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?
2- interface adjustments??
3- CFX software accuracy??
4- .....
Thanks in advanced :)

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

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

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

Nice answer Jan.

On the original question - if the meshes on both sides of the interface do not match then a naive averaging of heat fluxes (with simple area average) will result in the two sides not matching, due to the way the temperature is integrated over the face. The area Ave does not use the full control volume integration points, but the solver does in the GGI so you will get a difference in the two approaches.

Can you post an image of the interface mesh, and you say you get a 400 W/m^2 difference - but over what total heat flow?