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

Thermal specification for CHT.

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

Like Tree4Likes
  • 4 Post By abdul099

Reply
 
LinkBack Thread Tools Display Modes
Old   July 9, 2009, 00:02
Default Thermal specification for CHT.
  #1
New Member
 
mehul
Join Date: May 2009
Location: Bangalore
Posts: 7
Rep Power: 8
mehn is on a distinguished road
Hi friends,
I have been doing Conjugate Heat transfer problem. Here One solid block is put inside one bigger block. The fluid flows from the bigger block. My understanding is that, by specifying boundary conditions on the surfaces of bigger block (from where fluid is flowing), I can get temeperatures on the solid wall. But, in STAR CCM+, by default the walls need thermal specification. I think that, this should be the output. I mean, I need to get temperatures on solid block walls, then why shoud I specify thermal specifications (Adiabatic, temperature, Heat flux etc etc). Please clarify this, if anyone knows. I have attached the image.
Attached Images
File Type: jpg image1.JPG (67.3 KB, 78 views)
mehn is offline   Reply With Quote

Old   July 9, 2009, 08:20
Default Thermal specification for CHT. Reply to Thread
  #2
New Member
 
Join Date: Mar 2009
Location: Belgium
Posts: 13
Rep Power: 8
rabat is on a distinguished road
Why you do not work with the heat source in the small block.

regards,

Rabat
rabat is offline   Reply With Quote

Old   July 14, 2009, 07:25
Default
  #3
New Member
 
Join Date: Jul 2009
Posts: 3
Rep Power: 8
Polly Eda is on a distinguished road
When you calculate CHT between the fluid and the solid, you have no wall (in the sense of a BC) between the solid and the fluid but an interface that does not need any thermal specification.

If you don't want to model the solid block and have walls instead then you have to give the code some more information (i.e. a thermal specification) to get a meaningful answer.

hope that helps,

Polly
Polly Eda is offline   Reply With Quote

Old   October 12, 2011, 12:23
Default
  #4
New Member
 
MadhuVC
Join Date: Feb 2011
Posts: 27
Rep Power: 6
madhuvc is on a distinguished road
I have the same problem.. I need to define a coupled boundary condition for the walls, but all I have is heat flux, convection ..

Is there an equivalent wall thermal specification in STAR_CCM+ which basically works as a coupled boundary as in FLUENT, while simulating conjugate heat transfer?

please help.
madhuvc is offline   Reply With Quote

Old   October 15, 2011, 10:15
Default First try to understand what CHT means before setting boundary conditions
  #5
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
Guys, it seems there's some clarification needed.

CHT = conjugate heat transfer. That means, you need to have two different bodies as CHT means, you model the heat transfer from one body to the other one. Let's say, one body is a hot solid (pot on a cooker), the other one a cold fluid (water inside the pot). And you want to model how the water heats up due to heat transfer from the pot.

You have to build your two bodies. Then you have to create an interface at EVERY boundary where you want heat to pass from one body to the other one. In this case, at all faces where the fluid touches the inner side of the pot. IT WILL NOT WORK WITHOUT INTERFACES!
When the simulation starts, the interfaces will be initialized and all faces in the wall boundary which is connected to the interface will be transfered to the interface. That means, the former wall boundary is empty, there are no faces inside, as all faces are moved to the interface which connects the two bodies. The thermal specification you tried to set can no longer work, since the boundary is empty. This is no issue, since the two adjacent cells on fluid and solid side are now connected and the usual energy conservation equation is solved: Heat flux out of the solid cell equals heat flux into the fluid cell.

The thermal specification works only for boundaries which are not an interface. For example there will be a heat flux the bottom side of a pot due to the cooker. You can put the temperature or heat flux specification at this boundary, so you don't have to model the whole cooker. But this has nothing to do with the boundary where the heat goes from the solid to the fluid, because the heat flux from fluid to solid is a result of your simulation, not a boundary condition (otherwise you wouldn't need a CHT case).

