Hello, I was looking into
I was looking into ways of simulating a moving mesh, specifically where the motion is determined based on the result of the CFD solution of the previous time step.
I was wondering.... can the various topological changes possible in OpenFOAM such as adding a layer of cells and removing layers of cells, and the sliding interface, be implemented also on complex meshes generated say... using Netgen, and converted into the OpenFOAM format, or do they only work for meshes created using blockMesh?
Also, has anyone tried solving incompressible turbulent flow systems with mesh motion using meshes of industrial level complexity ? With around 400,000 to 1 million cells?
I have been using OpenFOAM for over two months now, with really great results with incompressible steady state turbulent simulations, and I now want to move ahead to transient moving mesh simulations of basically the same system (A hydraulic valve).
Have a nice day!
Hi, Well, enjoy the moving
Well, enjoy the moving mesh - I have to say I am pretty proud of it and various people have done some pretty cool things with it.
The setup of topological changes is independent from the way you built the mesh in the first place. This is very important and hinges on the fact there is no special hidden requirement in the topo change module. I have recently described the topo change implementation as "set and forget": it is meant to be autonomous and fully self-contained. For example, if you wish to define cell layering, you need to pick a set of faces from the mesh which define your "source" and "sink" of cells and make them into an oriented surface (= zone). The surface must have a front and a back; thus, the face zone is basically a list of face labels and a bool for each face telling me to flip it or not. Once you have an oriented surface, you define the min and max cell layer thinckess... and that's it!
I'm not sure I understand the question about "industrial complexity meshes". In fact, there are industrial users already using OpenFOAM (no name dropping allowed) and I personally run 5-10 million cell meshes on a regular basis. Because of the polyhedral mesh support, there are no issues with complex geometry. I would recommend using your CFD knowledge when setting up the discretisation: OpenFOAM does not aim to provide "default settings".
For transient moving mesh, Zeljko and I have some pretty good fluid-structure interaction solvers running and it's quite good fun.
Hi Hrv, Thanks for such a p
Thanks for such a positive sounding reply :-)!! Always nice to start something on a upbeat note! And wow... 5 - 10 million cells... thats something I cant even remotely think of now due to system limitations!!
I read about the concept of a cell zone with min and max layer thickness from an OpenFOAM Wiki article on setting up dynamic meshes... and I ran the movingCone example in the tutorials of OpenFOAM 1.3 (in icoDyMFoam)
The dictionary "dynamicMeshDict" had two lines... dynamicFvMeshLib and dynamicFvMesh which were not too clear to me....
Is the tetDecompositionMotionSolvers written specifically for the movingCone example, or can that be used in general? And... what exactly does the "dynamicFvmesh" line define?
Also... there is the concept of Mesh motion without topological changes, and mesh motion with topological changes.... wouldnt any mesh motion result in a change in the topology? As in... I always need to add or remove layers of cells and have sliding regions when I need one part of the mesh to move in relation to another right?
Would you happen to have a slightly more complex example than the moving cone one with a 3D mesh rather than a wedge?
I am not actually looking at simulating Fluid structure interaction... its more a situation where I have a solenoid moving a spool... so the system is force balanced, and with increasing static pressure and flow forces... the motion of the spool is effected, since the magnetic force is constant for a given current and position.
Thanks for the response! Need to do some more code digging :-)!
Have a nice day!
Hello, I want to simulate a t
I want to simulate a turbulent flows with mesh deformation.
Therefore I looked at the "icoDyMFoam" solver.
1) There the U-Equation is solved including the face fluxes (fvc::meshPhi).
Later within the PISO loop, these fluxes are no longer included. Is this correct?
As I asume it is, why?
2) If I include a turbulence model, can I just include an additional equation, as in "turbFoam"?
Do I have to include the face fluxes in this equation?
Thanks in advance
Hello Ralph, Some time bac
Some time back, I had the same requirements... a turbulent solver capable of handling mesh motion... and here is the result... :-)!
It would be great if you could try it out, and even better, if you could validate the results you get with experiments to see if everything works fine.
Basically, I just mixed together turbFoam and icoDyMFoam, and so far, I have not seen any really weird results, so I think it works... In case you do find some bug, it would be great if you could correct it, and repost it.
Have a nice day!
Thanks a lot Philippose, it
Thanks a lot Philippose,
it looks to be what I was looking for.
IŽll tell you about my experience with your solver.
|All times are GMT -4. The time now is 17:15.|