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

How to set a constant temperature for entire volume Not only its surfaces

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

Like Tree5Likes
  • 1 Post By siara817
  • 1 Post By fshak92
  • 1 Post By siara817
  • 1 Post By LuckyTran
  • 1 Post By abdul099

Reply
 
LinkBack Thread Tools Display Modes
Old   April 16, 2012, 06:52
Default How to set a constant temperature for entire volume Not only its surfaces
  #1
Senior Member
 
Join Date: Dec 2011
Posts: 121
Rep Power: 5
fshak92 is on a distinguished road
I want to have a flow(with a constant temperature) over a surface for simulating a convection simulation.
I don't want to use the Convection boundary condition because i have to set constant temperature to my surface as well.
Also if i create a block around my surface as Air,I just can set the constant temperature of the air for its outer surfaces and not for the air over the surface or entire volume.

Do you have any idea or suggestion regarding this?

Thank you in advance.

Last edited by fshak92; April 16, 2012 at 08:25.
fshak92 is offline   Reply With Quote

Old   April 17, 2012, 11:12
Default
  #2
Senior Member
 
Join Date: Dec 2011
Posts: 121
Rep Power: 5
fshak92 is on a distinguished road
I used the 'velocity inlet' with low velocity (like 0.01m/s) to have a constant temperature for entire volume but the results are influenced by the direction of the velocity and it cannot simulate a real room with no velocity.
Do you have any idea for simulating the situation of a room with no velocity?

Many thanks in advance
Attached Images
File Type: jpg LowVelocity.jpg (91.9 KB, 32 views)

Last edited by fshak92; April 17, 2012 at 12:41.
fshak92 is offline   Reply With Quote

Old   April 18, 2012, 05:46
Default
  #3
Senior Member
 
siara817's Avatar
 
siamak rahimi ardkapan
Join Date: Jul 2010
Location: Copenhagen, Denmark
Posts: 218
Rep Power: 9
siara817 is on a distinguished road
You need to define the system as isothermal.
fshak92 likes this.
siara817 is offline   Reply With Quote

Old   April 18, 2012, 08:53
Default
  #4
Senior Member
 
Join Date: Dec 2011
Posts: 121
Rep Power: 5
fshak92 is on a distinguished road
Quote:
Originally Posted by siara817 View Post
You need to define the system as isothermal.
Thank you for your reply.
But if i consider 'isothermal' then no energy equation is solved.
I have a heated body(as can be seen in the above picture) in the room(block) and i want to find the Heat Transfer Coefficient.
The surface of the body has the constant temperature but the air around the body can be warmed.
I need to simulate a real room around my body(with constant temperature) to find the heat transfer and consequently HTC.
I can set some constant temperature to block's wall but then some unwanted parameters like the dimensions influence on the gradiant of temperature and....

Do you have any idea?
Many thanks in advance.
siara817 likes this.
fshak92 is offline   Reply With Quote

Old   April 18, 2012, 12:50
Default
  #5
Senior Member
 
siara817's Avatar
 
siamak rahimi ardkapan
Join Date: Jul 2010
Location: Copenhagen, Denmark
Posts: 218
Rep Power: 9
siara817 is on a distinguished road
Dear Omid, I think it is wise to extend the territory. and see what will happen.
I think the reversed flow problem will be solved. Is it possible to change the boundary ( the boundaries parallel to the flow)?
fshak92 likes this.
siara817 is offline   Reply With Quote

Old   April 18, 2012, 13:14
Default
  #6
Senior Member
 
Join Date: Dec 2011
Posts: 121
Rep Power: 5
fshak92 is on a distinguished road
Quote:
Originally Posted by siara817 View Post
Dear Omid, I think it is wise to extend the territory. and see what will happen.
I think the reversed flow problem will be solved. Is it possible to change the boundary ( the boundaries parallel to the flow)?
Thank you for your reply and the time you took for answering.

I have just a body with a constant temperature in a room with a certain temperature and i want to find the heat transfer between air and my body.
yes i just want to have a simple room.(the picture above)
But the problem is that there isn't any velocity in my simple room.
I dont know how i can consider the natural convection...
(as i told above,setting some constant temperature to the walls,include some unwanted parameters(like the dimension of the block) in my simulation )

Thanks again for your answers.
fshak92 is offline   Reply With Quote

Old   April 25, 2012, 14:29
Default
  #7
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 686
Rep Power: 13
LuckyTran will become famous soon enough
Quote:
Originally Posted by omid88 View Post
Thank you for your reply and the time you took for answering.

I have just a body with a constant temperature in a room with a certain temperature and i want to find the heat transfer between air and my body.
yes i just want to have a simple room.(the picture above)
But the problem is that there isn't any velocity in my simple room.
I dont know how i can consider the natural convection...
(as i told above,setting some constant temperature to the walls,include some unwanted parameters(like the dimension of the block) in my simulation )

Thanks again for your answers.
omid. Just setup the model as a car inside a room. i.e. all 6 bounding surfaces are walls with specified temperature. This way there are no inlets or outlets and there is no forced velocity. Apply your surface temperature to the car.

I recommend using the segregated energy solver. If you are using the segregated solver, you can use either the temperature, isothermal, or enthalpy based formulation. But temperature is recommended. For coupled solver there is no separate treatment so no options. You will not be able to use constant density formulation. You will need to use Ideal Gas model or better (so that density can vary).

Make sure you include gravity or body forces in the simulation and then start running!

That's it!
fshak92 likes this.
LuckyTran is offline   Reply With Quote

Old   April 28, 2012, 07:21
Default
  #8
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
As soon as there is a heat transfer, you will NEVER have the same temperature all over the domain. So decide what you want! Either a constant temperature, or a solved energy equation. But you can NEVER have both of it!
You can put the walls of your room to a fixed temperature to model the big thermal mass of the walls, that would be realistic. But around a heated body, you will always have at least a thin layer with a higher temperature. That's what happens in the real world as well!
fshak92 likes this.
abdul099 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
No layers in a small gap bobburnquist OpenFOAM Native Meshers: snappyHexMesh and Others 6 August 26, 2015 09:38
Assigning constant temperature to an interface boundary in a conjugate HT. fshak92 STAR-CCM+ 3 February 16, 2012 08:36
set wall temperature Reunion STAR-CCM+ 7 January 29, 2012 07:25
mesh airfoil NACA0012 anand_30 OpenFOAM Meshing & Mesh Conversion 12 December 12, 2011 05:16
Two-Phase Buoyant Flow Issue Miguel Baritto CFX 4 August 31, 2006 12:02


All times are GMT -4. The time now is 17:43.