What is Tetra Meshing?

What is Tetra Meshing?

Tetrahedral is a four- nodded solid element that can be generated through the tria element by creating a volume and also through the existing volume of the geometry. These elements are used where the geometry has high thickness and complexity. The image attached below is a representation of a Tetra element. The Tetra element will have 4 triangular faces with four nodes joining them together (refer to Fig 1).

Methods to Generate Tetra Meshing:

Below are the three methods to generate Tetra Meshing:

• Conversion of 2D tria to Tetrahedral Elements, by using Tetra Mesh panel.
• Using the Quick Tetra Mesh, from the Utility panel.
• Using the Volume Tetra Mesh panel.

As per the above classification, we are going to mesh a component and clear the Tet collapse value:

First Method: Conversion of 2D Tria Elements into Tetrahedral Elements, by using Tetra Mesh panel

Steps to be followed to generate Tetra Mesh:

• Import the Model into HyperMesh and clean the geometry.
• Delete the solid from the model, by selecting the Delete→ Solid→ Delete entity.
• Now perform the 2D meshing on the model, by selecting the Mesh type as “Trias”.
  

• After completing the 2D meshing, the model should be cleared with the Minimum and Maximum Elemental error (refer Fig 2)

• Now the model is ready to perform the Tetra Meshing. Select the 3D→ tetramesh option.
• In the tetra mesh panel, select the elements under the “Fixed trias/quads to tetra mesh” option
• After selecting the elements, click on the “Mesh” button (refer Fig 3).

• Once the Tetra Meshing was completed, mask a few elements to check the mesh generation.

("Pink color denotes Tetra Mesh”)

Second Method: Generating Tetra Mesh, by using “Quick Tetra Mesh, from the Utility panel”

Steps to be followed to generate Tetra Mesh:

• Import the Model into HyperMesh and clean the geometry.
• Delete the solid from the model, by selecting the Delete→ Solid→ Delete entity.
• Click on the View→ Browsers→ HyperMesh→ Utility, as shown below:
  

• Now select the Geom/Mesh from the “Utility Menu”, then click on the Quick TetraMesh (refer Fig 4).
  

• In the Quick Tetra tab, select the Components and Surface.

1. Specify the Mesh size (as per the Quality mentioned).
2. Then change the Mesh type to “Trias only”.
3. Click on the Mesh button to generate the Tetra Mesh (refer Fig 5).
   

• After completion of the Surface Mesh, a dialogue box will be popping up, as shown below:

• Click on the OK button to complete the Tetra Meshing Process. Meanwhile, a new component collector will be created in the Tab bar, which contains the tetrahedral elements (refer Fig 6).

• Completed image of tetra mesh, by using Quick tetra Mesh panel.

Third Method: Generating Tetra Mesh, by using the Volume Tetra Mesh Panel

Steps to be followed to generate Tetra Mesh:

• Import the Model into HyperMesh and clean the geometry.
• Keep the solid of the model, select 3D→ tetramesh.
• Click on the Volume tetra option, and select the solid of the model (refer Fig 7).

1. Tick the checkboxes of “Use curvature” and “Use proximity”
2. Specify the Minimum element size (as per the quality criteria).
3. Then tick the checkbox of “Cleanup elements”.
4. Click on the “Mesh” button to generate the Volume Tetra Mesh.
   

• Completed image of tetra mesh, by using the Volume Tetra Mesh Panel.
  

Note:

• Reason for ticking the Checkbox - “Use Proximity”
  

• Reason for ticking the Checkbox - “Use Curvature”
  

It allows more Trias/ Tetras elements to be generated along the curved surfaces based on user-specified settings.

• Reason for ticking the Checkbox - “Cleanup elements”
  
  

It will apply an extra stage of calculation to improve the overall mesh quality by removing some nodes and combining elements. Meshing will fail if the shell elements of solids are present and are conflicting with the selection, when this occurs, the elements are cleaned up accordingly.

