[kel85uk]

Hi all,

Am still new to this free surface tracking solver, and I am trying to solve a similar problem as the one in the tutorial, but how do I change the size of the bubble to different initial diameters?

Thanks.

-kel85uk

[Bernhard]

The surface tracking solvers (I think you refer to bubbleInterTrackFoam?) are based on seperates meshes for different phases. For changing the bubble diameter, you need a different mesh. The easiest way to do this, is to rescale an existing mesh, you can use the utility transformPoints for that.

[kel85uk]

Hi Bernhard,

Thank you very much. Will try that and see.

-kel85uk

[kel85uk]

Hi,

Another quick question. How would I go about re-meshing the problem since scaling only changes the dimensions, and I might want to change the number of cells?

Many thanks.

Regards,
kel85uk

[Bernhard]

You can either use the refineMesh utility or make a mesh yourself.

[kel85uk]

Originally Posted by Bernhard

You can either use the refineMesh utility or make a mesh yourself.

Yes, I'd probably want to make the mesh myself, but how to make the shadow zones? I have no idea how to start because the blockMeshDict is not present... Any help on this would be much appreciated.

Thank you.

Regards,
kel85uk

[Bernhard]

You need to make two seperate meshes (can be done with blockMesh). Define the interface twice, for one fluid, call it freeSurface for the one, and freeSurfaceShadow for the other.

[kel85uk]

Originally Posted by Bernhard

You need to make two seperate meshes (can be done with blockMesh). Define the interface twice, for one fluid, call it freeSurface for the one, and freeSurfaceShadow for the other.

Hi Bernhard, sorry for the trouble again, but how do I make the refineMesh? I seem to get empty cells and the cellIDs are all over the place when I checked I converted it to VTK file format.

As for blockMesh, how do I merge the two separate meshes? Is it also possible if I can do the meshing in Gambit and then import it to OpenFOAM via the fluentMeshToFoam utility?

Thank you.

Regards,
kel85uk

[Bernhard]

To understand how to use refineMesh, copy refineMeshDict from utilities/mesh/manipulation/refineMesh to your case directory.

You don't have to merge the edges in blockMesh. And I don't see why you cannot make the mesh in gambit. Just give it a try. As long as you are consistent with naming the patches on the interface.

[kel85uk]

Originally Posted by Bernhard

To understand how to use refineMesh, copy refineMeshDict from utilities/mesh/manipulation/refineMesh to your case directory.

You don't have to merge the edges in blockMesh. And I don't see why you cannot make the mesh in gambit. Just give it a try. As long as you are consistent with naming the patches on the interface.

Hi Bernhard,

Thank you for the guide, it works properly now in serial using the FLUENT meshes. Any idea how I can use decomposePar for this solver? I read in the OpenFOAM forums that the interface has to be in the master processor, and until now I have no clue as to how to make sure that is the case.

Thanks again.

Regards,
Kelvin

[Bernhard]

In decomposePar you have a subdictionary preservePatches. I've not tested this yet, but maybe this can help you. Please let me know if you get it done like this, because I'm also interested

[kel85uk]

Hi Bernhard,

For the parallelization, it's easier to just use the manual decomposition method with funkysetfields to set the processor weights. However one more problem is with the fluidIndicator file. How do I create it? I searched the forums but they were unfortunately not very informative. Someone spoke about the setfluidindicator function but I have grepped it and found no files mentioning it in the src or even solver directories.

http://www.cfd-online.com/Forums/ope...indicator.html

Any ideas on how to proceed from here?

Thanks.

Regards,
Kelvin

[kel85uk]

Hi Bernhard,

I finally got it to work. The fluidIndicator file is nothing more like the alpha1, so, one can easily set it using funkySetFields. After that, it'll work.

-Kelvin

[chai]

Hi,
Can you explain the meaning of two seperate meshes. does it mean there is no connecting between these two meshese? for example, in my case that bubble rises in the water, there is a small gap between the grids occupied by water and grids for air. am i right?

Chai

[hfsf]

Originally Posted by Bernhard

You need to make two seperate meshes (can be done with blockMesh). Define the interface twice, for one fluid, call it freeSurface for the one, and freeSurfaceShadow for the other.

Sorry for the ressurection of a old thread and making a question that might sound too simple, but how can I create 2 separated meshes with the blockMesh utility? Once I run blockMesh with the configurations os the new mesh, the old one is replaced... I think I'm missing the point here, can anyone explain me please?

[Bernhard]

Just put it in a single blockMeshDict. The vertices on the interface have to be defined twice, to make sure you get two patches. Then you create the patches freeSurface and freeSurfaceShadow.

[hfsf]

Originally Posted by Bernhard

Just put it in a single blockMeshDict. The vertices on the interface have to be defined twice, to make sure you get two patches. Then you create the patches freeSurface and freeSurfaceShadow.

Thank you for so quick answer, Bernard. I will give it a try.