Hello there,

I'm modeling a natural convection problem. I have air contained in a metal cylinder where there is as well a 3D solid heat source. I normally use: -The Boussineq definition for the fluid density -A power density for the solid defined as a source -A power density for the walls that surround the heat source -Presto as pressure scheme -Convection on the outside walls of the metal cylinder etc.

The computation converges sometimes but the system does not heat at all. It remains at the tempeature that I initialize it.

If I turn off the flow the problem converges right away with a residual of somethig e-08. and having the flow and the energy the energy residual is always something e-08 from the beginnig.

I tried different configuration for air like piecewise linear, ideal gaz etc. and nothing allows a steady state heating.

Any ideas about this?

Thanks in advance

Carlos ortiz UQTR

Hi Carlos,

Please have a look at the following issues:

1)when you switch on boussinsque approximation,take care that you specify density and coeff of thermal expansion.

2)The PRESTO scheme is fine ,if the mesh contains hex elements orelse body force weighted is good.

3)Specify the operating density which plays a major role in calculations.

will you please elaborate "power density".I am unaware of it.

thanks, sri

Hi Sri,

>Please have a look at the following issues:

>1)when you switch on boussinsque approximation,take care that you specify >density and coeff of thermal expansion.

This has been done.

>2)The PRESTO scheme is fine ,if the mesh contains hex elements orelse body force weighted is good.

My mesh is indeed of hex type, I have already used both schemes with no succes at all.

>3)Specify the operating density which plays a major role in calculations.

I specify the operating density as the bulk density when the tempeature reaches 60 deg. C inside the cylinder, at a gauge pressure of 14.000 Pa.

>will you please elaborate "power density".I am unaware of it.

I have inside the metal enclosure three solid volumes that dissipate power, so I specify this power in positive W/m**3 for the solids as BCs. For the walls that form the outside of the three blocks I declare COUPLED BCs, a positive power density and a zero thickness. I have already tried planar conduction for these walls with a minimum thickness, but this does not change any thing. The heat from the solids does not propagate into the fluid. So the temperature remains where I initialize it. On the outside of the metal cylinder I declare convection BCs with an h coefficient and a free stream temperature.

As I mentioned before I can not get any energy results if I turn the flow off. The air is contained into the cylinder and there is no air inlet or outlet.

This problem is very similar to the ECC problem in the Fluent tutorial, with the exception that a constant temperature is specified between two surfaces, in my case I specify power density instead.

Thanks a lot for your reply.

Carlos Ortiz UQTR

Hi Carlos,

Few days back I faced the same problem while solving a natural convection problem.I will be in touch with you on this problem.

sri

Don't forget to swtich on gravity!!!!

Ashu

hi

i faced the same problem when i tried to use CHT cuple of weeks ago when i had a fluid and sold domain there where no heat transfer occured between the two domain as spouse to happen and the solution converged so fast without any changes in the temperature profile. after several trial with simpile geometry i discovered that it was fluent6.0. bugs. i reported that to fluent and they promise to fix.

Hi Carlos,

Did you have a look at the flux reports.I feel you have to switch off the convergence criteria and carry on the simulation till the percentage of imbalance in heat transfer rate reported in flux reports is insignificant.Hope this helps you !

sri

Hi Ali,

That's the feeling that I had for quite a while, and of course we recently got the 6.0 version. I will look into that aspect and probably report it as well. Because I tried all possible scenarios and nothing worked.

Thanks a lot and take care.

Carlos

Dear Sri,

I finally solved my problem, at least for now, and of course you are the one that made me realize my mistake by answering to "Deadly" about his problems with a quater model simulation. The quarter model approach may work for a fully developed flow in a pipe, but not for a 3D convection problem like the one I'm solving now. Fluxes were indeed crossing the symmetry planes that I defined.

I got rid of the symmetry planes limiting my quarter model and I closed the geometry. Sure enough the system started heating right away. I have now a physical distribution of velocity and temperature.

All I have left to do now, is using the whole geometry model and refining fluid properties.Thanks a million

Hi

Carlos said the quarter model doesnt work for 3D convection problem.. Hoever, when i checked the fluxes for the symmetry plane i realised tht there is zero flux in the symmetry plane...and also, both my full model and quarter model gave approximately similar results.. So why do you say tht it doesnt work?

My problem is actaully..the fact that the amount of heat in the solid region is very high..2000K!..but i input a high volumetric heat source, due to scaling my model..I dun really know how to solve this problem though i do get temperature distribution...and boundary lyers in my current quarter /full models..

Puck

Hi,

This definitely seems to be a bug.

sri

Ali,

I have to specify that I used a quarter model for a 2D problem in which the fully developed flow was dependent in only direction. That is the case of a laminar flow in a pipe where we specify an inlet and an outlet. (I did this computation by writing my own code though). In the case of the natural convection problem in 3D that I'm dealing with, there is air recirculation so if I use a quarter of the model there might not be continiuty in the flow, except if you look at a 2D cut for a particular region of interest. Like in the case of the ECC problem from the Fluent tutorial.

Now if you have almost the same results for both the quarter and the full model, you have indeed no fluxes crossing the symmetry planes that you defined, that is straight forward.

The fact that you have too much heat might be due indeed to units definition. I had that problem while solving thermal problems with magnetic codes. If you model in mm then everything has to follow the same scale. That is material properties,fluxes etc. and that is not always easy specially if you deal with 3D power density that you need to model in 2D.

