code_saturne User's Forum

Dear all,

I am trying to simulate the flow field around a tidal turbine immersed in a tank.
The computational domain consists of two parts and two meshes: Rotating cylindrical domain including the rotor+stationary domain with rectangular cross section for the rest of the tank.

I tried to join the two meshes by using the turbomachinery module in the GUI (frozen rotor option applied to the cylindrical domain).
I solved a first error (thanks to this forum) by selecting "groups by section zone" for the cell groups under mesh selection.

I have now encountered a new error cs_boundary_conditions.c:363: Fatal error.

Can someone guide me to understand what went wrong?
(please see files attached )

Regards,

FA

..other two files attached

Hello,

Without the mesh I cannot say more, but did you visualize the location of the boundary condition errors using the ERROR.case (or ERROR.med) output ?

In the case of a turbomachinery mesh, I suspect some joining tolerance/mesh quality issues leaving some slivers of rotor/stator inferface faces unjoined, so appearing as boundary faces, on which you may not have defined BC's. Visualisation will confirm/check that easily.

Regards,

Yvan

Hi Yvan,

I opened the ERROR.case with Paraview but I do know exactly what to visualize.
I can just see the BC_type...

Regards,

FA

maybe the image attached of the BC_type can tell something.
few blue patches may indicate where the error occurred: It looks that at the interface between the two domains some faces did not match; I am not sure about this statement though.

Regards,

federico

Hellon

Yes, this seems to be the case. You may also be missing wall conditions on the fan itself, but that part is easier to fix. Checking your rotor mesh surface, you have some very thin faces in some areas (seeming to be construction traces related to a structured or block_structured approach), which probably cause the issues (to avoid entangling meshes, the joining intersection tolerance is proportional to the shortest connected edge of a vertex). Making the surface mes a bit more regular (in the refinement sense) would certainely help.

Also if you are using Code_Saturne 5.2 or above (development), you can use the "explicit coupling" turbomachinery algorithm variants instead of the "joining" based variants. Those variants are less conservative, but in most cases, produce quite similar results, and are more tolerant of mesh refinement differences. (As that coupling is explicit and not implicit, it takes a bit more time steps to reach the "converged" flow, but otherwise works quite OK).

Regards,

Yvan

Hello

Thank you!
Is the "explicit coupling" an option available in the GUI with the newest development versions?

Now I am using the version 5.0.8. I will try to couple the "tank" domain with the "rotating" one through the user subroutines.
By doing this, Am I able to perform a steady simulation with the frozen-rotor approach?; in other words
can I do the coupling by using as well the turbomachinery module? ( I would like to impose a rotational velocity for the rotating cell zone..I guess, If this is the case, I would not need to prescribe any rotation vector through the "cs_user_parameters.f90").

Regards,

FA

Hello,

Yes, you can coose the method (transient/frozen rotor and joining/coupling) in the GUI in version 5.2.

I beleive you can do a steady simulation using the frozen rotor approach, though I am not sure of this (I would need to check with the turbomachinery expert who updated to code for this).

Also, when using the coupled variant in 5.2, only the turbomachinery approach choice in the GUI needs to be changed, while in older versions (including 5.0 at least for the frozen rotor), it was necessary to run a coupled computation using the 2 domains separately... So upgrading is definitely a good option if you have mesh joining issues and need to check the coupling approach.

Regards,

Yvan