# Wall with fixed heatFlux boundary condition

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

 February 16, 2005, 08:55 Hello, for a heat transpor #1 Martin Lorenz (Lorenz) Guest   Posts: n/a Hello, for a heat transport problem I would like to use a fixed heatFlux boundary condition, where 120 W/m^2 flux of heat are imposed on a patch named "inner". Therefore I created the following T file in the 0 directory using FoamX: ... boundaryField { inner { type heatFlux; // Field value value uniform 400; // Heat flux flux uniform 120; } outer { type fixedValue; // Field Value value uniform 300; } } ... UNfortunately, this doesn't work: this simply sets the temperature on the boudary to 400K. Removing the Field Value results in an error message. I don't know why one has to specify both temperature and flux since this would result into an over-determination! Any hints? Another question concerns external boundaries with a heat transfer constant k, i.e. the heat flux is given by k*(T-Tenv), where T is the surface temperature and Tenv is the temperature of the environment. I suppose that one has to use the "mixed" or even the "computed" boundary type, but I could not find any examples in the tutorials. Any help is appreciated. Thanks, Martin

 February 16, 2005, 09:28 That's because there's no suc #2 Hrvoje Jasak (Hjasak) Guest   Posts: n/a That's because there's no such thing as a heatFlux boundary condition - only a fixedGradient b.c. Somewhere in the documentation there should be a section on this. Currently, you are falling into a new-ish gap in the design: if a b.c. is not recognised, it will look for a value and use that; this will NOT allow you to do what you wish. Hrv

 February 16, 2005, 10:11 Hi Hrv, I know that the he #3 Martin Lorenz (Lorenz) Guest   Posts: n/a Hi Hrv, I know that the heat flux is connected with the gradient by J_th = lambda * grad T. But the strange thing is that FoamX allows one to choose "wallFixedHeatFlux" as boundary type for a patch of the mesh! This sets the patch field type to "heatFlux" for the field T! What about the boundaries with a heat transfer constant to the environment? Martin

 February 16, 2005, 12:59 Well, grep heatFlux lnInclude #4 Hrvoje Jasak (Hjasak) Guest   Posts: n/a Well, grep heatFlux lnInclude/* in the main library says nothing, which means the bug is in FoamX. use fixedGradient on the T field with the gradient of J_th/lambda and all will be well. Don't understand the second question... If you mean that lambda is a function of something else, that's no problem either, but you'll need a new top-level code. Enjoy, Hrv

 March 3, 2006, 07:13 Hi, could anybode explein to m #5 newbee Guest   Posts: n/a Hi, could anybode explein to me how the fixedGradient works. I'm running buoyantSimpleFoam on a case with a channel with airflow thru it. The airflow is supposed to be heated by one of the walls which is increasing in temperature thru the channel. I have tried running the case with different gradients of fixedGradient on the specified wall patch. But unfortunetly all I get is air flow with the same temperature as the intital setting of the internal field.

 June 7, 2006, 21:01 I am getting the same effect, #6 ccless Guest   Posts: n/a I am getting the same effect, any luck on this. It seems to only heat up the cells in the proximity to the walls. Basically, not providing any advection of thermal energy into cells next to the ones on the wall. Any ideas on this one?

 October 10, 2006, 06:32 Hi, how can I set a boundar #7 christian_hausmann Guest   Posts: n/a Hi, how can I set a boundary condition to fixedGradient? I want to set heat flux as boundary condition at a wall, but FoamX sets the patch field type to zeroGradient, if I set the boundary type to wall. Any suggestions?

 October 10, 2006, 06:53 Hi Christian! This is the p #8 Assistant Moderator   Bernhard Gschaider Join Date: Mar 2009 Posts: 4,036 Rep Power: 43 Hi Christian! This is the point where one abandons FoamX and uses a text-editor for editing the boundar conditions. Or rewrites the config-files for FoamX (with a text-editor). First route is easier. Not the answer you wanted, I know, maybe someone else knows something that doesn't involve a text-editor. __________________ Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request

 October 10, 2006, 07:20 Hi Bernhard, it doesn't bot #9 christian_hausmann Guest   Posts: n/a Hi Bernhard, it doesn't bother me to use a text-editor. I simply use FoamX, because the tutorials of the documentation are made with FoamX. Do I only have to edit the boundary-file and the T-file of my case? Replace fixedValue by fixedGradient? Can/must I edit a estimated Start-temperature?

