CFD Online Discussion Forums - Using variable values at domain interface across the domains

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- CFX (https://www.cfd-online.com/Forums/cfx/)

- - Using variable values at domain interface across the domains (https://www.cfd-online.com/Forums/cfx/215403-using-variable-values-domain-interface-across-domains.html)

Using variable values at domain interface across the domains

Two domains: Fluid, Solid.
In one of the boundary conditions in Solid domain, I want to use the values of one of the variables available for the Fluid domain (say, Absolute Pressure).

It does not seem like CFX allows a usage of variables in this manner (or at least I am not aware of it, yet.)

What bugs me is this: Since the location of the boundary(created by a Domain Interface) in the Solid domain and the boundary in the Fluid domain is physically the same, shouldn't CFX allow users to use the values of variables in this manner?

Anyway, please tell me if there are any ways this can be achieved.

What are you trying to do?

Hello folks,

I've got the same problem. I am simulating flow of a variable composition homogenous gas mixture through a Porous Domain, which is in contact with a Solid Domain. In addition, I am modelling Electric Current through the Porous and the Solid Domain as well as heat transfer in all domains. Now, I want to set an Electric Contact Resistance at the Solid Porous Interface that depends on the local Electric Current Density and the local mixture compositition. Trying to do so, the solver quits before the first iteration with the following error:

Code:

  +--------------------------------------------------------------------+

  | ERROR #001100279 has occurred in subroutine ErrAction.             |

  | Message:                                                           |

  | The physics setup on domain interface "Interface Foam Wall" c-     |

  | ontains an expression that refers to a variable that is not avail- |

  | able on both sides of the interface. This is not allowed. Correct  |

  | the problem, perhaps by using callback functions that refer to o-  |

  | ne side only.                                                      |

  |                                                                    |

  +--------------------------------------------------------------------+

The problem is that

Electric Current Density is only defined in the Solid Domain. In the Porous Domain, is is called Material.Electric Current Density and is higher than Electric Current Density by a factor of 1/(1-Volume Porosity).
The composition mixture is only defined in the Porous Domain, but not in the Solid Domain.

Does anybody have an advice? I already thought of an algebraic Additional Variable that would solve pt. 1, but not pt. 2.
I also found this thread with a similar problem but no solution: https://www.cfd-online.com/Forums/cf...-function.html

Thank you for your support.

Regards,
DaveD!

Ansys CFX support provides a Fortran Routine that allows to copy variable values from one domain side to the other using CEL:

https://support.ansys.com/AnsysCusto...ns/CFX/2040723

Originally, the routine was designed to model condensation, where the heat flux is calculated for and set as a sink at the fluid-side of a fluid-solid-interface and at the same time set the negative value as a source at the solid-side of the interface.

However, the routine can be used to copy arbitrary scalars from fluid to solid side (vectors and vice versa not tested yet).

The routines come as source text as well as pre-compiled DLLs for Ansys 16.2 under Windows and Linux. However, I had to recompile them for Ansys 2020 R2 under Windows and change the path and the Library Name in CFX slightly, see attached image.https://imgur.com/uL7zqEJ

Regards, DaveD!

Attachment 84019