Understanding 3D tetrahedral mesh quality evaluation

When you use the 3D Tetrahedral Mesh command to generate a solid mesh on your model, the software automatically evaluates the quality of the resulting elements.

These quality checks measure, for example:

• Different aspects of an element's deviation from an ideal size and shape, such as aspect ratio.

• The determinant of the Jacobian.

• Whether any tetrahedral elements have collapsed.

If the software detects any elements that fail the quality checks, it highlights their location in the graphics window.

Note:

For all quality checks other than the Jacobian check, the software uses corresponding quality threshold values specified in Threshold Values dialog box. For the Jacobian check, the Max Jacobian value you specify in the 3D Tetrahedral Mesh dialog box overrides the Jacobian values in the Threshold Values dialog box.

If you evaluate mesh quality at the time the mesh is generated, you can either automatically or manually correct quality issues before you try to solve the model.

Understanding how midnodes are adjusted for Jacobian failures

If the software detects that an element violates the specified Max Jacobian value specified in the 3D Mesh dialog box at the element’s integration points, the software iteratively moves the midnodes off the geometry to try to improve the Jacobian value. The software incrementally straightens the edge by moving the midnode along a line between the original location and a final straight location. The software first moves the node 25% of the distance along that line, then 50%, then 75%, then 100%. If the element passes the Jacobian criteria with the node at the 25, 50, or 75% location, then no further straightening occurs. As a result of this process, the nodes remain closer to the underlying geometry while still satisfying the quality criteria.

Note:

You can control the location at which the software calculates the Jacobian (at the element's Gauss points or vertices) in the Customer Defaults dialog box (Simulation→Pre/Post→Element Quality Check - Nastran, on the Jacobian Integration Points page).

See Midnode placement for parabolic elements for more information.

Automatically correcting quality issues with Auto Fix Failed elements

The Auto Fix Failed Elements option in the 3D Tetrahedral Mesh dialog box lets you control whether the software tries to automatically repair any detected element quality problems. Depending on the quality check that an element fails and its own topology, the software either removes the problematic element or remeshes the associated surfaces. See Understanding the Auto Fix Failed Elements process for more information.

Strategies for manually correcting quality issues

Depending upon your model and the number of quality issues with the mesh, it may be more efficient for you to manually address element quality failures. You should always evaluate the number of failing elements relative to the overall number of elements in the mesh. For example, if 10 elements in your model exceed the quality thresholds, it is probably more efficient for you to resolve those issues on a case by case basis than to have the software iteratively remesh the entire model.

Element quality issues often occur in regions where there are problems with the underlying geometry, such as surfaces that are very small relative to the specified element size. As a first step to resolving element quality options, you should always check the specified Small Feature Tolerance/Minimum Element Length value in the 3D Tetrahedral Mesh dialog box. Allowing the software to automatically clean up any features that are smaller than 10% of the target element size can often improve element quality.

You can also use the polygon geometry commands, such as Merge Face and Merge Edge, to repair issues with the underlying geometry that may cause poorly shaped elements. Additionally, you can also use the Mesh Control command to define edge or face densities in specific regions. This gives you better control over local element sizes in problem areas.

How do I

Create a 3D tetrahedral mesh

Learn more

3D tetrahedral meshing

Understanding the tetrahedral meshing process

Midnode placement for parabolic elements

Creating at least two elements through the thickness of tetrahedral meshes

Understanding the Auto Fix Failed Elements process

Controlling the size of interior elements in a 3D tetrahedral mesh

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Understanding 3D tetrahedral mesh quality evaluation, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });