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

how to give a temperature condition for a domain?

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

Like Tree2Likes
  • 1 Post By flotus1
  • 1 Post By KevinZ09

Reply
 
LinkBack Thread Tools Display Modes
Old   June 13, 2012, 08:21
Default how to give a temperature condition for a domain?
  #1
New Member
 
Join Date: Jun 2012
Posts: 4
Rep Power: 6
arun_thakur is on a distinguished road
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.
arun_thakur is offline   Reply With Quote

Old   June 13, 2012, 10:57
Default
  #2
Member
 
Robert
Join Date: Mar 2011
Location: Warsaw
Posts: 62
Rep Power: 8
Kwiaci is on a distinguished road
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.
Kwiaci is offline   Reply With Quote

Old   June 30, 2012, 01:52
Default
  #3
New Member
 
vignesh kumar
Join Date: Jun 2012
Posts: 1
Rep Power: 0
vigneshkumar_t is on a distinguished road
Which multi phase option will be better since same air will be for both the domain?
vigneshkumar_t is offline   Reply With Quote

Old   July 2, 2012, 08:22
Default
  #4
New Member
 
Join Date: Jun 2012
Posts: 4
Rep Power: 6
arun_thakur is on a distinguished road
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...??
arun_thakur is offline   Reply With Quote

Old   July 2, 2012, 11:57
Default
  #5
Member
 
Join Date: Nov 2011
Posts: 83
Rep Power: 7
robboflea is on a distinguished road
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

Quote:
Originally Posted by arun_thakur View Post
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 is offline   Reply With Quote

Old   July 3, 2012, 03:02
Default
  #6
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,456
Rep Power: 24
flotus1 will become famous soon enoughflotus1 will become famous soon enough
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.
Mazze[ITA] likes this.
flotus1 is offline   Reply With Quote

Old   July 5, 2012, 05:21
Default
  #7
New Member
 
Join Date: Jun 2012
Posts: 4
Rep Power: 6
arun_thakur is on a distinguished road
Quote:
Originally Posted by robboflea View Post
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.
arun_thakur is offline   Reply With Quote

Old   July 5, 2012, 05:45
Default
  #8
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,456
Rep Power: 24
flotus1 will become famous soon enoughflotus1 will become famous soon enough
Would you like to show us the computational domain and the boundary conditions of your setup?
flotus1 is offline   Reply With Quote

Old   July 31, 2012, 03:30
Default
  #9
New Member
 
Join Date: Jun 2012
Posts: 4
Rep Power: 6
arun_thakur is on a distinguished road
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.
arun_thakur is offline   Reply With Quote

Old   March 4, 2016, 23:57
Default
  #10
Senior Member
 
Ali
Join Date: Jan 2012
Location: Pakistan
Posts: 135
Rep Power: 9
Hybrid is on a distinguished road
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
__________________
Best Regards
Ali


Hybrid is offline   Reply With Quote

Old   January 25, 2017, 05:51
Default
  #11
New Member
 
Vignesh Lakshmanan
Join Date: Nov 2016
Location: N/A
Posts: 17
Rep Power: 2
ViLaks is on a distinguished road
Sorry for restarting the thread again, but as I am new to fluent, how can I initialise the desired temperature?
Quote:
Originally Posted by flotus1 View Post
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
ViLaks is offline   Reply With Quote

Old   January 25, 2017, 08:40
Default
  #12
Senior Member
 
Kevin
Join Date: Dec 2016
Posts: 138
Rep Power: 2
KevinZ09 is on a distinguished road
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.
KevinZ09 is offline   Reply With Quote

Old   January 26, 2017, 23:11
Default
  #13
New Member
 
Vignesh Lakshmanan
Join Date: Nov 2016
Location: N/A
Posts: 17
Rep Power: 2
ViLaks is on a distinguished road
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

Last edited by ViLaks; January 27, 2017 at 01:09.
ViLaks is offline   Reply With Quote

Old   January 27, 2017, 05:39
Default
  #14
Senior Member
 
Kevin
Join Date: Dec 2016
Posts: 138
Rep Power: 2
KevinZ09 is on a distinguished road
Quote:
Originally Posted by ViLaks View Post
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!

Quote:
Originally Posted by ViLaks View Post
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.

Quote:
Originally Posted by ViLaks View Post
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.

Quote:
Originally Posted by ViLaks View Post
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!
pakk likes this.

Last edited by KevinZ09; January 27, 2017 at 06:11. Reason: Added patching.
KevinZ09 is offline   Reply With Quote

Old   January 27, 2017, 06:35
Default
  #15
New Member
 
Vignesh Lakshmanan
Join Date: Nov 2016
Location: N/A
Posts: 17
Rep Power: 2
ViLaks is on a distinguished road
Dear Kevin,

Thank you very much for your inputs.

Regards
Vicky
ViLaks is offline   Reply With Quote

Old   January 30, 2017, 02:06
Default
  #16
New Member
 
Vignesh Lakshmanan
Join Date: Nov 2016
Location: N/A
Posts: 17
Rep Power: 2
ViLaks is on a distinguished road
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
ViLaks is offline   Reply With Quote

Old   January 30, 2017, 04:16
Default
  #17
Senior Member
 
Kevin
Join Date: Dec 2016
Posts: 138
Rep Power: 2
KevinZ09 is on a distinguished road
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.
KevinZ09 is offline   Reply With Quote

Old   January 30, 2017, 23:10
Default
  #18
New Member
 
Vignesh Lakshmanan
Join Date: Nov 2016
Location: N/A
Posts: 17
Rep Power: 2
ViLaks is on a distinguished road
Dear Kevin,

Thanks for your suggestions.

With Regards
Vicky
ViLaks is offline   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
How can I implement temperature jump boundary condition in microchannel walls? sima FLUENT 6 May 18, 2016 21:50
Can anyone give me some hint on how to make traction free boundary condition? poplar OpenFOAM 3 January 14, 2015 03:37
Natural convection in a closed domain STILL NEEDING help! Yr0gErG FLUENT 3 June 12, 2013 02:12
How to give velocity and temperature gradient's type of boundary conditions in fluent Kishorechand Main CFD Forum 0 April 4, 2012 05:01
(Heattransfer) Temperature boundary condition problem suitup OpenFOAM Bugs 15 October 14, 2010 22:18


All times are GMT -4. The time now is 23:31.