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

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 July 26, 2013, 11:11 NOT equal HEAT FLUXES at two sides of SOLID-FLUID interface ??!! #1 New Member   Hossein Join Date: Apr 2013 Posts: 20 Rep Power: 6 Sponsored Links 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
 Sponsored Links

 July 26, 2013, 12:22 Some questions to your case and things you should take care... #2 Member   Jan Join Date: Jul 2013 Location: Berlin - Germany Posts: 35 Rep Power: 6 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.

 July 26, 2013, 15:28 #3 New Member   Hossein Join Date: Apr 2013 Posts: 20 Rep Power: 6 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??

 July 26, 2013, 17:42 Heat flux balance. #4 Member   Jan Join Date: Jul 2013 Location: Berlin - Germany Posts: 35 Rep Power: 6 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.

 July 27, 2013, 07:24 #5 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,735 Rep Power: 106 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?

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post octavyo CFX 10 April 10, 2017 16:57 alfaruk CFX 14 March 17, 2017 07:08 Anna Tian CFX 1 June 16, 2013 06:28 Suyash26 ANSYS 4 April 22, 2013 15:59 Chander CFX 2 May 1, 2012 20:11

 Sponsored Links

All times are GMT -4. The time now is 14:51.

 Contact Us - CFD Online - Top