'Match Control' option limitations
 

Hello All,

The CFD case is involving the internal Flow of fluid.
Workflow:
1. I created the geometry in the Autodesk inventor.
2. Imported in designModeler to attach 'Named Selections.'
3. after that, I imported the geometry with 'named selections' in the meshing module.
4. generated the mesh using the cartesian body-fitted meshing method; the algorithm created all Hexahedra based structured mesh.
5. Exported towards fluent as '.msh' file.
6. setup the multiphase model; it worked like a charm! Flawless! (less simulation time, higher time steps (delta.t > 1e-3), overall wonderful!)

Now, I want to apply 'translational periodic' boundary conditions, so I decided to follow the same workflow.
Now this time at step 4. in the previous workflow, it is a disaster! I learned that the 'Match control' only workable on a tetrahedron, sweep, and multizone meshing. Not all methods support it, especially the cartesian method overrides it.
Hence, I decided to generate mesh using
1. patch conforming tetrahedra method based mesh,
2. multizone mesh with Hexa-core option,
3. and sweep method based mesh.
Out of the above three methods, only the first two options worked while the sweep method did not create any mesh at all.

With the options that I have, I decided to export the mesh towards ANSYS FLUENT, and none of the meshes worked at all, complete failure, I only received divergence messages.

Hence, my question is:
why can not ansys programmers allow algorithm of 'match control' work with all sorts of meshing methods? Why can the 'match control' option not work with the body-fitted cartesian method?

Now a new/modified workflow,
1. Create the geometry in the Autodesk inventor.
2. Import in designModeler to attach 'Named Selections'.
3. after that, import the geometry with 'named selections' in the meshing module.
4. Generate the mesh using the same body-fitted Cartesian mesh method.
5. Export the mesh with options as ICEM-CFD mesh files.
6. modify the mesh at the two surfaces and generate the periodic mesh on those surfaces so that the element and nodes count will be identical, apply periodic boundary condition at those two surfaces, other than that change nothing at all.
7. Export the mesh towards fluent by creating '.msh' file.
8. import the mesh in FLUENT and proceed towards simulation.

My question is: How to achieve steps 5, 6, 7 in a new/modified workflow?

Please help me; I shall provide any additional resources that are required.
The problem which previously worked flawlessly, now being a complete disaster, is putting in grave depression situations.

Anyone,... out here, who would like to take look in the problem?
Anyone,...?

Hi Ash,


Well-structured questions / workflow. To answer your question, different meshing methods are using different meshing algorithms and some features can be incompatible depending on the implementation.


For instance, linear periodic works perfectly fine with a multizone method but as soon as you want to add a second linear periodic (i.e. 2D periodic setup) sharing a common edge (ex. adjacent master faces share same common edge for Floquet periodic BC) it fails as there are conflicting conditions when the method is called making it in a way “over defined” for the algorithm.


A good starting point to answer your questions:

Is to says that it depends on how the different meshing methods / features were implemented. I would suggest to also have a look into the help > Meshing User guide > Local Mesh Controls > Match Control :
“
The Match Control is supported for the following mesh methods:
Volume Meshing:
Sweep
Patch Conforming
MultiZone

Surface Meshing:
Quad Dominant
All Triangles
“


Now it’s not because there are some limitations that you can’t achieve the mesh that you want. I see two options, call ICEM and apply the periodic meshing constraints in there or use a nice Fluent meshing to create periodic BC with non-conformal interfaces. This is really useful if you don’t want to setup the constraints inside of ICEM. There are some good examples and explanations. The help is your friend ;) > Fluent > User’s Guide > III Solution Mode > 6. Reading and Manipulating Meshes > 6.5 Non-Conformal Meshes > 6.5.4. Using a Non-Conformal Mesh in ANSYS Fluent.

Another option would be to use directly the fluent mesher starting from a watertight geometry.

Have fun ;)

Hi Ash.
Have a good time
Has your match control problem been solved?