explicit Dynamic

• Steady-State Coupled Thermal-Stress

• Transient Coupled Thermal-Stress

• Dynamic Coupled Thermal-Stress

The options in the Restart dialog box correspond to the options for the Abaqus *RESTART keyword.

Reading existing restart information into a solution

To restart analysis, you must read in the appropriate, existing restart information to your current solution. Use the options on the Restart tab the Solution dialog box to specify the restart information to read in. For example, you can do the following:

• Specify the name of the solution that you want to restart.

• Indicate whether you want to restart from the last available step or increment.

• Specify whether you want to resume the initial analysis or re-run the analysis from the beginning.

Example of restarting a solution

The following example shows how to restart and read in restart information to your current solution (Solution 1).

Three user-defined constraints are also defined for the simulation:

Solution 1 only uses two of the constraints.

To begin, you must clone the original solution to perform a restart-read analysis so the translator can process all the finite element data defined in the previous steps to export the new entities correctly and reformat and resolve label conflicts.

1. Clone Solution1:In the Simulation Navigator, right-click Solution1→Clone. A new solution called Copy of Solution1 appears in the Simulation Navigator.

2. Add a new step and the constraints to Copy of Solution1: Right-click Copy of Solution1→New Step. From the Solution Step dialog box, keep the default name and from the Step list, select General. Drag the Constraints folder to the new step, General 2.

3. Set the solution to restart from the second step: In the Simulation Navigator, right-click Copy of Solution 1→Edit. In the Restart tab of the Solution dialog box, select the Define Job Name Of the Run To Be Read check box. In the Job Name, type the name of the simulation file and Solution 1. In the Supply History Data from Solution Step Number box, type 2.

4. Restart the solution and read in existing information: In the Simulation Navigator, right-click Copy of Solution 1→Solve. The restart and read analysis runs without error.

Where do I find it?

Application	Pre/Post
Prerequisites	A Simulation file as the work part and displayed partAbaqus as the specified solverStructural or Thermal as the specified analysis type
Command Finder	Modeling Objects
Location in dialog box	Type→Restart

How do I

Create Abaqus conventional formulation shell elements

Learn more

Creating transition hybrid meshes

Controlling compaction of boundary conditions

Abaqus attributes for time-dependent fields

Control parameters for Abaqus analyses

Monitoring nodes to gauge the progress of a solution (Abaqus)

Customizing Abaqus input files with user-defined text

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Restarting Abaqus analyses, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });