[mariashva]

I'm now starting to do some simple simulation using a chip and a heat sink for heat dissipation using workbench fluent. I'm now sure whether my setup is correct because my simulation result is different from the experiment. So please help me check. thanks.
the heat sink is around 60*60*20mm size. chip is attached below with 6W power. The air domain is around the heat sink. I used laminar to solve, and added gravity direction. Then I set the air domain wall to be convective with the wall thickness of 1mm and free stream temperature 290K. Then I coupled the interface between the chip and the heat sink and also between the heat sink and air. Use SIMPLE solver with 2nd order upwind. I thought maybe this can automatically be taken as a buoyancy driven convection case, am I right? The mesh is tet with inflation near the air interface. But after I solve it, the temperature is 375K on the heat sink but experiment measurement was only 338K. And the whole heat sink temperature difference is less than 1K from the bottom to the top. But the experiment shows at least 3K difference.
Please let me know if my setup needs to be corrected. Thank you all for your great help.

[mariashva]

I maybe forgot to set air density to boussinesq. Is it critical?

[Rajaero]

hello, i think you set the problem correctly. i am also doing forced convection b/w solid and fluid domain to find out the h value. i also set the boundary condition and interface very well. but i am also getting the less temperature difference between solid and fluid region. i mean (less heat transfer).
my suggestion for you..
1. check your mesh quality and do the fine mesh.
2. try to use coupled solver with higher order term relaxation instead of simple solver.
3.try to change your reference temperature if you want to find out the h value.
if you know about forced convection problem then give me some suggestions.
thanks in advance...

[mariashva]

thank you for your help. I will do as you suggested. Just one more question. Since I don't need to set the convective heat transfer coefficient value between the heat sink and the air domain, then how is heat transfer being solved between these two? and also, do you mean I can predict the h value based on the simulation results? Thanks.

[Rajaero]

yes, you got the point. we can calculate the h values from fluent by creating coupled or mapped with coupled interfaces. once we create this interfaces then we will get two wall and wall shade in the boundary setup. there we can set a wall temperature. fluent will calculate the h value by calculating heat flux value and with reference temperature (bulk temperature). i did the same procedure but i am not sure about the h value results.

[mariashva]

Regarding the forced convection, I will also proceed to this area but now I don't have any similar experience. I will let you know if I get some results. Thanks.

[paolofug87]

Hi,
Check if your fluid density is set to bussinesq or incompressible ideal gas (often I use the second one). Be user also to use "body force weighted" for pressure in solver.

Good luck

P

Sent from my MotoG3 using CFD Online Forum mobile app

[Rajaero]

i am using ideal gas. why should i use incompressible ideal gas. can you explain clearly ?

thankyou...

[paolofug87]

Just to simplify the simulation, if your problem does not involve great change in pressure but the density is mainly dependent on the temperature you can use incompressible. Anyway ideal gas should be ok

Sent from my MotoG3 using CFD Online Forum mobile app

[Lucas_Gasparino]

Heat transfer in a cfd-thermal case calculates h for you given it knows the temperature boundary later and flow properties. Apparently your setup seems correct, but you might have a mesh problem. You don't need inflation for laminar cases, but I'd rather you have a full hexa mesh (or at least convert to polyhedra). Did you refine the mesh after convergence, to check if wether you have independence or not? Also, what's your element count and maximum skewness? Which gradient scheme did you use? Tet meshes require Green-gauss node based scheme. Would help if you could send some prints of the setup. I believe that the tutorials manual has a similar case. Now, if you're more into coupled heat transfer problems, I'd suggest using CFX, since it's easier to set. Finally, how are your residuals converging? I know it's a lot of questions, but maybe try the mesh modifications first; you might be surprised... Worst case, do a transient simulation and data-sample to get the steady state conditions. Hope it helps

Sent from my XT1635-02 using CFD Online Forum mobile app

[Lucas_Gasparino]

Originally Posted by Rajaero

hello, i think you set the problem correctly. i am also doing forced convection b/w solid and fluid domain to find out the h value. i also set the boundary condition and interface very well. but i am also getting the less temperature difference between solid and fluid region. i mean (less heat transfer).
my suggestion for you..
1. check your mesh quality and do the fine mesh.
2. try to use coupled solver with higher order term relaxation instead of simple solver.
3.try to change your reference temperature if you want to find out the h value.
if you know about forced convection problem then give me some suggestions.
thanks in advance...

