
[Sponsors] 
March 22, 2010, 13:25 
thermal analysis with buoyantBoussinesqSimpleFoam

#1 
Senior Member
Andrea Pasquali
Join Date: Sep 2009
Location: Germany
Posts: 142
Rep Power: 8 
Hi,
I'd like to simulate the thermal anlysis of a car. I'm thinking to use the solver "buoyantBoussinesqSimpleFoam". I saw the post:  Problems about buoyantBoussinesqSimpleFoam solver  buoyantBoussinesqPisoFoam: A detailed explanation I have some question: 1) Is it possible make what I want with "buoyantBoussinesqSimpleFoam"? Or I'm wronging solver? 2) Is it correct to simulate the heat flux of the engine like a fixedGradient for the Temperature? In this case I need the alfa_eff of the engine! If it exists, does anyone know a stardard value of alfa_eff for an car engine? 3) If I have the correct heat flux of the engine, could I use the BC "wallHeatFlux"? Do I set it into T file? Before to try with the car, I'm training myself with a simple model: a hot sphere into a room. I tried before a closed room: T: initialField 298, fixedGradient for the sphere, zeroGradient for the walls p: buoyantPressure for all U: fixedValue (0 0 0) for all Then I tried to add an inlet in front of the sphere and an outlet in the back side of the sphere: T: initialField 298, fixedGradient for the sphere, zeroGradient for the walls, inlet and outlet p: fixedValue 0 for the outlet, buoyantPressure for the other patchs U: fixedValue (1 0 0) for the inlet, inletOutlet for the outlet, fixedValue (0 0 0) for the other patchs But I obtain a strange result. The map of pressure and velocity in a section is not correct: I have over pressure near the inlet and big velocity near the outlet. My results are quite similar to the results showned in the posts above!!! Therefore, I made some stream lines: they start straight and when overcome the sphere, they turn on the right! I though the error was on inlet / outlet BCs! So I started changing the BCs first for inlet and outlet and then for all the patch (I tried also the slip type for the wall) and I entered in a blind loop! Could anyone give me any suggestion? Thank for any reply! Andrea
__________________
Andrea Pasquali 

March 23, 2010, 11:37 

#2  
Senior Member
Andrea Pasquali
Join Date: Sep 2009
Location: Germany
Posts: 142
Rep Power: 8 
Quote:
I tried new BCs: T: initialField 298, fixedGradient for the sphere, fixedValue $internalField for the walls p: fixedValue 0 for outlet, buoyantPressure for the other patches U: fixedValue (1 0 0) for inlet, inletOutlet for outlet, fixedValue (0 0 0) for the other patchs But with poor results... In the end I switch of the gravity g (0 0 0) and now the air flow seems correct and goes straight. But I thinking the results are not correct without g... Can anyone give me any advice? Thank for any reply Andrea
__________________
Andrea Pasquali 

March 27, 2010, 08:24 

#3  
Senior Member
Andrea Pasquali
Join Date: Sep 2009
Location: Germany
Posts: 142
Rep Power: 8 
Hello,
I tried these BCs with gravity on (0 0 9.81). Temperature Quote:
Quote:
Quote:
Could anyone give me any feedback? Does exist in literature any experimental test of a hot sphere into air flow to reproduce with buoyantBoussinesqSimpleFoam? Thanks Andrea
__________________
Andrea Pasquali 

March 29, 2010, 17:46 

#4 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12 
Hi Andrea,
I suggest you not use fixedValue for pressure as outlet unless it is perpendicular to the direction of gravity. In the new solvers, p = P  pRef, so p will be stratified. Using a fixed value outlet will give rather odd results. There is a new boundary called uniformDensityHydrostaticPressure that will do a better job. 

