2. Tetra

2.1. How do I create a tetra mesh?

• Closed geometry in the form of a tetin file. This does not mean that the geometry can not have small gaps, but it must be basically closed. See "How do I ensure a closed volume for Tetra?"
• Mesh sizes should be defined appropriately. See "How do I define mesh sizes for tetra?"
• Material point(s) must be defined. See "What is a Material point?"
• Appropriate curves and points need to be defined. See "Why do I need curves/points for tetra meshing?"

2.2. I run tetra and I do not see any mesh on all/some surfaces?

• After your Tetra run, you may not have loaded your domain file
• Scroll up in the messages window to see if Mesh Editor has loaded the domain file. If you do not see this message, simply load the domain file (File > Open > Domain (mesh) File), and you should see your mesh. Turn on Tri_3 in the Display Menu to see the surface mesh.
• You may have leakage, and a valid domain file was never created
• While you are running Tetra if there is a leakage in your geometry, then it pops-up a window that "you have a leakage, do you want to repair it now?". At that time you might have pressed NO. If you press NO, then it loads the uncut domain of the tetra mesh into Mesh editor. Since there is a leak it could not find a closed volume around the material point, and thus could not create surface mesh at some places. There are several ways to close holes:
  • The best way is to close the holes in the geometry, and re-run tetra. If it is difficult to find the holes in the model, the user can run tetra interactive to see where the holes are located, or run geometry repair on the model which also may indicate a hole, please see "How do I ensure a closed volume for Tetra"
  • If there are holes a window pops up asking the user whether he wants to close holes during Tetra run. See I run tetra-interactive, and I have leakage (a squiggly line appears on the screen).
• You may have defined material points in the same family on both sides of a surface, thus the mesh disappears on that surface
• Either define different material points across the surface or define the surface family as an internal/thin wall. Click to see How do I define an internal/thin wall?

2.3. I run Tetra - From CAD/Surface mesh and I have leakage.

• Select "Yes" indicating you want to repair the hole and then Surface repair options window will pop-up. Keep the defaults and press "Accept" in that window.
• Select single (yellow) edges that form a closed loop and hit the middle mouse button (complete function). Repeat procedure for any other closed loops.
• "Flood Fill" will start automatically. If successful you should be able to see your entire surface boundary mesh. If not successful try to close holes again, and re-run Flood Fill. If the hole is much larger than the element size (greater than 3 to 4 times the edge length of neighboring elements) it is most likely due to a gap in the geometry in which case you should re-check the geometry for missing surfaces and repair any gaps or holes.
• Save mesh by selecting "File > Save > Domain (mesh) file"

If you are unable to close the holes, please see I run Tetra-From CAD/Surface mesh, have leakage, but cannot close holes.

[ top ]

2.4. I run tetra, but my volume assignment seems wrong.

2.5. I run tetra, but my mesh looks too coarse/fine.

• Decrease/increase the Reference Size under Geometry > Mesh Parameters > Model. All surface parameters are multiplied by the Reference size to obtain the surface parameter used during the Tetra process. Reducing/Increasing the Reference size will result in a finer/coarser mesh on all surfaces in the model.
• Decrease/increase the surface parameters on certain surfaces or families of surfaces in the model. This will create a finer/coarser mesh on these surfaces only and the remaining surfaces will not be affected.

2.6. I run tetra, but I get Orientation Errors.

2.7. I run Tetra-From CAD/Surface Mesh and I have leakage, but cannot close the holes.

• The best option is to close the geometry holes in either ICEM CFD's Mesh Editor or in the Native CAD Package. After fixing the CAD data, Tetra needs to be re-run.
• If the surface data is of reasonable quality but Tetra is still indicating leakage, try increasing the Edge Criterion from the default value of 0.2 to 0.3 and re-run Tetra. The Edge Criterion value is set under Geometry > Mesh Parameters > Model.

2.8. Why do I need curves/points for tetra meshing?

Example 1 illustrates two flat surfaces, with a fillet surface going between the two. In Example 2, the two flat surfaces meet.