Hi mate,

You don't need p-v coupling for this case: just a better mesh, generally.
You'd use a staggered grid if you had something like a shock tube, where pressure gradient dominates the problem, or something driven by pressure on both inlet or outlet.
Natural convection doesn't reckon pressure gradients, so simple should be fine. My point is that you need a decent, unstructured mesh. Also, don't inflate it if your case is laminar, or inflate with a small stacking. It's better to keep element ratios close to 1 in this case. Now, CFX is way easier to setup for thermal convection dominated problems. Also, a bit more on theory you can find in the book Introduction to Heat Transfer, by Incropera and DeWitt. Forced convection is actually easier since you don't need buoyancy. One minor point: remember to set up air as ideal gas, otherwise density doesn't change (p=rRT) and the hot air will be stuck close to your dissipator.

Hope it helps

Sent from my XT1635-02 using CFD Online Forum mobile app

[mariashva]

But roughly how different would there be between bussinesq and incompressible ideal gas?

[Lucas_Gasparino]

These are two different things: one is a material model and the other a physics model. You need to use boussinesq model to capture movement driven by buoyancy, but also the material must allow density change. So they work in conjunction.

Sent from my XT1635-02 using CFD Online Forum mobile app

[mariashva]

Thanks. I may have some setting problems. I didn't use Green-gauss node based scheme, so I will use this one for another try. The mesh is difficult for hex. so I use tet instead. I thought 2nd order would decrease false diffusion. from my previous settings, the continuity and velocity can not converge to 10^-3 or lower, so maybe it is because of the few problems you mentioned. I will try more and let you know if I can get better results. Thanks.

[Lucas_Gasparino]

First, go on the Monitors section and edit the residuals: change from 0.001 to 1e-5. Keep momentum as 2nd order upwind and activate Boussinesq. Redo the mesh without inflation, but try to use hexa elements; then you can use LSQ cell based. As I said, inflation is more useful for turbulent flows, where you need to keep y+ at a controlled level. When you remove inflation, it will be easy to generate hexa if your geometry isn't too complex. Other way around us to use mesh\polyhedra\convert-domain in fluent, which will merge tets.

Sent from my XT1635-02 using CFD Online Forum mobile app

[mariashva]

one more question is that, if I have a long and thin metal sheet for convection. how would you recommend me to do with the mesh of this thin material?

[Lucas_Gasparino]

Don't hahaha fluent has interface exactly for that hahaha alas, if you must represent the sheet, don't try a 1:1 mesh mapping: your film will invariably be more dense always, so it's better to mesh with a 2:1 correspondence. Also, use ICEM in this case, as it's just a better mesher when you need broken connections. Fluent Tgrid is also useful. In general though, you want at least 4 elements through thickness in the film.

Sent from my XT1635-02 using CFD Online Forum mobile app

[mariashva]

Thanks. I tried to get all hex mesh. I slice some parts to make them easier. But some other parts (fluid domain) is just too complex. So my currently solution is to get all the other parts to be hex, but keep this one fluid domain to be tet but with relatively small mesh size. Would it be a big problem? I'm still waiting for the results.

One more thing during my setup is that, when I define the mesh interfaces, Fluent doesn't always automatically show the right interfaces between different domains, is this normal? then I have to set some of the interfaces manually. Regarding the interface between fluid and fluid domain or between fluid and solid domain, should them all be set as coupled wall？I know that normally there should be one interface from one part on the target side, and another one interface from another part on the source side, but sometimes I face the situation in which the target side has more than one interfaces from two or even more parts, and source side is the complete fluid domain interface. If I coupled them all together, should it be ok? Thank you very much for your help in advance.

[paolofug87]

I'll suggest to bundle all part in one assembly body in design modeller in order to build automatically a conformal mesh and let fluent to set up all contact regions. Tell me if I'm wrong please, I'm also interested in that argument

Sent from my MotoG3 using CFD Online Forum mobile app

[Lucas_Gasparino]

Ok, long question long answer hahahaha...
1st, tet mesh for CFD is acceptable, but you'll need way more nodes/elements to get decent results. Also, with tets you can't use cell based methods, which are superior if you use LSQ formulation.
About interfaces, that can be though to setup in Fluent: I suggest that you spend some time in the Ansys meshing defining manually the contact/interface regions using named selections that start with interface. This way, when. Fluent reads the mesh, it will id those regions correctly. About mesh connection, yes, it's defined as coupled wall, although that's default setting. The mesh doesn't need to be 1:1, but try to get as close as possible to that, by manual inspection (visualize if any element face shares more than one node). Just remember to define which interface is solid and which is fluid...
About hex generation, if you send me an image of your geometry I can suggest some ideas on how to generate an unstructured hexa mesh without too much trouble. Remember, your case is laminar, so no need for inflation . Also, don't exaggerate on sizing, you don't need too many elements for this case. If you can identify a sweeping path, use this to your advantage and define a sweep method for meshing, with hex dominant option. TBH, just for learning purposes I'd do a 2D case, it's less troublesome and demanding of PC resources. What's your hardware?
If you send me the geometry file, I can try creating a video tutorial for you guys.

Sent from my XT1635-02 using CFD Online Forum mobile app