March 29, 2010, 19:04 

#5 
Member
Matthias Walter
Join Date: Mar 2009
Location: Rostock, Germany
Posts: 63
Rep Power: 8 
Hello,
I would like to simulate the filling of a tank with hot water using buoyantBoussinesqPisoFoam but I always get an unphysical high velocity in the middle of the tank. In the initial state the tank is already completely filled with cold water. The tank is a closed cylinder with an inlet at the top and an outlet at the bottom. Both are perpendicular to the direction of gravity. The BCs are: U: fixedValue at the inlet, zeroGradient at the outlet, fixedValue(0 0 0) at the walls T: fixedValue at the inlet, zeroGradient all other patches p: zeroGradient at the inlet, fixedValue 0 at the outlet, buoyantPressure at the walls. The inlet velocity is 0.3 m/s but in the middle of the tank (after 1 second simulation time) the velocity raises up to 0.7 m/s. If I use the buoyantPisoFoam from Version OF1.5dev I get reasonable results with the exactly same setup (max velocity remains at ~0.3m/s). In OF1.5dev the Boussinesq Approx for density is different from the definition in OF1.6. Probably, in OF1.5dev the gravity term is absorbed into the pressure gradient? However, both solvers should give similar results with this setup. So, do I need a special BC for the pressure outlet in OF1.6? Best regards Matthias 

March 30, 2010, 04:17 

#6 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12 
Hi Matthias,
You boundary conditions look fine for this case. Your problem must be somewhere else. 

March 30, 2010, 05:58 

#7  
Senior Member
Andrea Pasquali
Join Date: Sep 2009
Location: Germany
Posts: 142
Rep Power: 8 
Hi Eugene!
How are you? thank you very much for your suggestion. I'm trying the new BC for the outlet. I set Quote:
Now it's running with 1 processor fine. I try to use more processor but I got 1 FATAL ERROR during decomposition step! Quote:
Thanks
__________________
Andrea Pasquali 

March 30, 2010, 07:03 

#8 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12 
The problem is decomposePar does not load the gravity dictionary, so it is not available when the boundary is constructed and therefore causes a fail. This is a general issue with boundaries that try to lookup things from the database during construction  a better solution is to construct fields ondemand.
To fix this, either modify the boundary to check whether g is available before looking it up, or decompose the case with some other boundary like zeroGradient and then manually modify it to the required boundary in each processor directory. 

April 22, 2010, 16:21 
buoyantBoussinesqSimpleFoam: the time step continuity errors blows up to inf.

#9 
New Member
John.B
Join Date: Mar 2009
Posts: 14
Rep Power: 8 
Hi!
I get problems with buoyantBoussinesqSimpleFoam, it must be the mesh or the BC. Checkmesh gives me: ***Number of edges not aligned with or perpendicular to nonempty directions: 21369 <<Writing 42738 points on nonaligned edges to set nonAlignedEdges ... Failed 1 mesh checks. Basically I have a room with a hot cube inside, I use an inlet, outlet, wall, cubewall and empty (2D case). The domains simply looks like: _______________________  _______[]_____________ inlet (left side) outlet (right side) cube in the middle top and bottom is wall empty in the z direction If I run simpleFoam, everything works just fine, but when i start with buoyantBoussinesqSimpleFoam the time step continuity errors blows up to inf. I tried many different variants of the pressure BC, but get the same time step continuity errors every time. Anyone that know why or that has a running case (with inlet and outlet) to send so I can have a look at your setup? Best regards John 

April 23, 2010, 04:20 
problem solved

#10 
New Member
John.B
Join Date: Mar 2009
Posts: 14
Rep Power: 8 
Hi
I converted to a 3D case and switch from empty to symmetryPlane instead. CheckMesh give no errors and the solver works perfect now. John 

April 23, 2010, 15:17 

#11 
Senior Member
Andrea Pasquali
Join Date: Sep 2009
Location: Germany
Posts: 142
Rep Power: 8 
You can't use type empty for your patch if in normal direction of your patch you have more than one cell.
Regards
__________________
Andrea Pasquali 

April 27, 2010, 15:21 

#12 
New Member
John.B
Join Date: Mar 2009
Posts: 14
Rep Power: 8 
Hi,
I am aware of the use of empty patch with just one cell thickness in the third dimension. What I am saying is that using a 2D case with empty patch wont work for me. My solution was to convert to a real 3D case or stick with the 2D case but use symmetryPlane patch instead of empty. John 

May 10, 2010, 04:31 

#13 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12 
After a lot of trouble, I have found that the new buoyantBousinesq line of solvers really are no good for real world cases. The main problem is the grad(p) and gravity density terms have to cancel out in a stationary fluid, but due to discretisation errors in the grad(p) term, this does not happen on all but the simplest meshes.