The power density in my model, I got it from measurements, and I fed it into a magnetic code that gave me physical results right away, in conjuction with materials properties that I got from handbooks that I did not modify at all.

If you want please drop a line with all the units that you use and the scale that you keep for your model in Fluent and I'll double check for you.

Thnx for replying....

I created my model in Gambit, meaning it to be in cm... So, when i entered Fluent, i kept the units to "m" but changed the scaling factor to 0.01..which actaully scaled the geoemtry to cm..(cos i find that i cant seem to scale in "cm", as the length shown in the units windows doesnt change to cm)

Therefore, i input my volumetric heat generation in terms of W/m3...When i calculated the volume, i converted it to "m" to put in the volumetric heat generation.. Is this correct?..my total volume is 1.17 to the power -6; my power is 1000W i got my volumetric heat generation to about 1.41 to the power 8. Plz help....got little time left:P Thnk you

Puck

Puck,

The steps you followed seem to be right. I did the same for a model that I created in mm in Gambit.

Once I loaded it with Fluent I scaled it to 0.001 by specifying that the model had been created in mm. I used the material thermal properties as specified in the data base, that is in W/m.K an so on.

Now, your power density order seems OK if you do all the computation in terms of cm, cm**2 and cm**3. As far as I'm corcerned Fluent does all the computation in m (Please somebody correct me if I'm wrong)

What is the value of your thermal conductivity? What is your initial volume in m**3. (If possible send me the dimension that you use for your solid )

As an example, I have a volume of 0.0045 m**3 in which I measured a power density of 1500 W/m**3. I specify this solid as having a thermal conductivy of 56.3 W/m.K, and when I run the simulation I obtain a temperature distribution between 294 K and 374 K, which is very physical in deed because I measured those temperatures as well.

Carlos

PS Do you have any means to evacuate heat from your system?. My model is cooled by natural convection on the outside of the closed geometry. I have no velocity inlet/outlet my air is contained inside a cylinder.

hi, thnx for replying....but im baffled by sumthing u said... I computed my volume in m**3 before putting in the volumetric heat generation in the boundary conditions as W/m3. Is this correct.. U said im am correct to calculate my volume in cm..but i didnt do tht..i calculated it in m3..Plz do clarify this..thnk you Also, im actually doing a hair dryer model but a simplified version..meaning i out in disc of volumes as the heating source instead of the coils of wires found in a hair dryer....usinf forced convection, i input a velocity inlet and a pressure outlet....air come in and goes out.. My mass flow rate etc, all seems balanced..

Hope u understand me....Thnk you P.S the dimensions of the discs are 0.5cm radius and 0.25 length....i changed all these in m before puttting in the values to run my iteration... Power source for each disc is 8W

Waiting for your reply..thnks

Puck

Puck,

I new you were dealing with that kind of applications, because that requires indeed a big power density dissipation. If you computed your volume in m**3 thats fine. Based in your disc dimensions

the volume of each disc should be: pi.r**2.h

that is 1.9635e-07 m**3

the power density should be 8/1.9635e-07

that is 4.074e+07 Watts/m**3

is quite normal that you obtain such a huge power density.

Now looking into the electrical aspect of your roblem, that means that the Joule losses in each disc are 8 Watts, which should be equal to:

RI**2

R:resistance of each disc.

I: rms value of the current in each disc.

(if we are not dealing with a high frecuency heat induction problem, in which we have to take into consideration Eddy losses.)

RI**2 might different of the total power applied to the circuit which is expressed as:

P = VrmsIrms ----- VI cos(phi)

Not all that power is necessarly converted into heat

Is too bad that you have little time to finish your project, I could have indicated you how to measure the power density dissipated in your solids.It takes a data acquisition system and some thermocouples. That's what I"ve done for my application.

In regards with your question about cm**3, I meant that if you enter a power density in terms of Watss/cm**3 is fine if you expresss everything else in terms of cm, cm**2 and cm**3. But what I forsee is that all your units definitions are right. The only problem that you have now, is that indeed you are heating too much. I had that problem with an HAHV oven application (Hot Air High Velocity), the power applied to the heating elements was 2500 Watts, and that gave the same kind of results that you get. We had to measure the power density as I told you, to be able to obtain physical results. Otherwise you have to adjust power density values until you get test data results, and that takes time.

Please try if you can to get the electrical parameters of your problem, because from what I can see, you have done everything right up to now.

Carlos

i see it now... Thnx a lot for your advice!!

Puck

Puck,

I hope this will help you solve your problem. I'm into the electrical field and I solved quite a few electrothermal problems before, in which computing the power dissipation was not that obvious, mainly because of circuits configuration and operating conditions, such as the duty cycle, current wave form, power convertion and so on.

That's why we apply when possible the measuring technique which is now of big interest for the automotive industry and the bio-engineering applications. I can send you a reference if you want.

Otherwise you need fine detail aspects of how your electrical configuration works. By all means a power density like the one you use (of e+08 order), is a way too high.

What I recommend for now, is that you adjust your power dissipation until you find physical or nown results. That makes part of the simulation process as well, specially when some specific data is not available. Data validation is an essential part in any simulation process though.

Good luck

Carlos

i see...okie, thnk you