# Conjugate heat transfer

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

 July 10, 2001, 14:31 Conjugate heat transfer #1 Tamer Elsoukkary Guest   Posts: n/a Dear Gambit users, Can any of you tell me how to specify conjugate heat transfer when meshing volumes in 3D I tested that in 2D meshes and it seem to work just by specifing solid and fluid faces How about just specifying solid and fluid volumes for 3 D why does not that work at all! Thanks,

 July 10, 2001, 15:48 Re: Conjugate heat transfer #2 Scott Whitney Guest   Posts: n/a After creating the 3D shapes (and before meshing) you must connect all faces, edges, and vertices. 1) Create your 3D geometry 2) Click geometry/faces/connect faces 3) Select all faces 4) Hit apply 5) Click geometry/edges/connect edges 6) Select all edges 7) Hit apply 8) Click geometry/vertex/connect vertices 9) Select all vertices 10 Hit apply 11) Make your mesh and continue as usual. If this is not done, then the Gambit meshes will not be aligned (for example what you wanted to be one surface with one mesh will actually be two surfaces with two different meshes). Also Fluent will not allow conjugate heat flow. This seems like a silly step, but sometimes you may want to work on two completely separate parts at the same time (and not have them interact).

 July 10, 2001, 16:22 Re: Conjugate heat transfer #3 Tamer Elsoukkary Guest   Posts: n/a your tip seems to work but I got the following two messages can you explain why? WARN: The call to connect on list of edges resulted in no actual connect operations.WARN: The call to connect on list of vertices resulted in no actual connect operations. By the way, does that work with any type of volumes no matter who many surface they consist of 3 or 6 or more surfaces (cylinder, cube, complex shape)!

 July 10, 2001, 20:18 Re: Conjugate heat transfer #4 Tamer Elsoukkary Guest   Posts: n/a The solid portion of the heat exchnger (tube wall) does not come as solid in fluent but have flow inside and the grid diverge. Can anyone suggest what is the problem?

 July 11, 2001, 00:53 Re: Conjugate heat transfer #5 AJ Guest   Posts: n/a Even if you represent some continuum as fluid in Gambit you can change them to solid as required by you. If you want to just model the thickness of heat exchanger as solid then use : planar conduction in 3D models, it allows heat transfer without modeling the thickness of the solid. AJ

 July 11, 2001, 12:42 Re: Conjugate heat transfer #6 Tamer Elsoukkary Guest   Posts: n/a plz give some tips on how to generate planar conduction is it in gambit or fluent and do I need to mesh any volumes for the solid part of the tube then. Can the tube thickness be inhomogenous ( fines attached!) please highlight necessary steps Thanks,

 July 11, 2001, 21:14 Re: Conjugate heat transfer #7 AJ Guest   Posts: n/a Planar conduction is available only in Fluent version 5.4 or higher. In Gambit you are making two volumes, eg. pipe fluid and outside fluid. The interface wall is BC generated in Gambit. This wall while assigning properties in Fluent you are specifying the thickness and switching on planar conduction on and selecting proper material for pipe material from material panel(left side). Hope it works! AJ

 July 12, 2001, 01:49 Re: Conjugate heat transfer #8 Tamer Elsoukkary Guest   Posts: n/a Yes I use version 5.4 what should I do to start the planar conduction

 July 12, 2001, 04:03 Re: Conjugate heat transfer #9 Greg Perkins Guest   Posts: n/a I suggest you look up the manual and have a good read. Then play around with options. While it takes a bit longer your understanding will be much improved. As stated above planar conduction is activated inside Fluent. Greg

 July 12, 2001, 11:34 Re: Conjugate heat transfer #10 Scott Whitney Guest   Posts: n/a It depends on how you created the surfaces. If during the geometry creation you created two surfaces which sit in the exact same location, then you need to connect faces. If during the geometry creation you created two edges which sit in the same location, you need to connect edges. If you created two vertices with the exact same coordinates, you need to connect vertices. Usually people will not do all three. Thus you probably had surfaces that needed connecting, but your edges and vertices were ok. The warning is just there to let you know that you didn't need to connect them (you can ignore the warning). It should work with any number of complex surfaces, but I have seen in the past that Gambit sometimes misses some surfaces when you have a large number of surfaces. Thus I would connect all the faces repeatedly until you reach the warning, "WARN: the call to connect on list of surfaces resulted in no actual connect operations." I hope that helps.

