code_saturne User's Forum

Dear all,

I am using code saturne 5.0.4 on a debian 8 64-bits machine. I am trying to set up a turomachinary simulation. The meshes of both rotor and stator are read correctly (although there are several warning due to the mesh quality provided by SALOME).

The calculation stops at the first step with the following error. Could someone tell me what's wrong?

===============================================================



MAIN CALCULATION
================


===============================================================




===============================================================


INSTANT 0.100000000E+00 TIME STEP NUMBER 1
=============================================================


-----------------------------------------
Property Min. value Max. value
-----------------------------------------
density 0.1179E+01 0.1179E+01
molecular_viscos 0.1830E-04 0.1830E-04
turbulent_viscos 0.3390E+02 0.3390E+02
-----------------------------------------

@
@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@
@
@ @@ WARNING: ABORT BY BOUNDARY CONDITION CHECK
@ ========
@ PROBLEM WITH ORDERING OF BOUNDARY FACES
@
@ number of faces classified by type = 302143
@ number of boundary faces (NFABOR) = 381424
@
@ The calculation will not be run.
@
@ Contact support.
@
@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@@
@


Pile d'appels :
1: 0x7f8b6fdd99c0 <typecl_+0x9a3> (libsaturne.so.5)
2: 0x7f8b6fc9148c <condli_+0xedc> (libsaturne.so.5)
3: 0x7f8b6fdd6500 <tridim_+0x3cc7> (libsaturne.so.5)
4: 0x7f8b6fc7557f <caltri_+0x1d89> (libsaturne.so.5)
5: 0x7f8b6fc4e33d <cs_run+0x55d> (libsaturne.so.5)
6: 0x7f8b6fc4dc95 <main+0x125> (libsaturne.so.5)
7: 0x7f8b6cf5bb45 <__libc_start_main+0xf5> (libc.so.6)
8: 0x400899 <> (cs_solver)
Fin de la pile

Kind regards

leguichet

Hello,

You have (NFABOR) = 381424 (Number of boundaries faces) and you have only set 302143 faces with boundary conditions. All the boundary faces must have an imposed boundary condition.

Check your selection criteria.

Regards,

Luciano

Hello,

Thank you for your reply.

Yes, the interfaces between rotor and stator were not defined correctly by me. I used 'and' instead of 'or'.

My case is running after correcting this error. But I have a furthur question. The interface should be 100% geometrically matched or not? In my simulation set up, the interface surface in my stator (red) is a larger than that of the rotor (blue) as shown in the figure attached here. I am wondering if it will be a problem. The extra part of the stator (red area beyound the blue area on the right) will be automatically considered as wall? Thank you very much!

Kind regards

Zhenlan

Luciano Garelli wrote:Hello,

You have (NFABOR) = 381424 (Number of boundaries faces) and you have only set 302143 faces with boundary conditions. All the boundary faces must have an imposed boundary condition.

Check your selection criteria.

Regards,

Luciano

Hello,

Yes, both interfaces has to match geometrically (you can use different discretization and some small differences i think that it is allowed ) because during the transient simulation the solver join the meshes at the interface.
You can adjust some parameters and also you can check if the joining process goes well doing only a mesh joining test and verify the result (if all the faces were joined).

Regards,

Luciano

Dear Luciano,

It seems that you are an expert in usage of turbomachinery module in Code Saturne.

I hope that you can direct me little bit, and maybe promote a tutorial for usage of this module, which might be based on a Python script I have written to generate a turbine geometry in Salome. I attach the script, which generate a turbine profile with cavities, circle hull, and solid volume as an Air. There is no input and output faces in the geometry of this turbine. It should just rotate and create vortices in the cavities, and between the rotor and stator.

I never used the Code Saturne turbomachinery module, and there is no tutorial in the distribution.
So I suppose that for such case one has to build a hexahedral mesh of the Air, then select faces of the stator wall, and faces of the rotor to be given to preprocerssor. Then the internal volumes of the Air mesh should be moved by the whole algorithm to simulate the rotor rotation, and cretaion of vortices in the Air.

Next step of this tutorial would be introducing of Lagrange particles into this turbine.

Yet right now I cannot make the hexahedral mesh of the Air in Salome so, that it is easy to select the the rotor and stator faces.
It's easy to proceed using second meshing variant - just to make a quadrangle 2D mesh on both stator and rotor pipes, then to make a tetrahedral mesh of the Air. However, I am really not sure that this is enoough to have three these groups to run the simulation using the module.

Could you please tell me, what software for the meshing should I use to proceed with the first meshing variant, or maybe second is acceptable for Code Saturne turbomachinery module?

The script for Salome is pretty flexible. It allows making of a variable number of cavities in the rotor, and their depth is also possible to vary. I hope it may become a basis for a tutorial both for Salome and for Code Saturne together.

Hello,

I'm not an expert, just an user of CS.

Ihave run your script and generate de geometry that you mention, but a transient turobomachinary simulation you need one mesh for the stator (fixed mesh) and another mesh for the rotor (rotating mesh). These two mesh will be joinned at a common interface during the simulation. So, if you script represent the rotor, you need another external cylinder that represent the stator. You can check this following link with some additional information.


https://www.code-saturne.org/doxygen/sr ... inery.html

http://cfd.mace.manchester.ac.uk/twiki/ ... ogress.pdf

You geometry seems to be 2D, so you can create a 2D mesh of quadrangles and then create some layer (extrude) in the z axis.

Regards,

Luciano

Hello,

I attach a very simple case with the python script for the mesh and the CS xml file. In this case the internal object (rectangle) rotate with his mesh (rotor) and the external mesh (stator) is fixed.

This is a typical sliding mesh case. I attach a picture with the velocity magnitude.

Dear Luciano,

Thanks a lot for your help. Especially for a real example, and the advices about meshing.
Now I know how to proceed.
Hopefully, your example can be applied for a little bit more complicated geometry.
Really glad to have here such a wonderful response.
Plrease, use my code as you wish. At least, I hope that it will be useful for you.

Sincerely,
Aliaksandr