CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   NOT equal HEAT FLUXES at two sides of SOLID-FLUID interface ??!! (https://www.cfd-online.com/Forums/cfx/121373-not-equal-heat-fluxes-two-sides-solid-fluid-interface.html)

 topsedar July 26, 2013 11:11

NOT equal HEAT FLUXES at two sides of SOLID-FLUID interface ??!!

Hi every Body Here !

I am modelling CHT in a pipe. the outer surface of pipe is subjected to constant heat flux.

my problem is that when i check the results, the values of HEAT FLUX at two sides of SOLID-FLUID interface are not equal. about 400 W/M^2 difference !! but the values of temperature are equal at each side.

I tried to model, using FLUENT software, i found that the value of diffrence is about 1 W/M^2 ..... !

any Idea ?? what would be wrong and what would be solution??

1- mesh problem?
3- CFX software accuracy??
4- .....

 Jan Smedseng July 26, 2013 12:22

Some questions to your case and things you should take care...

Hi.

How did you get the values of the heat flux? Please check this case in the ANSYS CFX Solver by defining a new monitor and selecting Flow >> Domain Interface >> ... >> T Energy and H Energy. Another way is to stop the run and watch the out file.

If you have an fluid-solid interface, you should always use the GGI intersection method (should be default setting).

Do you have defined any energy sources? Have you specified a temperature depended specific heat capacity?

Can you approximate the edge length ratio of the mesh at the interface?

Regards,
Jan

-------------------------
Jan Smedseng
CFX Berlin Software GmbH

 topsedar July 26, 2013 15:28

How did you get the values of the heat flux?

I got this values in CFD-Post:
Calculator TAB ==> Function Calculator , & using the following expressions ::

areaAve(Heat Flux)@Fluid_Solid interface Side 1
areaAve(Heat Flux)@Fluid_Solid interface Side 2

If you have an fluid-solid interface, you should always use the GGI intersection method (should be default setting)

What would be the effect of using a 1:1 interface or automatic method??

Do you have defined any energy sources? Have you specified a temperature depended specific heat capacity?

NO dear Jan

Can you approximate the edge length ratio of the mesh at the interface?

I got confused, what should be check?? :p

 Jan Smedseng July 26, 2013 17:42

Heat flux balance.

Hi.

please use "areaInt(Heat Flux)@Fluid_Solid_Interface 1 Side 1/2" for calculating an balance.

Can you also check the global bilances in the Solver manager?

Please check the "Conservative" values of the area integral of heat flux on both sides of the interface. Try also the variable "wall heat flux".

A 1:1 connection becomes instable, if the gradient of the diffusion coefficient of the connected domains is to high (e.g. thermal conductivity or specific heat capacity between fluid and solid). The wight of one side in the discretisation is to large.

Only use the 1:1 connection, if you have the same material on both sides. That is my personal experience. But that is also the default setting, when using "automatic". So, "Automatic" ist ok :-)

Regards,
Jan

 ghorrocks July 27, 2013 07:24