Generating a Mesh and Submitting an Analysis Job

The finite element mesh is the collection of nodes and elements used to represent the system and to transform the continuous mechanical problem into a discrete numerical problem. All user specifications on the system geometry are eventually translated by the program into mesh input data.

This task shows you how to specify mesh parameters such as size and sag, generate the mesh on your part, create an analysis job, and submit the job to the Abaqus solver.

  1. Expand the Nodes and Elements feature in the specification tree, and double-click the OCTREE Tetrahedron Mesh.1 feature to edit the global characteristics of the mesh.

    The OCTREE Tetrahedron Mesh dialog box appears.

    The important element characteristics are their order, their size, and their sag. The order is the degree of polynomial interpolation for the unknown field (the displacement field) inside the element. The size is the dimension of the element. The sag is a measure of how closely the element boundaries follow the geometry they are supposed to represent.

  2. In the OCTREE Tetrahedron Mesh dialog box, specify a global element Size of 0.025 m and a global element Absolute sag of 0.008 m. Accept the default choice of a linear element type, and click OK.

  3. Right-click on the Nodes and Elements object in the specification tree, and select Mesh Visualization from the menu that appears.

    A warning message dialog box appears, informing you that the mesh needs to be updated; click OK to close the dialog box and continue with the mesh generation. When the mesh generation is complete, the mesh is displayed on the part and a Mesh object appears under Nodes and Elements in the specification tree.

  4. Expand the Abaqus Jobs object set in the specification tree, and double-click the Job-1 feature to edit the analysis job.

    The Edit Job dialog box appears.

    Note:  To create a new Abaqus job for the current analysis case, click the Create Job icon .

  5. You can change the job identifier by editing the Name field. This name will be used in the specification tree and in the Job Manager.

  6. Enter a description for the job in the Description field.

  7. Accept the default values for the job data, and click OK.

  8. Save the .CATAnalysis file to a location where you have write permissions. Select File>Save from the menu bar, and select a directory in which you can save the file.

  9. Click the Job Manager icon .

    The Job Manager dialog box appears with a list of the Abaqus jobs that you have created. By default, jobs for all Abaqus Analysis Cases are shown.

  10. Select the job you edited from the list in the Job Manager, and click Submit.

    By default, consistency checks are run when a job is submitted. A Job Submission dialog box appears with the results of these consistency checks. In addition to the consistency check messages, messages from the input file writer are listed on the Write Input File Messages tabbed page. In this case the Consistency Check Messages page is empty, and the Write Input File Messages page indicates that the input file was generated successfully.

  11. Click Continue in the Job Submission dialog box.

    Abaqus for CATIA V5 submits the job for analysis using the job settings defined in the job editor. The information in the Status column of the Job Manager updates to indicate the job's status. The Status column for this tutorial shows one of the following:

    • Submitted while the analysis input file is being generated.

    • Running while Abaqus analyzes the model.

    • Completed when the analysis is complete, and the output has been written to the output database file.

    • Aborted if Abaqus finds a problem with the input file or the analysis and aborts the analysis.

  12. When the job completes successfully, you are ready to review the results of the analysis. From the buttons on the right edge of the Job Manager, click Attach Results.

    A link to the Abaqus output database file containing the results appears in the Links Manager, and a Static Step object appears in the specification tree under the Analysis Case Solution objects set for the current analysis case. In addition, the status of the Analysis Case Solution entry is updated to show that the solution is now available and is consistent with the model and history specification; in other words, the symbol no longer appears.

  13. Click Close in the Job Manager.

For information on related topics, click any of the following items: