To verify selected elements:

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 17.13.)

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

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 minimum face corner angle.

The maximum face corner angle.

The aspect ratio.

The shortest edge.

Whether the element passes the checks found in the input file processor in ABAQUS/Standard and ABAQUS/Explicit.

Continue selecting elements, as desired. From the buttons along the bottom of the Verify Mesh dialog box, click Dismiss to close the dialog box.

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

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

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 17.13.)

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.

From the top of the Verify Mesh dialog box, select one of the following types of verification checks:

Statistical checks

Analysis checks

If you selected Statistical checks, do the following:

Select the element shape to verify.

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

Smaller face corner angle

Larger face corner angle

Aspect ratio

Shortest edge

Shape factor

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

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.

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.

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

Click Reselect to select a different part instance or region.

Click Defaults to restore the default element failure criteria.

Click Dismiss to close the Verify Mesh dialog box.