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 17.14.)

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 17.14.)

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

5. If you selected Shape metrics, do the following:

   1. Select the element shape to verify.

   2. Choose one of the following selection criteria and enter a value:

      • Shape factor

      • Smaller face corner angle

      • Larger face corner angle

      • Aspect ratio

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

   3. Click Highlight.

      Abaqus/CAE highlights the elements that fail the element checks. 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.

6. If you selected Size metrics, do the following:

   1. Choose one of the following selection criteria and enter a value:

      • Geometric deviation factor

      • Shortest edge

      • Longest edge

      • Stable time increment

      • Maximum allowable frequency for acoustic elements

      Stable time increment is unavailable if the selected element types are not in the Abaqus/Explicit element library. Maximum allowable frequency for acoustic elements is unavailable if the selected element types are not acoustic elements in the Abaqus/Standard element library.

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

   2. Click Highlight.

      Abaqus/CAE highlights the elements that fail the element checks. 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.

7. If you selected Analysis checks, click Highlight to verify the mesh using the checks found in the input file processor in Abaqus/Standard and Abaqus/Explicit.

   Abaqus/CAE highlights any elements that generated error or warning messages during the mesh quality tests. Abaqus/CAE also displays in the message area the number of elements tested along with 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 neccessary, 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.

8. 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.