CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

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

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By Jan Smedseng
  • 1 Post By Jan Smedseng

Reply
 
LinkBack Thread Tools Display Modes
Old   July 26, 2013, 11:11
Default NOT equal HEAT FLUXES at two sides of SOLID-FLUID interface ??!!
  #1
New Member
 
Hossein
Join Date: Apr 2013
Posts: 19
Rep Power: 4
topsedar is on a distinguished road
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
topsedar is offline   Reply With Quote

Old   July 26, 2013, 12:22
Thumbs up Some questions to your case and things you should take care...
  #2
New Member
 
Jan Smedseng
Join Date: Jul 2013
Posts: 9
Rep Power: 4
Jan Smedseng is on a distinguished road
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 likes this.
Jan Smedseng is offline   Reply With Quote

Old   July 26, 2013, 15:28
Default
  #3
New Member
 
Hossein
Join Date: Apr 2013
Posts: 19
Rep Power: 4
topsedar is on a distinguished road
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??
topsedar is offline   Reply With Quote

Old   July 26, 2013, 17:42
Thumbs up Heat flux balance.
  #4
New Member
 
Jan Smedseng
Join Date: Jul 2013
Posts: 9
Rep Power: 4
Jan Smedseng is on a distinguished road
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
topsedar likes this.
Jan Smedseng is offline   Reply With Quote

Old   July 27, 2013, 07:24
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,958
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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?
ghorrocks is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Difficulty in calculating angular velocity of Savonius turbine simulation alfaruk CFX 8 December 3, 2013 17:51
Question about heat transfer coefficient setting for CFX Anna Tian CFX 1 June 16, 2013 06:28
Another Boundary Condition to The Fluid Solid Interface octavyo CFX 9 May 7, 2013 17:28
Heat transfer between solid and fluid Suyash26 ANSYS 4 April 22, 2013 15:59
Enforce bounds error with heat loss boundary condition at solid walls Chander CFX 2 May 1, 2012 20:11


All times are GMT -4. The time now is 22:20.