You can also model only a single body, let's say the water contained in the pot. When you know the temperature of all walls or the heat flux, you can put this values and don't have to model the solid. But this is NO CHT simulation, because there is no second body connected.
This works for simple cases when you've got all heat fluxes or temperatures at the boundaries - but for a complex case, it's nearly impossible to have all boundary conditions. That's the point when you start to model the solid as well as the fluid and get a CHT simulation.
abdul099 is offline   Reply With Quote

Old   February 8, 2012, 06:29
Default
  #6
ooo
Member
 
Join Date: Feb 2012
Posts: 49
Rep Power: 5
ooo is on a distinguished road
Thank you for your usefull information.
But How can we see the influence of the Air convection on our body if we cannot specify anything in our boundary conditions?
consider we have a block which has interface to Air.we should specify for thermal condition of the surface of the block to : convection(with an ambient temperature)
This surface has interface to Air..after runing how can the convection can be considered?
Thank you in advance.
Quote:
Originally Posted by abdul099 View Post
Guys, it seems there's some clarification needed.

CHT = conjugate heat transfer. That means, you need to have two different bodies as CHT means, you model the heat transfer from one body to the other one. Let's say, one body is a hot solid (pot on a cooker), the other one a cold fluid (water inside the pot). And you want to model how the water heats up due to heat transfer from the pot.

You have to build your two bodies. Then you have to create an interface at EVERY boundary where you want heat to pass from one body to the other one. In this case, at all faces where the fluid touches the inner side of the pot. IT WILL NOT WORK WITHOUT INTERFACES!
When the simulation starts, the interfaces will be initialized and all faces in the wall boundary which is connected to the interface will be transfered to the interface. That means, the former wall boundary is empty, there are no faces inside, as all faces are moved to the interface which connects the two bodies. The thermal specification you tried to set can no longer work, since the boundary is empty. This is no issue, since the two adjacent cells on fluid and solid side are now connected and the usual energy conservation equation is solved: Heat flux out of the solid cell equals heat flux into the fluid cell.

The thermal specification works only for boundaries which are not an interface. For example there will be a heat flux the bottom side of a pot due to the cooker. You can put the temperature or heat flux specification at this boundary, so you don't have to model the whole cooker. But this has nothing to do with the boundary where the heat goes from the solid to the fluid, because the heat flux from fluid to solid is a result of your simulation, not a boundary condition (otherwise you wouldn't need a CHT case).

You can also model only a single body, let's say the water contained in the pot. When you know the temperature of all walls or the heat flux, you can put this values and don't have to model the solid. But this is NO CHT simulation, because there is no second body connected.
This works for simple cases when you've got all heat fluxes or temperatures at the boundaries - but for a complex case, it's nearly impossible to have all boundary conditions. That's the point when you start to model the solid as well as the fluid and get a CHT simulation.
ooo is offline   Reply With Quote

Old   February 9, 2012, 15:04
Default
  #7
Member
 
Join Date: May 2010
Posts: 38
Rep Power: 7
Ladnam is on a distinguished road
The transport of heat from surface to air by convection and conduction is taken care of by the solver. But you need to specify a thermal resistance on the boundary, and radiation properties if you use radiation.
Ladnam is offline   Reply With Quote

Old   February 18, 2012, 07:47
Default
  #8
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
ooo, read my last post more carefully, it's all written there!
There are two options how to deal with your problem.

EITHER do a CHT simulation. You will model the fluid and the solid, connected with interfaces. The energy transfer from fluid to solid (or vice versa) through the interfaces will be calculated by the solver, and you will need NO boundary condition, except maybe an additional thermal resistance. The amount of heat transferred depends on the thermal boundary layer which is calculated with the flow field.
The MAYBE needed additional thermal resistance only needs to be specified when you want to model something like an additional insulation layer around your block without having to mesh and solve for that insulation layer.

OR you just simulate the solid, without fluid and therefore without any interfaces. Then you need to specify boundary conditions, most propably a convection condition. That's less computational effort, but also less accurate.
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
Simulation of a single bubble with a VOF-method Suzzn CFX 18 October 2, 2009 04:18
Specification of thermal conductivity in rhoSimpleFoam seb62 OpenFOAM Running, Solving & CFD 0 February 6, 2009 06:15
Anistropic thermal conduction in Fluent 6.2 Bharath FLUENT 0 November 23, 2006 22:07
Short Course: Computational Thermal Analysis Dean S. Schrage Main CFD Forum 11 September 27, 2000 17:46
Info: Short Course On Thermal Design of Electronic Equipment Arnold Free Main CFD Forum 0 August 10, 1999 10:18


All times are GMT -4. The time now is 02:56.