|
ANSA mesh for sliding meshes (pimpleDyFoam
Dear users,
I was wondering if you could give me some tips/"best practices" to create a mesh for OpenFOAM with a cylindrical interface where a fan lies in it. I have used the this method: - I meshed everything and define the interface as baffles, then exported to OpenFoam case. Then in the polyMesh/boundary I change manually the baffles patches to cyclicAMI type. I use then the pimpleDyMFoam solver for the simulation, it works perfectly when I start from 0, but then if I write the solution and I restart the simulation, it is not possible due to some error in the interpolation between the faces. (this is due to the following: when I export the mesh to openfoam, the faces of the two patches that baffles creates share the same points instead of one duplicating these points, so writing the solution with the moved mesh does not modify the points of the patches but the points of the cells inside the moved mesh are updated). - I use then the tool of OpenFOAM to duplicate the points (mergeOrSplitBaffles -split -overwrite), it duplicates the points but then I cannot even run the solver. Is there a good method to create sliding meshes for OpenFOAM with ANSA? I think I am doing something wrong. Kind regards, yosuu pd; ansa support in my country cannot give me any tips since they don't have any experience in such meshes. |
Hi yosuu,
Our workflow is a bit different: Define the interface as a wall, so you get two different volumes in ANSA. Next do the meshing of both volumes, with the volumes having a different PID. Only show one of the volumes and all the boundaries (including the interface) of only that volume and use save visible as function. Press invert, show the interface again, rename the interface as interface_slave and use save visible as again. Now open the first "save visible as" saved file and use merge to include the second saved ansa file. You should now have the complete mesh with the interface split in 2 equal patches (interface and interface_slave), which can be wall in ANSA. Now export to OpenFOAM and again manually change the interface patches to cyclicAMI and off you go. I hope this is clear enough? Kind regards, Tom |
Hi there
I just want to add that you can set these two properties as cyclicAMI type in the PID list in ANSA and output the mesh ready to run without need for manual changes afterwards. Then in auxiliaries>Interface create a new interface of type AMI and set it to noordeting type Vangelis |
Quote:
hello Tom Is there any tutorial material for this propeller |
Quote:
Regards, Tom |
Quote:
|
Type ? in each field (patch and neighboring patch)
and select the PID of each side Quote:
|
Hi vengalis
thanks for the help so far my case involve meshing a propeller, or wing which has sharp edges, when ever i press fix quality it automatically deforms shape of mesh by deleting some mesh regions which dont represent the shape that we want to simulate. I have one more question-how to reduce non orthogonality and skewness ?. |
If the sharp angles are very acute then it is not possible to satisfy openfoam criteria for skewness and orthogonality by definition of these criteria.
Can you post an image of the surface mesh where you have the problems? |
2 Attachment(s)
Thanks Vengalis
when I am using scripts for post wrap fix and quality criteria i am getting good results. I will post picture of my propeller, I want to generate a good quality o-grid using hexa_block meshing. your suggestion would be invaluable. |
Hi there
It seems that you have a domain made out of Faces while your propeller is probably in STL mesh and you used wrap to create a CFD surface mesh. It would help a lot if you also had the propeller geometry as Faces. Could you do that? Creating a Hexablock mesh is not an simple task and it would also require the presence of the actual geometry of the propeller as Faces. |
Quote:
Hi Tom, I'm as well trying a Propeller simulation with ANSA mesh in OpenFOAM. I followed the workflow of the two ANSA files as explained. The Dynamic motion is applied to the selected zone. The AMI are generated with AMI weights as perfectly 1. But I get following error just at the first iteration of PIMPLE foam - Not implemented From virtual void Foam::cyclicAMIGAMGInterface::write(Foam::Ostream& ) const in file AMIInterpolation/GAMG/interfaces/cyclicAMIGAMGInterface/cyclicAMIGAMGInterface.H at line 160 Any ideas what it might be? And how to resolve it? Thanks a lot! :) Best regards, Vishwas |
Hi Vishwas,
This message is too general to tell you what is wrong. However it does seem to be on the OpenFOAM side, not ANSA. Maybe check your setup against the setup of the propeller tutorial of OpenFOAM, for version 2206 I have it at: $FOAM_TUTORIALS/incompressible/pimpleFoam/RAS/propeller Good luck, Tom |
Hi Tom,
Thanks for your reply. There were some minor differences in the fvSchemes (my old fvSchemes were adjusted for the MRF simulations). Also the includeEtc "caseDicts/setContraintTypes" was missing in the boundary condition files (which could've been influential point for the AMI patches). But thanks everything is working now. :) Cheers, Vishwas |
| All times are GMT -4. The time now is 00:03. |