 October 10, 2006, 09:49 Hi Christian! I didn't want #10 Assistant Moderator   Bernhard Gschaider Join Date: Mar 2009 Posts: 4,036 Rep Power: 43 Hi Christian! I didn't want to imply you were afraid of text-editors. There is just a point in a man's life where he wants more than FoamX can offer him and you seem to have reached that point quite early (right after the tutorials). Your questions: Yes. Yes. No I think the neccesary field that replaces "value" is called "gradientValue" __________________ Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request

 October 12, 2006, 04:46 Hi, thanks Bernhard for you #11 christian_hausmann Guest   Posts: n/a Hi, thanks Bernhard for you help. I am now able to set boundary condition to fixed Gradient. But how do I treat the dimensions? I have heatflux over walls and airflow through an inlet. The dimension of the heatflux boundary condition is [K/m] and for the Temperature of the Inlet is [K].

 October 12, 2006, 05:08 q = alphaEff * snGrad(T) Th #12 Senior Member   Eugene de Villiers Join Date: Mar 2009 Posts: 725 Rep Power: 14 q = alphaEff * snGrad(T) Thus snGrad(T) = q/alphaEff Your BC needs to look up the turbulence model in the database and then it needs to ask the turbulence model for the near-weall heat transfer coefficient. I might still have some code that does this for another purpose, so let me know if you would like a snippet.

 October 12, 2006, 10:00 Hi Eugene, For some boundar #13 christian_hausmann Guest   Posts: n/a Hi Eugene, For some boundaries I have an airflow with a fix temperature and for others I have a fix heat flux density. Since I know the heat conductivity of the wall my intention was to specify snGrad(T) directly in the T-file. The problem is I don't know how to specify different dimensions in the T file. One dimension for gradient and one for value. If I am totally wrong, I will appreciate it to get a snippet of your code, to solve this problem.

 October 12, 2006, 10:29 You don't have to. Gradient is #14 Assistant Moderator   Bernhard Gschaider Join Date: Mar 2009 Posts: 4,036 Rep Power: 43 You don't have to. Gradient is implicitly "original dimension per meter". Or the more practical view: the dimension of the gradientValue isn't checked anyway. __________________ Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request

 October 12, 2006, 10:45 ? Specifying the gradient of T #15 Senior Member   Eugene de Villiers Join Date: Mar 2009 Posts: 725 Rep Power: 14 ? Specifying the gradient of T at the boundary will not fix the heat flux. Anyway, you do not need to specify the dimensions for the gradient, in the boundary section of the field file: someboundary { type fixedGradient; gradient 2000; } To really have a fixed heat flux, you need to know the heat transfer coefficient between the wall and the fluid: In the evaluate function of your new boundary (drived from the fixedGradient type) put: const compressible::turbulenceModel& rasModel = db().lookupObject(" turbulenceProperties"); scalarField alphaEffWall = rasModel.alphaEff()().boundaryField()[patch().patch().index()]; gradient() == q/alphaEffWall; There are some details that have to be sorted regarding dictionary inputs, the face size and direction of the flux, but I'll leave this to you. nlc, fumiya, murrdpirate and 2 others like this.

 July 10, 2007, 02:58 Hello to all, I'd want to #16 New Member   Oscar G Join Date: Mar 2009 Location: Bogotá, Bogotá, Colombia Posts: 27 Rep Power: 10 Hello to all, I'd want to realize my own heat transfer application but I haven't found specific information about it. Thanks, Oscar

 November 10, 2008, 05:29 hi to all.. I want to simulat #17 emilianyassenov Guest   Posts: n/a hi to all.. I want to simulate Heat flux increasing till in the middle of the pipe than decrease it..which solver I should use?and how to include heat flux in the boundary conditions. best regards, Emo

 November 14, 2008, 12:09 Hello Hrvoje, Could you exp #18 emilianyassenov Guest   Posts: n/a Hello Hrvoje, Could you explain in details how to include heat flux? what is J_th there? thanks in advance Emo

 November 17, 2008, 09:26 hello I want to have fixed #19 emilianyassenov Guest   Posts: n/a hello I want to have fixed heat flux in boundary I am using icoFoam and turbFoam I have included energy equation in them I am using Water in a pipe... how to get that fixed flux on the boundary.. thanks in advance Emo

 November 17, 2008, 11:11 can anyone help me? thanks #20 emilianyassenov Guest   Posts: n/a can anyone help me? thanks EMo

 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 mahe Phoenics 1 July 15, 2008 04:21 pour FLUENT 0 May 20, 2008 08:56 Ssn FLUENT 0 January 25, 2008 04:43 woytex Main CFD Forum 1 August 19, 2004 07:11 Enda Bigarelli Main CFD Forum 1 March 15, 2002 00:13

All times are GMT -4. The time now is 18:54.