[arun_thakur]

hi,
i am using fluent for a scenario in which air is coming inside the room at a certain temperature and the air inside i want to keep at certain temperature. Purpose is to see the mixing behaviour of air.
but problem is how to give the temperature to the air inside the room.

it may be very silly question. But to be honest i need help on this.

rgds.

[Kwiaci]

You need to create a separate volume for the air in the room, at the boundary of fluid use internal boundary, patch temperature inside the room and choose one of the multiphase models.

[vigneshkumar_t]

Which multi phase option will be better since same air will be for both the domain?

[arun_thakur]

making separate volume is not so easy task for every different encountering problems..and how we can use multiphase when we are taking about same air only difference is temperature...??

[robboflea]

Sorry but I'm missing something. You have a volume (say a room) with air at a certain temperature and a current of air (at a different temperature) coming from a inlet in the room walls. Am I right?
In this case you don't have constant temperature in the room. If you're mixing two air streams at a different temperature you'll never have constant temperature.

Rob

Originally Posted by arun_thakur

making separate volume is not so easy task for every different encountering problems..and how we can use multiphase when we are taking about same air only difference is temperature...??

[flotus1]

What is the point of a multi-phase computation in this case?

Just set the initial temperature of the fluid inside your room to the desired temperature.

At the inlet, set the temperature of the fluid entering your room. now all you need is an outlet and a transient simulation and you are good to go.

Keeping the temperature in the room at a constant temperature all the time would be possible ("Cell Zone Conditions" -> "edit" -> check "fixed values" ->"fixed values" tab -> specify temperature; or via UDF). But if I am not missing something essential here, you would not see any mixing of temperatures since the temperature will be constant throughout the domain.

[arun_thakur]

Originally Posted by robboflea

Sorry but I'm missing something. You have a volume (say a room) with air at a certain temperature and a current of air (at a different temperature) coming from a inlet in the room walls. Am I right?
In this case you don't have constant temperature in the room. If you're mixing two air streams at a different temperature you'll never have constant temperature.

Rob

you are absloute right it could not be constant temperature.It needs a transient case but problem is have tried every thing but results are not coming in favour.

how u define the problem is absolutely right.I have to see the mixing of outside air with the insider air of room.But its not giving the exepcting results. Even in transient its showing all the room temperatrue equal to entering air temp at just start. which could not be possible. in actual walls are insulated too to keep the difference of 10 deg to outside.

either i have to run it pressure based or density based.

i have no clue where i'm making a mistake.

[flotus1]

Would you like to show us the computational domain and the boundary conditions of your setup?

[arun_thakur]

sorry for replying so late. I found out the solution for my problem.

it should be run as a transient and initialization condition should not be the default temp calculated by fluent but here need to put as temerature of air entering inside the room.

[Hybrid]

Would you please share the complete solution what you have done, I have similar problem. Please refer to the link: http://www.cfd-online.com/Forums/flu...wo-fluids.html

[ViLaks]

Sorry for restarting the thread again, but as I am new to fluent, how can I initialise the desired temperature?

Originally Posted by flotus1

What is the point of a multi-phase computation in this case?

Just set the initial temperature of the fluid inside your room to the desired temperature.

At the inlet, set the temperature of the fluid entering your room. now all you need is an outlet and a transient simulation and you are good to go.

Keeping the temperature in the room at a constant temperature all the time would be possible ("Cell Zone Conditions" -> "edit" -> check "fixed values" ->"fixed values" tab -> specify temperature; or via UDF). But if I am not missing something essential here, you would not see any mixing of temperatures since the temperature will be constant throughout the domain.

Thanks and Regards
Vignesh

[KevinZ09]

It's not precisely clear what you're asking, but depending on the complexity of your geometry/problem you can either:
- Just set an initial temperature and initialise your problem.
- Patch the temperature of a certain volume.
- Use a UDF to set the temperature in a certain volume.
- Etc.

Perhaps give some details so it's more clear what solution would be the best for your case.

[ViLaks]

Dear Kevin,

Thanks for your reply.

I am trying to simulate using Fluent natural convection inside a deep freezer geometry, whose walls are maintained at 253 K and the air inside is at 316 K. My aim is to simulate the time required for cooling of air from 316 to 255 K . My questions are:

1) What should be the operating temperature (operating conditions) in my case?

2) Also should the operating temperature and the input density be given as reference values also??

3) AT what temperature should I initialise my problem?
4) How can i set the temperature of air inside the deep freezer to 316K?

