Errors occur in CFX
 

Hello, I encountered some problems in CFX.

I actually simulate spent fuel dry storage by using CFX. I want to see how to occur heat transfer at the heat transfer fin attached outer of dry cask.

So, I made an full model and added outer fin into the dry cask.

In the dry cask, the fluid domain set to helium(ideal) and atmos set to air(ideal). For that, I used Beta Features->turn off "Constant domain Physics".

And I also made "air-exposure space"(now i named it to atmos). Atmos surround dry cask.
So, for atmos boundary conditions, I set "wall" and "no-slip condition" at all faces except for interface face. And used temperature condition for heat transfer option.

Finally I started solver and error ouccurs...

Error and geometry are attached.

For error about isolated fluid regions, I checked geometry and interface but there is no problem..

For error about IO module, I don't know what it's about.

Please give me some advise..

add pictures about errors

Beta features are designed to be used by experienced users who can debug the sometimes strange ans misleading error messages you get when using beta software. So it would probably be better to model this as a multicomponent fluid and then you won't have to use any beta features - and this is a simple model which won't add much to your simulation time.

The errors about setting pressure levels are saying you have to define a somewhere pressure in each fluid region.

The errors about reading the file suggest some files have been corrupted or deleted. I would regenerate the input files and run it again.

Then,,how can i set the pressure in each fluid region?? Is it differ to set the reference pressure in fluid domain?

And what's means input files?

Thank you for your help!

The reference pressure just sets the offset to the pressure variable. By setting the pressure level you have to define a pressure somewhere in the domain. Using a pressure inlet or outlet is the most common way, or it could be by setting the pressure in an initial condition for a transient simulation.

The input files means the def file.

I realized that the wall boundary conditions at atmos side and top face is wrong.
So, I will set the "opening boundary conditions" at atmos side and top face. (At atmos bottom face, I will set the wall boundary condition.)

And how can i regenerate the def file for my case???

If you don't have a boundary with a pressure level set (relative to the reference pressure), then you can set the pressure level at a specific position in closed volumes. Look for Solver Control>Advanced Options> Pressure level information

You regenerate the def file by updating the simulation setup in CFX-Pre and writing a def file.

Thank you for your answer!! but i set the opening conditions instead of wall condition.
After that i solve my problem!

Really thank you!! I clear my problems because of your answers.