Hi!

As I mentioned in other topics I calculate mixing in a fully developped flow through a rod bundle. I calculated the developed flow by periodic boundary conditions. I changed the periodic conditions to inlet-outlet, because I need to solve diffusion of additional variables.

After writing the new def file with inlet-outlet, I imported the result of the previous calculation (periodic). Than checked by Post, but it was not exactly the same! I did not changed the mesh! Is it possible, that non of the CFX function works correct? (I had similar problem with cloud interpolation...)

How to perform a calculation-chain in which the flow is calculated by periodic boundaries, but the heat transfer, or additional variable diffusion is to be calculated by inlet-outlet boundary calculation?

LEGO

Have you tried the following:

- calculate the flow flied with periodic boundaries

- change the periodic boundaries to inlet and outlet boundaries, using Cfx5cmds.

- rerun the simulation with heat transfer and/or add.variables, with the expert parameter SOLVE FLUIDS = f and SOLVE TKE EPSILON = f

Astrid

Thanks,

I am just performing this calculation!

LEGO

Hi Astrid

I'm afraid this won't work. When Build writes periodic boundaries to the definition file it adds some datasets which the solver reads to determine the periodic node mapping on these boundaries. If you simply change the Boundary Type in the command file, the Solver will get confused.

The best way I found of solving this problem is to import the original def file into a new database in VMI mode, and then re-write the original periodic boundaries as an Inlet and an Outlet.

By the way, you can solve the velocity field periodicity problem by employing user fortran to write the outlet velocities to a file, say, and then read the values in at the next iteration and apply them to the Inlet.

Regards,

Sharks

Yes, you have right. It did not work. (See my new topic: Replace periodic by inlet-outlet pair)

But interpolating did not work neither. The field which was imported was changed. The mesh was not changed. I do not undertand why? What is this VMI mode importing? I used the import method which can be found in the Solver Manager.

Thanx: LEGO

Other possibility:

Remain the periodic as periodic, turn off the solve fluids and solve tke omega, turn on the solve scalar parameters, and change this lines of the ccl:

ADDITIONAL VARIABLE : h01

Option = Conservative Interface Flux

END

by

ADDITIONAL VARIABLE: h01

Option = Value

Additional Variable Value = 1. [kg m^-3]

END

in the inlet. But what to do in case the outlets? Which kind of Options are there to set?

Thanx: LEGO

Aha. Well, I have never tried to change a periodic boundary to an inlet. We sometimes change an inlet to an opening v.v with CFX5cmds. That works fine.

Astrid

VMI = Volume Mesh Import; that's one of the first options you selct when entering Build! It alllos you to work from an imported mesh.

Regarding Cloud Interpolation, it is normal that the field is not the same as you are performing a DWA calculation that will tend to smooth the peaks in particular. That is a known effect of using an interpolation. If you were using the same meshes, or nearly the same (ie the distance between cooresponding nodes < DWA tolerance) then you would not see this difference as the nodal value would get transfered on a one-to-one basis.