I am planning to use the Boussinessq approximation and run a transcient simulation but the material properties are confusing me

Thanks and Regards
Vicky

[KevinZ09]

Originally Posted by ViLaks

1) What should be the operating temperature (operating conditions) in my case?

Set the operating temperature to your initial temperature, i.e., T_0 = 316K. Since you're using the Boussinesq model, you'll also need to specify the expansion coefficient (unless you're using the gas law). And since you're doing an unsteady simulation, you won't need to specify an operating density I believe. If you do have to specify it, you can either choose the density at T_0 = 316K, or don't specify it, then Fluent will just use a cell-average.

Don't forget to specify gravity though!

Originally Posted by ViLaks

2) Also should the operating temperature and the input density be given as reference values also??

Reference values are only for postprocessing when computing non-dimensional coefficients and derived quantities. So you should enter them, and I'd suggest using your initial condition values. However, they won't affect the solution/simulation.

Originally Posted by ViLaks

3) AT what temperature should I initialise my problem?

At T = 316K, since that's your initial temperature. Also, that temperature, along with your initial density/gas law will define the mass in your domain.

Originally Posted by ViLaks

4) How can i set the temperature of air inside the deep freezer to 316K?

If you've only got one volume, just go to Solution Initialization --> Standard Initialization --> set your Temperature and press Initialize.
If you've got multiple volumes, and only want to set the initial temperature in your freezer to 316K, you can use Patch, which you can find on the Solution Initialization panel. Just choose your freezer volume and, after initializing the rest, patch the temperature of that volume to 316K.

Hope this helps. Good luck!

[ViLaks]

Dear Kevin,

Thank you very much for your inputs.

Regards
Vicky

[ViLaks]

Dear Kevin,

I have given 316K in operating conditions (no density). I have also initialised temperature (in soln. initialisation- standard initialisation) to 316K.
My boundary conditions are:
1) constant temperature to walls (left, right, front, back and bottom) of 253 K
2) top wall as adiabatic (zero heat flux).

I have given material properties at 316K to air and density is boussinesq approximation. Gravity is -9.81 in y direction.

I ran the simulation for around 500 iterations as steady state and then started transcient case.

Now, I monitored the residuals, at the start of simulation itself the energy dropped to about 10^-16 (and additionally I monitored temperature over an iso surface inside the domain - area weighted average - te,perature - static temperature - iso-surface). Here the temperature is shown 253 K (whereas it should be 316 K right?). When I checked the contours (over the same surface) after running the steady case it was shown 253 K. Is there any mistake in my modelling?

I couldnt run the case over the weekend so I did not model the transcient case. But today after a few iterations, still the temperature monitor I created shows only 253 K (of course it shouldnt change because it is the wall temperature and hence, the lowest)

With Regards
Vicky

[KevinZ09]

Two things:
- Firstly, after initialisation, but before clicking on calculate, check your volume average temperature (report --> volume integrals --> volume average and select temperatre --> static temperature). This should give 316K at the start. If it doesn't, you didn't initialise it correctly.
- Secondly, the results you're getting aren't necessarily wrong. If your temperatures at the start are 316K, then it just means your solution converged really quickly. Remember, you're starting with a certain temperature, but the walls all around are at 253K, so your fluid will eventually end up at that T too. Especially since you've got no wall with a higher T. It's like you put water in a freezer. It could be at 300K when you put it in there, but the final temperature will be the same as the freezer's temperature. You'll get different results when running the transient case, as the temperature will evolve over time. But what the Steady - State runs do, is iterate towards your FINAL solution. It could have intermediate results, depending on the complexity of your problem. But in your case, the final state is quite straight forward, hence probably the fast convergence.

So try the transient case and you should see different results.

[ViLaks]

Dear Kevin,

Thanks for your suggestions.

With Regards
Vicky

[ViLaks]

Dear All,

Sorry for restarting the thread, I am revisiting this problem now. I just need to know the total time my transcient simulation ran in Fluent. Following are the parametrs I gave as input:

Time Stepping Method: Fixed
Time Step Size (s) : 0.5
No: of Time Steps : 200
Max Itr/Time Step: 20

Is it right that my simulation has run for (200*0.5) 100 s ??

If yes, then my simulation is wrong. If the simulation is run for 100 s, I get the result. But it is wrong right. 43 to -18 deg celsius in just 1.5 mins?

Thanks and Regards
Vignesh

[flotus1]

0.5 s/timestep x 200 timesteps = 100s

You might want to start your own thread to describe what you are trying to do (pictures/sketches) and why you think your result is wrong.