# how to give a temperature condition for a domain?

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

 June 13, 2012, 08:21 how to give a temperature condition for a domain? #1 New Member   Join Date: Jun 2012 Posts: 4 Rep Power: 7 Sponsored Links 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.

 June 13, 2012, 10:57 #2 Member   Robert Join Date: Mar 2011 Location: Warsaw Posts: 62 Rep Power: 8 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.

 June 30, 2012, 01:52 #3 New Member   vignesh kumar Join Date: Jun 2012 Posts: 1 Rep Power: 0 Which multi phase option will be better since same air will be for both the domain?

 July 2, 2012, 08:22 #4 New Member   Join Date: Jun 2012 Posts: 4 Rep Power: 7 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...??

July 2, 2012, 11:57
#5
Member

Join Date: Nov 2011
Posts: 83
Rep Power: 7
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 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...??

 July 3, 2012, 03:02 #6 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,504 Rep Power: 25 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.

July 5, 2012, 05:21
#7
New Member

Join Date: Jun 2012
Posts: 4
Rep Power: 7
Quote:
 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.

 July 5, 2012, 05:45 #8 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,504 Rep Power: 25 Would you like to show us the computational domain and the boundary conditions of your setup?

 July 31, 2012, 03:30 #9 New Member   Join Date: Jun 2012 Posts: 4 Rep Power: 7 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.

 March 4, 2016, 23:57 #10 Senior Member   Ali Join Date: Jan 2012 Location: Pakistan Posts: 135 Rep Power: 9 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

January 25, 2017, 05:51
#11
New Member

Vignesh Lakshmanan
Join Date: Nov 2016
Location: N/A
Posts: 17
Rep Power: 2
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 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

 January 25, 2017, 08:40 #12 Senior Member   Kevin Join Date: Dec 2016 Posts: 138 Rep Power: 2 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.

 January 26, 2017, 23:11 #13 New Member   Vignesh Lakshmanan Join Date: Nov 2016 Location: N/A Posts: 17 Rep Power: 2 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.

January 27, 2017, 05:39
#14
Senior Member

Kevin
Join Date: Dec 2016
Posts: 138
Rep Power: 2
Quote:
 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!

Quote:
 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.

Quote:
 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.

Quote:
 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!

Last edited by KevinZ09; January 27, 2017 at 06:11. Reason: Added patching.

 January 27, 2017, 06:35 #15 New Member   Vignesh Lakshmanan Join Date: Nov 2016 Location: N/A Posts: 17 Rep Power: 2 Dear Kevin, Thank you very much for your inputs. Regards Vicky

 January 30, 2017, 02:06 #16 New Member   Vignesh Lakshmanan Join Date: Nov 2016 Location: N/A Posts: 17 Rep Power: 2 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

 January 30, 2017, 04:16 #17 Senior Member   Kevin Join Date: Dec 2016 Posts: 138 Rep Power: 2 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.

 January 30, 2017, 23:10 #18 New Member   Vignesh Lakshmanan Join Date: Nov 2016 Location: N/A Posts: 17 Rep Power: 2 Dear Kevin, Thanks for your suggestions. With Regards Vicky

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post sima FLUENT 6 May 18, 2016 21:50 poplar OpenFOAM 3 January 14, 2015 03:37 Yr0gErG FLUENT 3 June 12, 2013 02:12 Kishorechand Main CFD Forum 0 April 4, 2012 05:01 suitup OpenFOAM Bugs 15 October 14, 2010 22:18