In Example 1 the tetra mesh will round along the filleted region. The mesh does not have to conform to the edges ofthe surfaces. In fact if the mesh did have to conform to the edges of the surface, the mesh could be over-constrained, since if the mesh size is large, the mesh could jump from one edge to the other edge, and neglect to model the fillet region. Thus, the curves at the top and bottom of the filleted surface shouldn't be included in the model.

In Example 2 the mesh will round the corner unless there is a curve where the vertical and horizontal surface meet. This said, it is important to include the curve in example 2, since it will force ICEM CFD Tetra to line nodes along this corner.

The illustrations above say the same for points in the corners of curves, if two curves come together at a sharp angle, and the user wants to capture this feature, they need a point in this corner.

Let's see another example. For the geometry on left picture, you _DO_ need curves and points at the kink areas as defined there. If you don't give them, you might end up with a mesh like the one on right top instead of the one on right bottom:

Without Curves/points With Curves/points

[ top ]

2.9. Why does my mesh jump from one surface to another?

If you cannot ensure that then it is recommended that the user define a thin cut on these two surfaces. To define a thin cut, the two surfaces have to be in different families, and if converging, the curve at the intersection of the surfaces has to be in a third family.

If the mesh size is larger or approximately the same size as the gap, the surface mesh could have a tendency to jump the gap creating non-manifold vertices. This occurs in the Tetra process, because Tetra will automatically try to close holes in a model.

[ top ]

2.10. How do I define periodicity?

2.11. How do I create squeezed/stretched tetras to resolve my boundary layer?

Create your tetra mesh, create prisms on the boundary and convert all elements to tetras including pyramids if any. However, you need to put special attention towards following:

• How much is the stretch ratio that your solver can handle? Some solvers can take even 1:200 ratio of height/base of a tetra while some can even blow up with just 1:20. Theoretically, it should not matter much as towards the boudary, there are not big cross flow gradients
• Ideally there should not be any big cell jump between the last prism height and the immediate tetra. See "How do I ensure that there is a smooth volume transition from prism to tetras?" to follow this.
• Try to see if you can avoid pyramids coming in your prism mesh. Pyramids could sometimes be of extra-ordinary height as compared to their adjacent prisms.

Having a squeezed/stretched triangular surface mesh and then running "Tetra from surface mesh" is not a solution to this as it does not put any restriction towards the tetra height. Further, "Tetra from surface mesh" is pretty sensitive towards base triangle quality as well as adjacent cell size ratio. Thus, it may never create the tetra mesh for you.

If you are at the solution stage, then probably you can use OptiMesh to get the squeezed tetras at the steep solution gradients. However, OptiMesh is limited to a few solvers at this stage.

[ top ]

2.12. How do I run tetra from command-line?

SurfaceFile	"project/tetinfile"
DomainOutputFile	"project/tetra_mesh.uns"
CacheIntersections	0

On command-line you should run:

$ICEM_ACN/icemcfd/tetra tetra_params

Please be aware that the paths for the tetin and domain (mesh) files in the "tetra_params" file are relative to the current location..

If you want to run parallel version of tetra (ICEMCFD version 4.2 onwards), you can run the command

$ICEM_ACN/icemcfd/tetra tetra_params -nproc {number of processors}

to tell how many processors you want to use. If you do not specify "nproc" then it will use all the processors.

[ top ]

2.13. Why does my tetra crashes with "suspect value in AddVertexToSet" message?

• You did not define the global max size in the model
• There are no surfaces in the model

2.14. How do I ensure a closed volume for Tetra?

Typically, the procedure for geometry repair is as follows:

• Set a tolerance
• Create topology (build curves and points) - the curves will automatically take on the color of their association to adjacent surfaces.
• Select repair method.
• Either save the change, don't save or retry with a different repair method.
• Continue to next problem if same repair method is desired, simply select a new set of curves. If a different repair method is desired, go back to 3).

