Verify selected elements
To verify the quality of selected elements, select
from the main menu bar.
Abaqus/CAE displays prompts in the prompt area to guide you through the procedure.
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 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
Continue selecting elements, as desired.
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.
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
from the main menu bar.
Abaqus/CAE displays prompts in the prompt area to guide you through the procedure.
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, 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.
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.
If you want to specify verification checks on the Shape
metrics tabbed page, do the following:
-
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.
-
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.
-
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.
-
Specify a value for the Aspect ratio.
For a detailed description of the selection criteria, see
Verifying your mesh.
If you want to specify verification checks on the Size
metrics tabbed page, specify failure criteria for any of the
following:
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.
If you want to specify analysis checks, click the Analysis
checks tab, and toggle Errors and
Warnings to select which elements will be highlighted.
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.
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.
Your changes to the mesh verification criteria are saved for use in future
Abaqus/CAE
sessions.
|