[CFXer]

Hello.

I'm simulating some fluid dynamics.

Domain 1 and 2 are connected by domain interface, same fluid passes through.

Domain 1 should be calculated as "turbulent" and Domain 2 should be estimated as "laminar".

But when I used domain interface of each "turbulent" and "laminar" interface, error occurred.
+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Equation subsystem: "Wall Scale - 1" has not been found on both s- |
| ides of interface "outheader_outlet_header". Check that you have |
| set consistent physics across all domains that use this interface- |
| . |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine DEF_ALGM_SUBSYS_ZIF |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+


I have to use Turbulent / Laminar interface.

How can I do this? someone please help me.

[Gert-Jan]

I have seen turbulent and laminar settings together in 1 CFX-simulation, but only in an application where both were defined in 2 unique domains separated by a solid. You are connecting both domains directly using an interface. I don't think this is possible in CFX. If I would like to do this, I would go to Fluent, where this can be achieved by setting a volume as Laminar zone, even if it connected to a turbulent zone.

But alternatively, use the SST model which converges to a laminar solution if the conditions a laminar. At least, I have seen parabolic velocity profiles in a straight tube corresponding to laminar conditions. Not sure if this will be achived in your application....

[ghorrocks]

Some suggestions:
* Use the SST turbulence mode as Gert-Jan suggests. If you use SST on a laminar flow in most cases it still gives you a result very close to the laminar result. SST handles zero turbulence nicely (unlike k-eps).
* Use the transitional turbulence model with specified intermittency. This allows you to explicitly set which areas are laminar and which are turbulent.
* Do the laminar and turbulent bits as separate simulations, replacing the interface with a boundary condition. This will only work if you can approximate the interface with a relatively simple boundary.
* You might be able to get this to work by setting the non-constant domain physics expert parameter, but I suspect it will not work as the boundary will cause undefined turbulence parameters.

[Opaque]

Q: what are you trying to achieve by splitting the turbulence model spatially?

The turbulence model requires boundary conditions at inlets, outlets, walls, etc. When the model is split, it requires a boundary condition at the split interface.

Ignoring how to implement them in the model, how would you realize the value of those conditions?

Perhaps it is best to describe your modeling goals, and let others in the forum pitch in some suggestions.

[CFXer]

Originally Posted by Opaque

Q: what are you trying to achieve by splitting the turbulence model spatially?

The turbulence model requires boundary conditions at inlets, outlets, walls, etc. When the model is split, it requires a boundary condition at the split interface.

Ignoring how to implement them in the model, how would you realize the value of those conditions?

Perhaps it is best to describe your modeling goals, and let others in the forum pitch in some suggestions.

Thank you for all of yours reply.

My simulation is heat exchanger with plate structure.

I uploaded my domain structure to the image.

In plate parts, when I applied turbulence model, the heat transfer coefficient did not work.

So, I applied non-turbulence(laminar) model to the porous domain, It works very well.

So, I should apply fluid domain with turbulence model in header, porous domain with laminar model in plate.

Separate simulation could not be applied because the header and plates are related strongly.

[CFXer]

Originally Posted by ghorrocks

Some suggestions:
* Use the SST turbulence mode as Gert-Jan suggests. If you use SST on a laminar flow in most cases it still gives you a result very close to the laminar result. SST handles zero turbulence nicely (unlike k-eps).
* Use the transitional turbulence model with specified intermittency. This allows you to explicitly set which areas are laminar and which are turbulent.
* Do the laminar and turbulent bits as separate simulations, replacing the interface with a boundary condition. This will only work if you can approximate the interface with a relatively simple boundary.
* You might be able to get this to work by setting the non-constant domain physics expert parameter, but I suspect it will not work as the boundary will cause undefined turbulence parameters.

Thank you for your kind reply.

After I set the transitional turbulence model, how can I set it?

In case of fully turbulent, intermittency = 1.0 or just fully turbulent,
and laminar, intermitency = 0?

And could this method apply the heat transfer based on laminar condition?

Thank you in advance.

[ghorrocks]

Before we get into the transitional turbulence model, let's just follow up Opaque's comment as your answer puzzles me.

What did not work when you made the whole thing turbulent? Please attach the output file. This is the best way to get it working (if it is applicable), so we should try to get the fully turbulent approach working first.

Can you describe why you are using a porous domain for the plates? Please show an image of your model.

[CFXer]

Originally Posted by ghorrocks

Before we get into the transitional turbulence model, let's just follow up Opaque's comment as your answer puzzles me.

What did not work when you made the whole thing turbulent? Please attach the output file. This is the best way to get it working (if it is applicable), so we should try to get the fully turbulent approach working first.

Can you describe why you are using a porous domain for the plates? Please show an image of your model.

Between the hot and cold plate, the heat transfer occurs.

I used porous domain to reduce the computing cost.

So, I used friction factor and Nusselt number correlation between hot and cold fluid.

When I did a simulation with fully turbulent model, the heat transfer coefficient goes to very high value, so input correlation doesn't work.

I think it is because of the turbulence model's heat transfer characteristics.

When I turn off the turbulence model with only porous plates model, the heat transfer coefficient work very well.

[ghorrocks]

Then isn't your problem how to get the heat transfer accurate in a turbulent simulation?

[CFXer]

Originally Posted by ghorrocks

Then isn't your problem how to get the heat transfer accurate in a turbulent simulation?

Yes it is.

You are right

[ghorrocks]

So then your question is how can you make the heat transfer more accurate.

Have a look at the FAQ on accuracy: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

Key points are:
* What Reynolds Number and/or Rayleigh Number are the tubes running at?
* Have you done a mesh refinement study? You really need to do this if you want to be accurate.
* What turbulence model are you using? Why? And what turbulence boundary conditions have you applied?

[Gert-Jan]

Do I understand corectly that you are using a porous region to separate hot and cold parts? As if it is a wall?