[qujianyu]

The model is main about a heat transfer problem between water and hot gas, which are separated by a thin wall. Several question are listed below：
1, How to set different fluid property in seperated fluid domains?i.e. define water in water domain, gas in gas domain.not use multi_fluid mehod.
2, How to set different physics timescales in two separted fluid domain?
3, which boundary condition is proper for a infinite nature convection problem. How about setting all boundary condition with Opening boundary conditon and Opening pressure?
Thank you!

[ghorrocks]

There are two methods to do this:
1) Use a multiphase simulation, and both side of the interface just have volume fractions of one pure phase or the other. If you set this to be a homogenous multiphase model the loss in this method will not be too much.
2) Use the expert parameter which allows different domains to have different physics - search the forum for the exact parameter name.

You cannot set different time scales for both side of the interface. If you are steady state you can use the local timescale factor which automatically does a similar thing, but make sure you use physical timescale steps in the final run to convergence.

I assume you mean a far-field boundary. THis can be done many ways depending on what factors you wish to model. In this case I suspect an opening might be approriate.

[Opaque]

I will be using paths to refer to locations in the user interface.

1 - You can activate non-constant physics for fluid domains by opening the following tab: Outline/Case Options/General. Enable Beta Features, and deactivate Constant Domain Physics.
NOTE: from this point on, you MUST be extremely careful setting up your physics details since the software no longer enforce certain checks, and the CFX-Solver may drastically fail due to an invalid setup.

2 - For steady state cases, you can activate different timescales for each domain by opening Outline/Simulation/FlowAnalysis1/Domain:MyDomain. You will see there is a Solver Control tab within the Domain panel. You can activate Domain Solver Control and set specific values there. Those domains w/o local activation will continue using the global settings from Outline/Simulation/FlowAnalysis/Solver/Solver Control-->Basic Settings

NOTE: if you are familiar on how to set timescales for specific equations at the Outline/Simulation/FlowAnalysis/Solver/Solver Control-->Equation Class Settings tab, you can extrapolate how to do so for specific domains as well. However, such feature is not exposed in the user interface, but described in the documentation under CFX Solver Modeling Guide/Advice on Flow Modeling/Timestep selection.

Hope the above helps..

[qujianyu]

Originally Posted by ghorrocks

There are two methods to do this:
1) Use a multiphase simulation, and both side of the interface just have volume fractions of one pure phase or the other. If you set this to be a homogenous multiphase model the loss in this method will not be too much.
2) Use the expert parameter which allows different domains to have different physics - search the forum for the exact parameter name.

You cannot set different time scales for both side of the interface. If you are steady state you can use the local timescale factor which automatically does a similar thing, but make sure you use physical timescale steps in the final run to convergence.

I assume you mean a far-field boundary. THis can be done many ways depending on what factors you wish to model. In this case I suspect an opening might be approriate.

Hi,
It‘s really kind of you! I have finished the simulation with multiphase method, just as your first advise. As for the physical timescale, I chose a smaller one to avoid bounce convergence, but costs almost 2000 time steps to reach the convergence criterion. It is acceptable for me. Thank you very much!
Someone told me all the boundary set to opening pressure boundary may cause initial value dependent result. Have you ever done the similar simulation before?

[qujianyu]

Originally Posted by Opaque

I will be using paths to refer to locations in the user interface.

1 - You can activate non-constant physics for fluid domains by opening the following tab: Outline/Case Options/General. Enable Beta Features, and deactivate Constant Domain Physics.
NOTE: from this point on, you MUST be extremely careful setting up your physics details since the software no longer enforce certain checks, and the CFX-Solver may drastically fail due to an invalid setup.

2 - For steady state cases, you can activate different timescales for each domain by opening Outline/Simulation/FlowAnalysis1/Domain:MyDomain. You will see there is a Solver Control tab within the Domain panel. You can activate Domain Solver Control and set specific values there. Those domains w/o local activation will continue using the global settings from Outline/Simulation/FlowAnalysis/Solver/Solver Control-->Basic Settings

NOTE: if you are familiar on how to set timescales for specific equations at the Outline/Simulation/FlowAnalysis/Solver/Solver Control-->Equation Class Settings tab, you can extrapolate how to do so for specific domains as well. However, such feature is not exposed in the user interface, but described in the documentation under CFX Solver Modeling Guide/Advice on Flow Modeling/Timestep selection.

Hope the above helps..

Hi,
It is a miracle! Beta Feature works well, Thank you very much. Have you ever done a steady state simulation with different physical timescale for separated fluid domains, or for each equation? How about the result? Is it necessary to finish the simulation with the same physical timescale? In my case. It is a natural convection heat transfer problem. The temperature rise of concern is 19K by the same physical timescale, but 16K by different physical timescale for specific equation. What should be noted is I apply opening pressure to all boundary in order to simulate the infinite situation. Could you give me some advises about the boundary condition? Thank you again.