 July 12, 2001, 11:52 Re: Conjugate heat transfer #11 Scott Whitney Guest   Posts: n/a Since I cannot display pictures on this easily I will describe one heat exchanger boundary. Suppose you zoomed in on one wall with the hot fluid to the left and the cold fluid to the right. There is a wall in between these fluids. You have two choices when it comes to the fluids: 1a) Both fluid sections can be gridded and modeled. Create the geometry for both sections (3D volumes in your case) and mesh both 3D volumes. 2a) Or if you want you can grid and model just one of the fluids - this can be done if you know the other fluid has: A) constant temperature or B) constant heat flux. For this solution method create and mesh a 3D volume that only contains the fluid that you want to model. Delete any volume that relates to the constant temperature or constant heat flux fluid (and thus it cannot be meshed). There are two methods for discribing the wall in between the two fluids. I will start with the simplest. 1b) Create a surface (not a volume) to represent the wall. Thus the wall is geometrically infinitely thin. In Fluent you can then specify the thickness of the wall. Use zero thickness if you expect no heat transfer resistance (thus no temperature gradient over the wall). Use a finite thickness if you expect heat transfer resistance (and thus a temperature gradient over the wall). You can approximate fins by reducing the thickness of the wall from the actual wall thickness (this may take work to ensure a good approximation). 2b) Create a volume (not a surface) to represent the wall. This method is more powerful since the wall thickness does not have to be constant (you can even model the effects of different fin shapes, sizes, and numbers). This wall volume must be meshed and must be specified as a solid (the continuum type button in Gambit). If you need help with your specific model, tell me which combination above you want to use.

 July 12, 2001, 16:08 Re: Conjugate heat transfer #12 Tamer Elsoukkary Guest   Posts: n/a Well I think I unerstand now. But I can't use the planar conduction because it is not really what it is. I need to compute the effect of inner and outer fines effect on the heat transfer. In the beginning I thought there is an easy way to neglect the third dimension conduction which planaer conduction implicitly means. But the options Scott talked about is known for me and they are not planar conduction according to my definition then. Now I have a problem is that the geometry is too complicated and I need grid around the walls ( boundary layer grids) but this option does not work at intersections and not working for faces. I had to split the gometry to several closed pieces (faces) should that make problem when I sweep the faces and connect them into three volumes???

 July 12, 2001, 18:12 Re: Conjugate heat transfer #13 Tamer Elsoukkary Guest   Posts: n/a What does the boundary condition show for a solid is it interior just like fluid but with additional wall and shadow zones inside and outside? I am asking because in one of my trials I found flow developing in the soild zone with is logically incorrect!!

 July 13, 2001, 12:22 Re: Conjugate heat transfer #14 Scott Whitney Guest   Posts: n/a I cannot help you with the mesh around the fins. It may be difficult to get a good mesh. However, if it is broken into small pieces you should be able to do it. If flow develops in the solid region then you forgot to specify it as a solid (by default everything is fluid). This can be done either in Gambit or in the Fluent boundary conditions panel.

 July 13, 2001, 16:58 Re: Conjugate heat transfer #15 Tamer Elsoukkary Guest   Posts: n/a the solid zone come as interior when I open the mesh in fluent is that correct?

 July 15, 2001, 17:08 Re: Conjugate heat transfer #16 Tamer Elsoukkary Guest   Posts: n/a Can anyone send me a griding file that will work on fluent5 has two hexahedrals one inside the other (two concentric ducts) where they have conjugate heat transfer and counter current. Plz just for this elimentry type problem fluent does not work. I now want just to learn how to do simple things before I go more complicated. I did this gird about 20 times now and non-converge!!

 July 15, 2001, 18:33 Re: Conjugate heat transfer #17 John C. Chien Guest   Posts: n/a (1). I need to step in and give you my suggestions: (a). continue on the current appraoch, and you will likely to get the answer after 99 trials, so 20 down and 79 to go. (b). try to get a tutorial sample related to your problem and follow the instructions. (c). sketch your problem with the problem definition, send it to the vendor's support engineer and try to get some technical help. (2). If I were you, I would try the option-c first to see if the code can easily handle your problem or not. (3). And if you are the beginner, the option-b will save you a lot of time. But if you think you are die-hard kind of researcher, the option-a is the common approach. and hope that someone out there has the right solution for you.

 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 Chander CFX 2 July 9, 2011 22:22 enigma Main CFD Forum 2 November 1, 2009 23:53 hvem10 FLUENT 2 October 29, 2009 18:31 shankara.2 FLUENT 0 April 21, 2009 15:55 Mark CFX 6 November 15, 2004 16:55

All times are GMT -4. The time now is 10:55.