To verify selected elements:

1. To verify the quality of selected elements, select MeshVerify from the main menu bar.

   Abaqus/CAE displays prompts in the prompt area to guide you through the procedure.

   Tip:  You can also verify selected elements using the tool, located in the Mesh module toolbox. (For more information, see “Using the Mesh module toolbox,” Section 17.15.)

2. From the Select the regions to verify by field in the prompt area, select Element.

3. Select the element that you want to verify. Abaqus/CAE displays the following in the message area:

   • The name of the part or part instance

   • The element index

   • The element shape

   • The shape factor for triangle and tetrahedra elements

   • The minimum and maximum face corner angles

   • The aspect ratio

   • The geometric deviation factor

   • The stable time increment

   • The maximum allowable frequency for acoustic elements

   • The shortest edge and longest edge

   • Whether the element passes the checks found in the input file processor in Abaqus/Standard and Abaqus/Explicit

4. Continue selecting elements, as desired.

5. When you have finished selecting elements, either

   • Click mouse button 2 in the viewport, or

   • Select any other tool from the toolbox, or

   • Click the cancel button in the prompt area, or

   • Click the verify mesh tool in the Mesh module toolbox.

To verify a part, a part instance, or a region:

1. From the Object field in the context bar, select a part or select the assembly.

2. From the main menu bar, select MeshVerify from the main menu bar.

   Abaqus/CAE displays prompts in the prompt area to guide you through the procedure.

   Tip:  You can also verify a mesh using the tool, located in the Mesh module toolbox. (For more information, see “Using the Mesh module toolbox,” Section 17.15.)

3. From the text field in the prompt area, select the type of region to verify:

   • Select Part or Part Instances and select the part or part instances whose mesh you want to verify, and press mouse button 2.

   • Geometric Regions. Select the cells, faces, or edges whose mesh you want to verify, and press mouse button 2.

   Abaqus/CAE displays the Verify Mesh dialog box.

4. From the top of the Verify Mesh dialog box, click the tab corresponding to the desired verification checks. The following verification types are available:

   • Shape metrics

   • Size metrics

   • Analysis checks

   You can specify verification checks on multiple tabbed pages. Abaqus/CAE refers to the verification checks specified on all three tabbed pages when you click Highlight.

5. To save a set containing results of the selected verification checks, toggle on Create set near the bottom of the Verify Mesh dialog and either accept the default set name or enter a new name for the set.

   If there are any results displayed, Abaqus/CAE creates the set when you click Highlight, as described in the following steps.

6. If you want to specify verification checks on the Shape metrics tabbed page, do the following:

   1. From the Shape factor options, specify the shape factor criterion for triangular elements and tetrahedral elements in your selection. If your selection includes both triangular elements and tetrahedral elements, the Shape factor options provide separate controls for each type; if your selection includes only triangular elements or only tetrahedral elements, a single control is provided.

   2. If your selection includes triangular elements, you can specify the small face corner angle and the large face corner angle for triangular elements from the Tri-Face Corner Angle options.

   3. If your selection includes tetrahedral elements, you can specify the small face corner angle and the large face corner angle for tetrahedral elements from the Quad-Face Corner Angle options.

   4. Specify a value for the Aspect ratio.

   For a detailed description of the selection criteria, see “Verifying your mesh,” Section 17.6.1.

7. If you want to specify verification checks on the Size metrics tabbed page, specify failure criteria for any of the following:

   • Geometric deviation factor

   • Shortest edge

   • Longest edge

   • Stable time increment

   • Maximum allowable frequency for acoustic elements

   Stable time increment is available only for elements in the Abaqus/Explicit element library. Maximum allowable frequency for acoustic elements is available only for acoustic elements in the Abaqus/Standard element library.

   For a detailed description of the selection criteria, see “Verifying your mesh,” Section 17.6.1.

8. If you want to specify analysis checks, click the Analysis checks tab, and toggle Errors and Warnings to select which elements will be highlighted.

9. Click Highlight.

   Abaqus/CAE highlights elements that fail the element checks specified in the Shape Metrics or Size Metrics tabbed pages as warnings. In addition, any elements that generated errors or warnings using the checks found in the input file processor in Abaqus/Standard and Abaqus/Explicit are highlighted in the appropriate colors. If you selected Create set in Step 5, Abaqus/CAE saves a set containing the highlighted results. In addition, Abaqus/CAE displays information in the message area, such as the name of the part instance, the total number of elements, the number of highlighted elements, and the average and worst value of the selection criterion.

   Regardless of your selection of Errors and Warnings in the Analysis checks tabbed page, Abaqus/CAE also displays in the message area the total number of elements tested and the number of errors and warnings. In most cases, it will be obvious from the element shape why the input file processor issued an error or a warning. If necessary, you can submit a datacheck analysis from the Job module and review the messages that Abaqus writes to the data file. Abaqus/CAE does not support analysis checks for beam, gasket, or cohesive elements.

10. From the buttons along the bottom of the Verify Mesh dialog box, do the following:

    • Click Reselect to select different part instances or regions.

    • Click Defaults to restore the default element failure criteria on all of the tabs.

    • Click Dismiss to close the Verify Mesh dialog box.