CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   How to set a constant temperature for entire volume Not only its surfaces (http://www.cfd-online.com/Forums/star-ccm/99924-how-set-constant-temperature-entire-volume-not-only-its-surfaces.html)

 fshak92 April 16, 2012 06:52

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

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?

 fshak92 April 17, 2012 11:12

1 Attachment(s)
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?

 siara817 April 18, 2012 05:46

You need to define the system as isothermal.

 fshak92 April 18, 2012 08:53

Quote:
 Originally Posted by siara817 (Post 355331) You need to define the system as isothermal.
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?

 siara817 April 18, 2012 12:50

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 April 18, 2012 13:14

Quote:
 Originally Posted by siara817 (Post 355442) 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)?

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 )

 LuckyTran April 25, 2012 14:29

Quote:
 Originally Posted by omid88 (Post 355447) 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!

 abdul099 April 28, 2012 07:21

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!

 All times are GMT -4. The time now is 17:23.