[gi12]

Hi all

A quick question. Is it possible to specify the number of nodes for tetra meshing?, and if yes how can you do that

Many thanks
GI12

[PSYMN]

You specify the size of the mesh in the volume and/or on entities... Then the mesher fills the volume with elements of the specified sizes. The number of elements in the volume or the number of nodes in the mesh are the result of that filling process and will vary with a number of parameters including the type of mesh, growth rate, etc...

For unstructured mesh in simple situations, it may be possible to predict roughly, but the more complicated the geometry or the greater variety of mesh parameters, the harder that would be...

If you are talking about hexa blocking (structured meshing), then it becomes simpler and you can calculate the number of nodes or elements you want in each block and then back calculate the required edge parameters...

Usually, we use experience or trial and error with setting mesh params and seeing how many elements result for a particular model. If you want to scale things up just a bit, you can adjust the Global Element Scale Factor...

[gi12]

Thank you very much for your reply
Any mesh morphing capability in ICEM? the FLUENT mesh morpher is not clear
Thank you
GI12

[PSYMN]

No, not in ICEM CFD... There is one in ANSYS Meshing, but that is beta...

But actually, the Fluent Mesh Morpher just got decent for 14.0 (promoted from beta to release for 14.0)... It is not fancy like RBF-Morph which also works well in Fluent), but it is included at no extra cost ;^) and has powerful integration advantages because it morphs the mesh inside the case file while the solver is running (no expensive I/O or restarting).

You can get presentations about it on our website... I presented one over a month ago at the Houston conference and again last week at the conference in Irvine California... Go to the ANSYS website and you can download those presentations.

Best regards,

Simon

[PSYMN]

Just an FYI, ANSYS 14.0 release is planned for 4 to 6 weeks from now...

[gi12]

Hi PSYMN
Can you define the number of nodes in a curve for tet meshing? I know that is possible for Hex meshing , but for tet meshing number of nodes identifies the maximum size not the exact number of nodes and I always do not get the same number of nodes I entered.

Many Thanks

[PSYMN]

It depends on the tetra method...

If you use delaunay or Advancing Front, it starts from the sizes set on the curves to mesh the curves (so you get exact sizes). From there the surface mesh is marched across the surfaces, and then from the surface mesh it generates the volume mesh. So with those meshers, the answer is yes. You can right click on curves in the model tree to display the curve sizing, you can use the Mesh tab to adjust the curve node distributions, biasing, etc. on the curves.

However, if you are using patch independent tetra, it uses a top down method that starts with the volume mesh and ends up fitting to the surfaces and curves after the mesh is refined. This method looks as the general sizing on the curves and surfaces and uses it with the Octree algorithm (you can check the help for specific details on this algorithm) to decide if the mesh needs to be refined or not. This method does not give you a precise use of the curve node distribution, it just uses the base size to decide (yes or no) to a further level of refinement. In fact, with octree, each level of refinement just splits the elements in half from the previous level, so control is approximate and sizes are limited to powers of 2 over the min size.

Read more about the algorithm in the help and you will get a good appreciation of how it is using your meshing parameters. I find this awareness helps users set their parameters more simply and more quickly.

[gi12]

Thanks PSYMN.. That was really helpful
One more question please, is it possible to export XYZ nodes position as a txt file for a selected part?
Many thanks in advance
GI12