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

Set temperature t=0

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 23, 2016, 18:14
Default Set temperature t=0
  #1
New Member
 
Damiano Bagnasco
Join Date: Jul 2016
Posts: 6
Rep Power: 9
Damiano93 is on a distinguished road
Good evening. I am studying the heat transfer between a solid zone and a fluid zone. How can I initialize the temperature of the solid zone?

Thank you for the support!
Damiano93 is offline   Reply With Quote

Old   October 24, 2016, 08:57
Default
  #2
Senior Member
 
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 22
vasava will become famous soon enough
You can patch temperature value to the domain. See this webpage. The page is for older version but the way it more or less same in newer versions also. You just select variable, zone, input a value and press 'patch'. You can verify by plotting contours for corresponding walls.
vasava is offline   Reply With Quote

Old   October 24, 2016, 18:19
Default
  #3
New Member
 
Damiano Bagnasco
Join Date: Jul 2016
Posts: 6
Rep Power: 9
Damiano93 is on a distinguished road
Mmmm no.. It doesn't start from that T. I must find another method. Thank you the same.
Damiano93 is offline   Reply With Quote

Old   October 25, 2016, 02:26
Default
  #4
Senior Member
 
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 22
vasava will become famous soon enough
Quote:
Originally Posted by Damiano93 View Post
It doesn't start from that T.
I didn't catch that. Could you elaborate what exactly you did?
vasava is offline   Reply With Quote

Old   October 25, 2016, 03:51
Default
  #5
New Member
 
Damiano Bagnasco
Join Date: Jul 2016
Posts: 6
Rep Power: 9
Damiano93 is on a distinguished road
I have a cylinder with an internal diameter with the fluid flow in a ceramic honeycomb (porous medium). The cylinder is a steel vessel, I set coupled as method of heat exchange betweeen the fluid (air) and the solid. I wrote an UDF for the Tinlet, in function of time. If I don't initialize the temperature of the ceramic and the steel it starts from the first value of the UDF. If i fix the temperature of steel and ceramic it is not correct because it means that this temperature will be constant for all the simulation. I don't really know how to solve it, because with patch the temperature deverges and the temperature at t=0 is taken from UDF (higher than the ambient that I'd like to initialize...). It is for my thesis... I don't like Fluent, it is ambiguos.
Damiano93 is offline   Reply With Quote

Old   October 25, 2016, 04:28
Default
  #6
Senior Member
 
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 22
vasava will become famous soon enough
Quote:
Originally Posted by Damiano93 View Post
If i fix the temperature of steel and ceramic it is not correct because it means that this temperature will be constant for all the simulation.
I hope you haven't misunderstood patching as fixed temperature. I mean it is not like if you patch 500 K to a domain it will remain 500 K throughout simulation. It will change as your simulation progresses.

It would be interesting to see your case. Can you upload it somewhere?
vasava is offline   Reply With Quote

Old   October 25, 2016, 05:00
Default
  #7
New Member
 
Damiano Bagnasco
Join Date: Jul 2016
Posts: 6
Rep Power: 9
Damiano93 is on a distinguished road
Nono, I understood the difference. And here is the problem. The size is too big. I don't want to waste your time, I ask you simply... I have two zones, fluid and solid. I don't fix the temperature. What should I do before, do "hybrid initialization" or write values for the patch? In order of time...
Damiano93 is offline   Reply With Quote

Old   October 25, 2016, 05:42
Default
  #8
Senior Member
 
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 22
vasava will become famous soon enough
I think you do both. Initialize first and then use patch.

Also, if you want the flow to develop first, you can solve only flow equations first. Once the flow is developed then you use patch and then solve flow and energy equations together.
vasava is offline   Reply With Quote

Old   October 25, 2016, 14:23
Default
  #9
Senior Member
 
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,654
Rep Power: 65
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Quote:
Originally Posted by Damiano93 View Post
I have a cylinder with an internal diameter with the fluid flow in a ceramic honeycomb (porous medium). The cylinder is a steel vessel, I set coupled as method of heat exchange betweeen the fluid (air) and the solid. I wrote an UDF for the Tinlet, in function of time. If I don't initialize the temperature of the ceramic and the steel it starts from the first value of the UDF. If i fix the temperature of steel and ceramic it is not correct because it means that this temperature will be constant for all the simulation. I don't really know how to solve it, because with patch the temperature deverges and the temperature at t=0 is taken from UDF (higher than the ambient that I'd like to initialize...). It is for my thesis... I don't like Fluent, it is ambiguos.
Are you using "compute from" and specifying the inlet? If you use compute from and specify any boundary, Fluent will use the temperature of the boundary as the initial condition. This isn't am ambiguity.

If you know what the initial values are then specify them explicitly using standard initialization.

Patching also works!

If you have divergence errors then it may be because your initial conditions are in an inconsistent state. For example you may think that an initial flow field will be a perfectly uniform temperature but because of the discretization cause by the mesh this is impossible. In this case it is helpful to freeze other variables (like flow) and run a few iterations to get over the numerical error hurdle.
LuckyTran is online now   Reply With Quote

Old   October 25, 2016, 16:09
Default
  #10
New Member
 
Damiano Bagnasco
Join Date: Jul 2016
Posts: 6
Rep Power: 9
Damiano93 is on a distinguished road
Ops.. I forgot compute from inlet!!! I don't know how to say THANK YOU!!!!!
Damiano93 is offline   Reply With Quote

Old   November 21, 2016, 04:54
Default
  #11
Senior Member
 
Onur Özcan
Join Date: Feb 2016
Location: Istanbul/Turkey
Posts: 461
Rep Power: 12
oozcan is on a distinguished road
[QUOTE=LuckyTran;622916]Are you using "compute from" and specifying the inlet? If you use compute from and specify any boundary, Fluent will use the temperature of the boundary as the initial condition. This isn't am ambiguity.

If you know what the initial values are then specify them explicitly using standard initialization.

Compute from is made ''standard initialization'' right?

it is like a transient boundary condition in a sense by making ''compute from'',hovewer, ''specify boundary in hand '' provides it ''constant'' value in all process.

are those right or not?
oozcan is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
How to set slip velocity and temperature jump awuunity CFX 10 July 2, 2018 09:40
How to set the temperature on the wall , which varies each coordinate in CFX? alexfirst CFX 6 August 3, 2016 10:15
How to set a constant temperature for entire volume Not only its surfaces fshak92 STAR-CCM+ 7 April 28, 2012 08:21
How to set Temperature as heat source in Solids shahpar73 CFX 2 August 20, 2009 19:51
how to set up high temperature gas turbine flow simulation? adam2008 CFX 1 July 22, 2009 19:33


All times are GMT -4. The time now is 09:55.