CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

initial temperature in unsteady state

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 27, 2007, 16:41
Default initial temperature in unsteady state
  #1
Cristian
Guest
 
Posts: n/a
Hey everybody. I have trouble to find solution for my problem, appearly simple. I must set an initial temperature to a material who lost his heat in time to ambient air, and to observe his maximum temperature evolution in time . Practicly initialy, at the time 0, the material has a temperature bigger then the air, then, there are no conditions, and the material start to getting colder to arrive finaly to the air temperature.

If i set a fixed values of temperature to this material in boundary conditions, this means heat generations, and in time the material will allways have this temperature.

If anyone know why or how to solve this, please help me. Thanks.
  Reply With Quote

Old   July 28, 2007, 00:40
Default Re: initial temperature in unsteady state
  #2
Razvan
Guest
 
Posts: n/a
After solution initialisation, use Solve\Initialise\Patch option in the GUI to set the initial temperature in the solid zone only. Then save your .dat file and start your time steps.

Warning: this is a buoyancy-driven flow, set your case accordingly!

Razvan
  Reply With Quote

Old   July 29, 2007, 13:05
Default Re: initial temperature in unsteady state
  #3
amir
Guest
 
Posts: n/a
Dear Razvan i have same problem(like Cristian but forced convection) i use initilize and patch option,but i dint see any changing on solid zone.(i can only thjermal boundary layer over solid) Best regards Amir
  Reply With Quote

Old   July 30, 2007, 05:30
Default Re: initial temperature in unsteady state
  #4
Razvan
Guest
 
Posts: n/a
Dear Amir,

I do not have a direct answer for you because you did not give me enough information, but the only error I can think you could make in the setup of such case is to mess up the BC specification. The easiest way to setup the BC for this case is to make the grid fully connected in Gambit without assigning any BC at all on the separation line/surface between the fluid and the solid zones; when imported into FLUENT, the solver will detect that there are two different zones in the grid, one fluid and one solid, and it will immediately separate them by creating a wall zone and wall-shadow zone at the interface, and it will also set the appropriate BC for these zones automatically.

All the best,

Razvan
  Reply With Quote

Old   July 30, 2007, 12:24
Default Re: initial temperature in unsteady state
  #5
Cristian
Guest
 
Posts: n/a
Thanks Razvan for your help. It works now with the initial temperature but i obtain a non realistic case, beacause it seems that the material become colder very very slow (1degreeC at 16 hours) and its not possible. This is something like Amir, i did not see any changing on solid zone, and i have already a wall-shadow. You said something that is a buoyancy-driven flow and to set my case accordingly, what that it means?

Thanks a lot.

Cristian
  Reply With Quote

Old   July 30, 2007, 14:23
Default Re: initial temperature in unsteady state
  #6
Razvan
Guest
 
Posts: n/a
Buoyancy-driven flows are a very special type of fluid movements: the driving force in their case is the density gradient present in the flow domain combined with gravity effects. Density gradient is practically omni-present, but it can be safely neglected if the ratio of inertial forces vs. buoyancy forces is sufficiently high.

In your particular case (natural convection cooling), buoyancy forces are fully dominant. So you have to take them into account, otherwise your results will simply be rubbish. This means that, in the first place, you MUST give up on the incompressibility assumption. You also cannot use Boussinesq approximation because the temperature differences are too high, so you need to use IDEAL GAS LAW for density. Another requirement is to activate gravity force (be careful with the direction you specify for it!). The rest of the settings are usual.

I can tell you now that in both your cases, the unphysically slow cooling was due to the fact that your setup wasn't considering the density variation in the fluid region and the cooling was exclusively done by conduction (which, by the way, is very slow in gases, that have a heat conduction coeff. five orders of magnitude lower than metals!!!). Correct me if I am wrong!

All the best,

Razvan

P.S.: You could make a superb animation of this type of flow using density or temperature plots!
  Reply With Quote

Old   July 31, 2007, 06:19
Default Re: initial temperature in unsteady state
  #7
amir
Guest
 
Posts: n/a
Dear Razvan and Cristian i think Buoyancy forec doent have any sensible effecton cooling time. i split a face whit an edge and so create 2 zone, one of those is solid and another one is fluid(air) i assign vilocity_inlet to left edge of fluid zone and outflow to right. indeed flow air cross over the solid. i active energy equation and use unsteady condition and K-e. i want to see its cooling after several minutes. but after 20secs i couldn't see any changing in solid zone. i can see thermal boundary layer over solid wall but seem that air can not cool the solid i hope it be enough explanation ,.please tell me : why solid's temperature is constant? k=100 initial temp of solid:500k(i patch solid zone on 500k) velocity inlet :10m/s-300k Whit king regrds Amir

  Reply With Quote

Old   August 1, 2007, 04:17
Default Re: initial temperature in unsteady state
  #8
Razvan
Guest
 
Posts: n/a
Dear Amir,

In your particular case (forced cooling), buoyancy forces might not have a great importance, and all the recommandations I gave to Cristian do not apply to you too. I have tried and simulated myself a case similar to yours, the only difference being the inlet velocity (1 m/s instead of 10 m/s). The results are: 24 deg drop after 10 s and about 98 deg after 1 min, for an aluminium plate, 10 mm thick. I do not know if this is realistic or not, I'm not a heat transfer specialist. But to me it looks like the cooling rate is too high.

Here is a step-by-step procedure for you:

- define your case completely and initialise the solution (you should use constant density for cooling air, although it is not accurate at all);

- calculate a steady solution, with the energy equation deactivated (to obtain a fully developed flow field);

- switch to the unsteady solver, activate the energy equation and deactivate all the other equations, and continue to iterate using a 0.01 s time-step for example, with only one iteration per time-step;

- monitor the volume-averaged temperature in the solid zone.

One important observation: the time-step size is extremely important, because it heavily influences the cooling rate (higher time-steps result in slower cooling). So you should compare your solution to an analytical result, to be sure that the chosen time-step does not influence the solution too much.

Anyway, there are two other important factors influencing the solution:

- air density, which should be calculated using ideal gas law, especially at the beggining of the simulation, when the temperature difference is largest (the error introduced by the incompressibility assumption is diminishinig with time, but it might be too big at the start);

- heat conduction coefficient for air, which should not be constant, but dependant on temperature (you could find tabulated values for that on the net).

All the best,

Razvan
  Reply With Quote

Old   August 4, 2007, 01:37
Default Re: initial temperature in unsteady state
  #9
amir
Guest
 
Posts: n/a
Dear Razvan first of all i should press my appreciation for your guidance. i follow steps and took you advices but i didn't see any changing on temperature(both solid and fluid) so if you are agree ,i can send my case file for you. whit king regards Amir

  Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
icoLagrangianFoam OF1.6 myNewParticleSolver heavy_user OpenFOAM 16 February 11, 2012 06:15
Orifice Plate with a fully developed flow - Problems with convergence jonmec OpenFOAM Running, Solving & CFD 3 July 28, 2011 05:24
ForcesCoeffs ronaldo OpenFOAM 4 September 14, 2009 07:11
Problems with simulating TurbFOAM barath.ezhilan OpenFOAM 13 July 16, 2009 05:55
MRFSimpleFoam amp cyclic patches david OpenFOAM Running, Solving & CFD 36 October 21, 2008 21:55


All times are GMT -4. The time now is 09:13.