May 11, 2010, 01:18 

#14 
Member
santhosh
Join Date: Apr 2009
Location: India
Posts: 69
Rep Power: 8 
Hi Eugene,
After a expert like you comments on these set of solver, My soul is relaxing now knowing there are other people also feeling the same heat with boussinesq solvers. Forgive my poetry, I am also these days using boussinesq set of solvers for solving a complex heat exchanger problem. I am also facing the problems in matching with experimental results. I have posted my problems in the following post. uniform heating of fluid region Regards Santhosh 

May 11, 2010, 04:26 

#15 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12 
What would you like me to comment on?
The div(phi)*T term prevents local errors due to nonconsrvation of fluxes in unconverged velocity fields. It is zero at conergence. 

May 11, 2010, 07:25 

#16 
Member
santhosh
Join Date: Apr 2009
Location: India
Posts: 69
Rep Power: 8 
Hi Eugene,
I figured out that little back. Currently I facing convergence problems If I use linear in place of upwind. Also, If you look at the last post in the above thread (uniform heating of fluid region), I posted residual plot with sensitivity of turbulent prandtl number, Initially, unknowingly, I have used Prt=5 in which case solution is converged. Later I thought it is not correct to use Prt=5, so I changed it to 0.8 where I could not get convergence. Can u comment on whether it is proper to use Prt = 5. (I have read an article showing Prt used as turbulence generation due to buoyancy in k equation.) Regards Santhosh 

May 11, 2010, 07:52 

#17 
Member
santhosh
Join Date: Apr 2009
Location: India
Posts: 69
Rep Power: 8 
Hi,
I read with wikie article http://en.wikipedia.org/wiki/Turbulent_Prandtl_number It says Prt range is 0.70.9. So I think I should stick to Prt=0.8 and play with others to get the residual down.. Thanks Santhosh 

May 25, 2010, 09:27 

#18  
New Member
valeria garbero
Join Date: Jun 2009
Posts: 2
Rep Power: 0 
Dear Eugene,
what do your words mean? Quote:
Thank you, Valeria 

May 26, 2010, 01:38 

#19 
Member
santhosh
Join Date: Apr 2009
Location: India
Posts: 69
Rep Power: 8 
My observation is that BuoyantBoussinesq simple foam predicts the flow and temperature profile well. But when it comes to validation (comparing the number) I am finding difficulty.
I tried thermal cavity, the flow profiles are pretty good but validation ( non dimensional velocity and temperature at mid section) is not impressive. The same observation I have found with industrial heat transfer problem. PS: I have used only upwind (first order). I could not do linear (second order) as it is not converging well. Regards, Santhosh. 

May 26, 2010, 02:50 

#20 
New Member
valeria garbero
Join Date: Jun 2009
Posts: 2
Rep Power: 0 
Dear Santhosh,
thank you! I am also trying to simulate a heated cavity immersed in a neutral atmoshere but I am having difficulties to impose boundary conditions on p, U and T. U: I imposed an experimental velocity profile on inlet, a driving velocity on top and noslip condition on wall. p: I imposed buoyantPressure condition on inlet, top, outlet and wall. I tried to impose on outlet both the uniformDensityHydrostaticPressure condition and a stratified profile rho*g*z but the velocity assumed high and unphysical values. T: I imposed uniform profile (T=300 K) on inlet, top and wall (I started to simulate the case without heating to compare the results with those obtained by simpleFoam.. I found some differences in U(1), k and epsilon profiles). There is someone who could help me? Thank you! Valeria 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
wrong values in thermal analysis  Trofrensis  STARCCM+  0  December 7, 2009 06:41 
thermal analysis  caesrinivas  ANSYS  0  October 12, 2009 00:52 
FSI Transient Thermal Analysis  Abduri  CFX  0  December 8, 2008 21:00 
Short Course: Computational Thermal Analysis  Dean S. Schrage  Main CFD Forum  11  September 27, 2000 17:46 
Info: Short Course On Thermal Design of Electronic Equipment  Arnold Free  Main CFD Forum  0  August 10, 1999 10:18 