Example:

Hint:

1. Though the selection in Volume tetra, shows all the solids for meshing are selected in the status bar, it won't perform the Tetra Mesh for all the selected solids, unless and until the checkbox for “Cleanup elements” is ticked.
2. Though the feature capturing is more in detail by ticking the checkbox of “Use Proximity” and “Use Curvature”, we will have more elements in the curvatures. Due to this, the element size will be smaller and they will be prone to tet collapse failure. So care has to be taken while using these two options.
   

What is Tet Collapse?

Tet collapse is one of the quality parameters, which will be checked while generating Tetrahedral elements. It can be calculated by measuring the distance of a node from the opposite face, and then each of the four values will be divided by the Square root of the opposite face’s area. The minimum of four resulting values is then normalized by dividing it by 1.24.

Generally, tet collapse can be calculated by the formula = Min of (h/√A) ÷ 1.24

In that formula,

“h” represents the Height, between the Node (N1) and the opposite face of the Triangle.

“A” represents the Area of the Opposite Face (area of the Triangle).

Methods to clear Tet collapse:

There are two methods to clear the Tet collapse as stated below:

1. Using the “translate” command, to increase the height.
2. Using the “Tetra remesh” panel, to remesh failed elements.

First Method: Use the “translate” command, to increase the height.

Steps to be followed to clear the tet collapse:

• After completing the Tetra Mesh, check for the failed element.
• Select Tools→ check elems→ 3D→ tet collapse.
• In the status bar, it will show how many failed elements are present in the model.

• Click on the “save failed” option to save the tet collapse failed elements (refer Fig 8).
  

• Isolate the failed elements, by clicking on “Mask” option
• Then right-click on “elements”, to select the “retrieve” option.
• This will automatically select the failed elements as your masking entities.
• Click on the “mask” to hide the failed elements, then select the “reverse” option to show only the failed elements in the HyperMesh GUI (refer Fig 9).
  

• Now to clear the Tet collapse, select the Tools→ translate command.
• Manually inspect the failed element and do the following procedure:

1. Pick a node in any one failed element, which has minimum height.
2. Select N1, N2, and N3 which represent the opposite plane of the prior selected node.
3. Choose the magnitude value approximately by trial and error method.
4. Click on the “translate” button to move the node (refer Fig 10).
   

• After correcting the failed element, parallelly check the Tet collapse value in the “check elems” option.

Second Method: Using the “Tetra remesh” panel, to remesh failed elements.

Steps to be followed to clear the tet collapse:

• After completing the Tetra Mesh, check for the failed element.
• Select Tools→ check elems→ 3D→ tet collapse.
• In the status bar, it will show how many failed elements are present in the model.
  

• Now go to the Tools→ tetramesh→ Tetramesh parameters, to specify the tet collapse value.
• Tick the checkbox of “Max tetra size” and “Min tetra size”, to specify the limit of the tetra mesh size.
• Under “Elem quality target”, enter the target tet collapse value and tick the checkbox of fill voids, fix midnodes, and smoothing (refer Fig 11).
  

• Once, after setting the “Tetramesh parameters”, select the “Tetra remesh” option.
• Select the “3D elements” and “2D baffle elems” for re-meshing the model.
• Click on the “remesh” button, to clear the failed elements (refer Fig 12).
  

• To ensure the Tet collapse quality, check the failed elements in the “check elems” option.
• In the status bar, now it will show the 0% failed elements as shown below:
  

Note:

• We can select the “3D elements” and “2D baffle elems” under Tetra remesh panel, only when we choose the “Conversion of 2D tria to Tetrahedral Elements, by using Tetra Mesh panel (First method)” and “Using the Quick Tetra Mesh, from the Utility panel (Second method)”.
• For “Using the Volume Tetra Mesh panel (Third method)”, we have to select only the “3D elements” under Tetra remesh panel, since we have the 3D mesh alone in the model.
  

Hint:

Before working on the Tetramesh panel, it is advisable to fix the “Tetramesh parameters”.