Multiblocks
 

Hi,

I would like to create a Mesh in multiblock.

For example, you have deux blocks side by side.
What's the boundary condition for the face between two blocks ?

And now, if you have one cylindrical block inside the other. What's the boundary condition ?

Thanks all for your help

if you use blockMesh to create two blocks, it defines that face which is in both blocks as internal face, so you need just when you are going to sub divide those blocks, use the same number of cell face for internal face in both side!

Thanks for your answer.

I have already done my geometrie in my "blockMeshDict" file. It's composed with 12 points, 2 blocks, 12 edges (to create the cylindrical block).

My problem is in the definition of the boundary in "blockMeshDict" file. In fact, I don't know the condition to have a continuity of the ecoulement.
Should I add the orange face (cf. picture) on limits conditions? If yes, what is the associate limite condition in the file "boundary"?

Same question for the second case ...

http://img822.imageshack.us/img822/899/caseauf.jpg

Thanks all for your help

ps: If you need, I can post my "blockMeshDict" and "boundary" files

refer you to my last post, there is no need for specific boundary condition! the shared face between two blocks consider as internalface
so you need just to subdivide that internalface equally in both blocks

Could you also explain your problem so that we may help you more?
I assume that you have something like a conjugate heat transfer problem, right?
In this case, you need to have a boundary condition on the interface.
I assume that this is the case because otherwise it would not make sense to have two boxes next to each other instead of a bigger one with the same volume.

I'll post a clearer answer (I hope ^ ^) in the morning.

Thank you.

Edit : morning in France ^^,

I must study an aerodynamic profil. The object is placed à 0° of incidence and saw a velocity inlet (to simulate is air-speed).

This object is circular, so I chose a circular domaine (to limit cells deformation).

Moreover, I want a linear repartition of the cells (to optimize the number of cells and the simulation's time). The picture 1 shows a uniforme repartition, and the second shows a linear repartition. But, to have good results, the evolution of the coefficient of cell dimensions don't overtake 20%. That's why I create 2 blocks. With this two blocks, I can respect the limite of 20% Exactly, I chose 10%). And the two blocks allow me to do an increasing evolution for the first block and decreasing for the second one.






The picture 3 shows my domaine with the two blocks, and their dimensions. And we can see the initials points on the picture "initial geometrie.

The picture 4 shows the surfaces where I have the inlet and the outlet. The boundary type of the external surface of the cylinder is a bordure.

Yes anon_a, my problem is the interface between the two blocks and the continuity of my flow.... (surface highlight in green).


Here is my blockMeshDict file :

It isn't apparent on the picture, but I have a raffinement around my study object.

:o I hope I was clair in my explications ... And sorry if my english isn't totaly understandable.

Thanks for your help :)

Ok, now it is much clearer.

When I use your blockMesh to generate the geometry, the following appears in the blockMesh report:
This means that all the faces that are common for two blocks (such as faces 10-4-1-7 and 7-1-4-10 in your picture) are considered internal and you do not have to define anything on them. Do not worry about internal faces, unless you want to apply a different solver in each region (and you don't want to here). All conservation properties are satisfied. The only thing you have to take care of, as nimasam mentioned, is to have the same number, position and size of faces.

Regarding the object inside the field, you will have to create it and then you will have to impose a boundary condition on its faces. That's another story.

Other than that, I would suggest also trying to build your mesh another way: After a lot of struggling with many tools, I have recently moved to SALOME, an excellent (French!) program. I believe it will make your life easier, you will get tired very quickly with blockMesh.

Ok.

I will use the same solver for the two volumes : simpleFoam.
I already done a simulation, and my aerodynamic coefficients (Cx et Cz) diverge ... That's why I create this topic.

For the object I already create it and impose its boundary condition. In fact, I simulated my study with a cuboc domaine and the results were corrects. Now I want to refine my results.

So, my divergence problem shouldn't due to the blockMesh ? May be my snappyHexMesh ? Or, my boundary conditions ?


I don't know SALOME, it was validated by professional users ? Did you realise pre-processing, meshing, calcul and post-processing on it ?

Do you mean that your simulation diverges or that the coefficients that you calculate do not agree with the previous results? If it is the latter, maybe something went wrong during their calculation. Does the rest of the field seem ok?

Divergence in a simulation can be (and is frequently) caused by a bad mesh.
After running blockMesh (and also after running snappyHexMesh), you should always run checkMesh, which gives you information about the quality of your mesh.
In your case and without the object inside, I get this warning:
There are various ways to visualize the bad faces (nonOrthoFaces), such as
http://www.cfd-online.com/Forums/ope...e-comment.html
The problem however, is how to correct them in blockMesh. It can get very tricky for complex geometries.

I use SALOME (http://www.salome-platform.org/) to define the geometry and mesh.
Then I export to .unv format and import to OF with ideasUnvToFoam.
It seems pretty professional to me :-)
Some people alternatively suggest enGrid but I have not tried that yet.
Just search a little around this forum and you will find some information.

Yes, the coefficients tant I calculate aren't anormal (10e34), so I closed the simulation and I don't look the field ... I think that I have correctly defined the calcul of the coefficients (because it's the same condition that my cubic domaine).



You're right ! Many faces aren't non-orthogonal. But, like you spotlight it, the problem is how to correct them ...


I'll look this later, if possible I would like to do my study in the same software :(

Using square blocks to mesh a cylindrical domain is bad, and will be bad in any other meshing software as well. Build an OGrid (see picture) and your solution will be a lot better. You can do that in blockMesh.

Edit :


I try to do an O-grid but I have warnings during the generation and during checkMesh.

Can you help me to solve this problem ?

Here is my blockMeshDict file :

One thing you have forgotten is to specify the patches.

Please post your warning messages, so we can help you.

With the patches, the warning messages are so long ...

My complete blockMeshDict is the next :

Thanks for your help !

You had the a series of warnings like
This is because the order of the nodes in the blocks matters. I corrected the blockMeshDict lines 69-88. there is still something wrong with the patches, though.

Thanks.

Edit : It's good :)