Verifying your mesh

Upon completion of a meshing operation, Abaqus/CAE highlights any bad elements in the mesh. Abaqus/CAE also provides a set of tools in the Mesh module that allow you to verify the quality of your mesh and to obtain information about the nodes and elements in the mesh. You can use these tools to isolate regions where the mesh quality is poor and to guide you if you need to refine your mesh. To verify the quality of the mesh, choose the Object from the context bar, and select MeshVerify from the main menu bar. You can then select the part, part instances, geometric regions, or element to verify. Abaqus/CAE allows you to choose between checking that your mesh will pass the quality tests in the analysis products and checking that your mesh passes individual quality checks, such as checking for elements with a large aspect ratio. Any elements that do not pass the specified criteria are highlighted in the viewport, and you can choose to create and save a set containing the highlighted elements or, if applicable, the cells, faces, or edges related to those elements. For detailed information on using the mesh verify tools, see Verifying element quality.

You can use the Analysis checks to verify that the elements in your mesh will pass the element quality checks that are included with the input file processor in Abaqus/Standard or Abaqus/Explicit. Abaqus/CAE highlights any elements that fail the mesh quality tests and displays the number of elements tested along with the number of errors and warnings in the message area. The mesh quality tests in the input file processor are extensive and specific to each element type. At a minimum, the mesh quality tests issue a warning for elements that seem inappropriately distorted, and the tests issue an error if the distortion is severe. Abaqus/CAE does not support analysis checks for beam, gasket, or cohesive elements.

You can use the Shape metrics to highlight elements of a selected shape that do not meet one of the following selection criteria:

Shape factor

Abaqus/CAE highlights elements with a normalized shape factor smaller than a specified value. The shape factor criterion is available only for triangular and tetrahedral elements. The shape factor ranges from 0 to 1, with 1 indicating the optimal element shape and 0 indicating a degenerate element.

  • For triangular elements the normalized shape factor is defined as

    s⁢h⁢a⁢p⁢e⁢f⁢a⁢c⁢t⁢o⁢r=e⁢l⁢e⁢m⁢e⁢n⁢t⁢a⁢r⁢e⁢ao⁢p⁢t⁢i⁢m⁢a⁢l⁢e⁢l⁢e⁢m⁢e⁢n⁢t⁢a⁢r⁢e⁢a.

    Optimal element area is the area of an equilateral triangle with the same circumradius as the element. (The circumradius is the radius of the circle passing through the three vertices of the triangle.)

  • For tetrahedral elements the normalized shape factor is defined as

    s⁢h⁢a⁢p⁢e⁢f⁢a⁢c⁢t⁢o⁢r=e⁢l⁢e⁢m⁢e⁢n⁢t⁢v⁢o⁢l⁢u⁢m⁢eo⁢p⁢t⁢i⁢m⁢a⁢l⁢e⁢l⁢e⁢m⁢e⁢n⁢t⁢v⁢o⁢l⁢u⁢m⁢e.

    Optimal element volume is the volume of an equilateral tetrahedron with the same circumradius as the element. (The circumradius is the radius of the sphere passing through the four vertices of the tetrahedron.)

Small face corner angle

Abaqus/CAE highlights elements containing faces where two edges meet at an angle smaller than a specified angle.

Large face corner angle

Abaqus/CAE highlights elements containing faces where two edges meet at an angle larger than a specified angle.

Aspect ratio

Abaqus/CAE highlights elements with an aspect ratio larger than a specified value. The aspect ratio is the ratio between the longest and shortest edge of an element.

Table 1 shows the default limits for the selection criteria based on the element shape.

Table 1. Element shape selection criteria limits.
Selection criterion Quadrilateral Triangle Hexahedra Tetrahedra Wedge
Shape factor N/A 0.01 N/A 0.0001 N/A
Smaller face corner angle 10 5 10 5 10
Larger face corner angle 160 170 160 170 160
Aspect ratio 10 10 10 10 10

You can use the Size metrics to highlight elements that do not meet one of the following selection criteria:

Geometric deviation factor

Abaqus/CAE highlights elements with an edge whose geometric deviation factor is greater than the specified value. The geometric deviation factor is a measure of how much an element edge deviates from the original geometry, and Abaqus/CAE calculates this value by dividing the maximum gap between an element edge and its parent geometric face or edge by the length of the element edge. By default, Abaqus/CAE highlights elements whose geometric deviation factor is greater than 0.2.

Abaqus/CAE calculates the geometric deviation factor only for elements in a native mesh. If you select a part that contains no geometry, Abaqus/CAE disables this option in the Verify Mesh dialog box. If your selection includes both native and orphan elements, Abaqus/CAE considers only the native elements for calculations of geometric deviation factor.

Short edge

Abaqus/CAE highlights elements with an edge shorter than a specified value.

Long edge

Abaqus/CAE highlights elements with an edge longer than a specified value.

Stable time increment

Abaqus/CAE highlights elements with a calculated stable time increment less than the specified value. The stable time increment calculation requires a suitable material definition and section assignment and is meaningful only for Abaqus/Explicit analyses.

The stable time increment calculation in Abaqus/CAE is an approximation of the initial stable time increment calculation made by Abaqus/Explicit for an element-by-element formulation. It does not account for any of the following conditions:

  • Mass scaling

  • Point mass

  • Rotary inertia

  • Nonstructural mass

  • Reinforcement (rebar)

Material behaviors supported for the stable time increment calculation in Abaqus/CAE include elastic, hyperelastic, hyperfoam (without user-defined test data), and acoustic medium. Composite sections with multiple materials are not supported. For more information, see Stability.

Maximum allowable frequency for acoustic elements

Abaqus/CAE highlights finite acoustic elements that may not be valid for modal or steady-state dynamic analyses in Abaqus/Standard above the specified frequency value. The maximum allowable frequency calculation requires a suitable material definition and section assignment. The calculation is a guideline based on approximately 10 elements per wavelength:

fm⁢a⁢x=P⁢Co10⁢h,

where P is the interpolation order (1 or 2), h is the size of the element bounding box, and Co is the speed of sound (b⁢u⁢l⁢k⁢m⁢o⁢d⁢u⁢l⁢u⁢sd⁢e⁢n⁢s⁢i⁢t⁢y).

In addition, for both shape and size metrics Abaqus/CAE displays the following information in the message area for each selected part, part instance, or region:

  • The name of the part or part instance.

  • The total number of elements of the selected shape in the part instance or in the selected regions.

  • The number of highlighted elements and the percentage of the elements being verified that these elements comprise.

  • The average value of the selection criterion. For the geometric deviation factor, Abaqus/CAE calculates the average value by considering only elements along a curve or face; solid elements in the center of a volume are excluded from this value.

  • The worst value of the selection criterion—the value closest to the criterion if it is not exceeded or the value farthest beyond the criterion if it is exceeded.