[CFXer]

Hello.

I want to simulate the heat exchanger which has counterflow heat exchange.

The working fluid is supercritical CO2 for hot fluid and water for cold fluid.

To apply the real-scale geometry, I have modeled two plates to pre-test.

In upper plate, SCO2 flows to the right direction, in lower plate, water flows to the left direction.

Those two plates are all porous domain, which has porosity and loss coefficient.

I checked isolated fluid regions as 'f' in solver - Expert parameters - Convergence Control - Convergence and Runtime Control option.

Between two plates, I set up Domain interface as porous-porous interface, mass and momentum option free slip wall, Interface Model as Thin material thickness of 0.6mm.

The inlet temperature of SCO2 is 76.2℃, water is 34.6 ℃.

The problem occurs in CFD-post. In the whole domain, the fluid density comes out as water's density : 997 kg/m3

It seems to be mixed through the domain, although I set the isolated fluid region.

How can I proceed this domain? In future, I want to simulate the whole SCO2 heat exchanger domain and water domain as isolated region.

Thank you in advance.

[Gert-Jan]

Did you made the beta option available allowing you to override the defaults Constant physics?
If you don't select that, then CFX-Pre will set the same fluid in each domain, even if these are isolated...

[CFXer]

Originally Posted by Gert-Jan

Did you made the beta option available allowing you to override the defaults Constant physics?
If you don't select that, then CFX-Pre will set the same fluid in each domain, even if these are isolated...

As I checked each domain, It was set as the same fluid, not isolated fluid.

Can you notice me how I can make the beta option? I cannot find where it is.

[Gert-Jan]

In the top ribbon, select Edit>Options
There go to General>Beta options>Physics Beta Features
There select Enable Beta Features and deselect Constant Domain Physics

[CFXer]

Originally Posted by Gert-Jan

In the top ribbon, select Edit>Options
There go to General>Beta options>Physics Beta Features
There select Enable Beta Features and deselect Constant Domain Physics

Thank you!

But a problem has occurred.

While simulating the domain, bounding error occurs.

+--------------------------------------------------------------------+
| Table bounds warnings at: END OF TIME STEP |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| |
| Independent variables went out of bounds while computing the |
| variables listed below using table interpolation. In each case |
| the bounds error was handled by clipping or extrapolation. |
| If this situation persists, consider increasing the table range. |
| |
+--------------------------------------------------------------------+
| |
| Location Name : Domain Interface 1 Side 1 |
| Mesh location : BELG12/IP |
| Routine : MINMAX |
| Variable Name : Static Enthalpy |
| Ind. Variable : Absolute Pressure |
| Bound : Lower |
| Min Value : 7.9910E+06 |
| Handled By : Clipping |
| |
+--------------------------------------------------------------------+
| |
| Location Name : inlet_hot |
| Mesh location : BELG1/IP |
| Routine : MINMAX |
| Variable Name : Static Enthalpy |
| Ind. Variable : Absolute Pressure |
| Bound : Lower |
| Min Value : 8.0027E+06 |
| Handled By : Clipping |
| |
+--------------------------------------------------------------------+
.....

The pressure doesn't have any problem, but because of this error, CO2's property does not accurate.

Do you know why this error occurs? In previous simulation, this bounding error did not occurred.

[Gert-Jan]

In the previous simulation, CFX set all properties to water.
Now it also runs with CO2, where CFX has to determine its properties based on your settings. Probably your conditions are too demanding so CFX can't determine the properties on the run.
You should start with a good initial guess (water and air ideal gas?), such that pressure and velocity already are quite accurate. Then restart with CO2.


If it does not help, your error can be anything and I refer to the FAQ: https://www.cfd-online.com/Wiki/Ansys_FAQ