2.15. How do I define mesh sizes for tetra?

• Select Geometry > Mesh Params > Model apply the meshing parameters that are applicable to the entire model. Here the user has to define the following parameters depending on the mesh constraints:
  • Reference Size: A parameter that is referred to by other mesh parameters. This value will be multiplied by other parameters to give the actual value. For example, if the "Maximum size" of a given entity is 4, and the reference size is 3.5, the actual maximum size value to be meshed on that entity will be 4 x 3.5 = 14.0. The reference size allows the user to globally control the mesh size instead of changing the mesh size on each and every entity. User inputs any positive real number.
  • Maximum size:A factor that is multiplied by the "Reference size" which value will be the largest possible element size in the model. User inputs a power of two.
  • Natural size:When turned on, natural size will automatically subdivide to create elements that are smaller than the prescribed entity "Maximum size" in order to capture finer features of the geometry. The value entered is a factor multiplied by the "Reference size" and is a lower limit for the automatic subdivision. Natural size is used primarily to avoid setting up meshing parameters specifically for individual entities and allowing the geometry to determine the mesh size. In general, you would have larger elements on flat, planar surfaces and linear curves, and smaller elements on entities with a high degree of curvature and within small gaps. User inputs a power of two.
  • Refinement: A parameter that works along with "Natural size". This option is only accessible when "Natural size" is toggled on. It defines the number of edges along a radius of curvature if that radius were extended out to 360 degrees. This is generally used to avoid having too many elements along a given curve, if the natural size is too small for that particular curve. User inputs any positive integer value.
  • Define thin cuts as applicable.
  • Finally press Accept.
• The user can also define mesh parameters locally on the families. To do this, select Geometry > Mesh params > Selected Families and can enter the values like size, Minimum size and maximum deviation etc,.
• The user can also define different sizes on different surfaces of the same family using Geometry > Surface > Entity params and select the appropriate surface and can give the size on that surface different from that of the family to which it belongs.
• After this the user can save the geometry file and can proceed for Tetra run, ofcourse it is assumed that user has already defined the material point.

2.16. What is a Material point?

2.17. How many licenses tetra would consume on a multi-processor machine?

2.18. Why do I get error message "could not find opposite point in triangulate" while generating tetra mesh?

2.19. Why do I get the error "possible error in trim curve for surface" while tetra mesh generation?

2.20. What is edge-criterion , how does it effect the tetra mesh?

Significance of Edge-criterion:

• Consider two surfaces close to each other with the ends of the surface at a distance of 0.05.
• If the specified size on these surfaces is 1, the gap between the two surfaces cannot be resolved by tetra of size 1.
• To resolve this gap, set the edge-criterion to 0.05.
• This would split the tetra of size 1 to capture the gap of 0.05 as shown in the picture.
• Because of lower value of edge criterion, stretched tetras of bad quality are created ,which cannot be improved by smoothing.
• The general rule is:

Tetra stretched to capture the gap of 0.05

Mesh with edge criterion set lower than 0.2

Mesh with edge criterion set to 0.2

2.21. How do I insert a closed surface mesh into an existing volume mesh and get rid of trapped tetras?

1. Save the two tetin files separately.
2. Merge both tetin files and define ORFN point inside the tetin file for which we want only surface mesh. Save this tetin file.
3. Merge the existing volume mesh and the new surface mesh
4. Load new tetin file & domain file
5. Run Make_consistent.
6. Now run Edit Mesh -> Utilities -> Flood fill. This basically finds out the material points and separates out the volume families. If it finds ORFN volume, it deletes that too.
7. If you again do Make_consistent, that also runs this flood fill as a part of make_consistent. Sometimes it may happen that after loading a tetin file, if a geometric entity is created it will be not used for mesh editing. This could be the source of problem. So, it is advisable to load the merged tetin file & domain file and run flood fill (or make_consistent)

2.22. My tetra run reports for the leakage, I do see the line but there is no single/multiple edges! What is happening?

If you have all red curves and you still see this problem when you don't have any single/multiple edges, it's highly probable that your material point location is wrong. It is possibly lying on a surface itself.

[ top ]

2.23. How is the expansion ratio for linear progression calculated? (given number of layers, total height and initial height)

2.24. What is "unhandled case in fix spike node...."?

2.25. What are stuck elements appearing in my subset?