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

heat resistance on solid-solid interface

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 12, 2009, 05:32
Default heat resistance on solid-solid interface
  #1
Bela
Guest
 
Posts: n/a
Dear CFX users!

My problem is the following: there are two solid bodies which are connected with solid-solid interface. There is heat generation (W/m3) in either of the solid domains. The thermal conductivity of the solids is different. I should define an additional heat transfer coefficient (4000 W/m2K) because the thermal contact is not perfect between them. I don't know how to define this htc on the domain interface. I found that I could set up source, where the Flux coefficient is the htc, but I don't know the value of the Flux. Does anybody could help me?

Bela
  Reply With Quote

Old   March 16, 2009, 14:31
Default
  #2
Member
 
Pratik Mehta
Join Date: Mar 2009
Posts: 32
Rep Power: 17
pratikmehta is on a distinguished road
Hi, could you please explain what do you mean by thermal contact is not proper . What exactly is your problem set-up .
pratikmehta is offline   Reply With Quote

Old   March 19, 2009, 03:55
Default
  #3
New Member
 
Join Date: Mar 2009
Posts: 5
Rep Power: 17
andy2o is on a distinguished road
Thermal contact resistances are not supported in ANSYS CFX 11. There may be some way of representing such resistances with user defined code or CEL though - it might be worth contacting ANSYS directly for advice.

I was told by ANSYS that they will be supported (together with other surface physics enhancements) in CFX 12, but I haven't seen the Beta release of CFX 12 to check whether they actually made it to the actual product...

Best regards,
andy2o
andy2o is offline   Reply With Quote

Old   March 19, 2009, 08:53
Default
  #4
Senior Member
 
Jack
Join Date: Mar 2009
Posts: 106
Rep Power: 16
rogbrito is an unknown quantity at this point
You can use Fluent for solving this problem.

Quote:
Originally Posted by Bela
;92318
Dear CFX users!

My problem is the following: there are two solid bodies which are connected with solid-solid interface. There is heat generation (W/m3) in either of the solid domains. The thermal conductivity of the solids is different. I should define an additional heat transfer coefficient (4000 W/m2K) because the thermal contact is not perfect between them. I don't know how to define this htc on the domain interface. I found that I could set up source, where the Flux coefficient is the htc, but I don't know the value of the Flux. Does anybody could help me?

Bela
rogbrito is offline   Reply With Quote

Old   March 19, 2009, 11:11
Default
  #5
Member
 
Pratik Mehta
Join Date: Mar 2009
Posts: 32
Rep Power: 17
pratikmehta is on a distinguished road
Hi,
Is your problem a natural convection or forced convection , all I can for now think of is that , you can have model the improper contact between the two solids as a porous media ( separate porous domain) , this porous domain should be having all the flow resistances in 3 directions.

I hope this helps

cheers
Pratik
pratikmehta is offline   Reply With Quote

Old   March 19, 2009, 17:43
Default
  #6
New Member
 
Join Date: Mar 2009
Posts: 5
Rep Power: 17
andy2o is on a distinguished road
Pratik,

When two bodies are held together, the (perhaps large, or perhaps microscopic) roughness of the surfaces of the bodies means that they do not come into uniform perfect contact. There will be small gaps between them (often filled with air). Therefore for heat to flow from one body to another it has to cross this small gap by conduction, small scale convection, or radiation. This gives rise to thermal resistance.

Because the gap is so small, you do not want to mesh it or model it as a 3-d feature. Instead, it is often modelled as a thermal resistance at a surface. Unfortunately CFX does not yet easily support this. This is what Bela was asking about.

I hope it makes sense now.

Best regards,
andy2o
andy2o is offline   Reply With Quote

Old   March 20, 2009, 02:28
Default
  #7
Member
 
Pratik Mehta
Join Date: Mar 2009
Posts: 32
Rep Power: 17
pratikmehta is on a distinguished road
Hi Andy ,

ok, now it is clear abt Bela`s query , you are right CFX till now have no such feature till now

thanks andy

best regards
pratik
pratikmehta is offline   Reply With Quote

Old   October 25, 2022, 15:57
Default
  #8
New Member
 
Ubade Kemerli
Join Date: Feb 2016
Posts: 2
Rep Power: 0
ubadekemerli is on a distinguished road
Hi Bela,

I use fluent, and I don't know if you can do it at CFX, but what I do in fluent is that I add a wall thickness and define a material for that wall thickness. By doing that, you can have the same thermal resistance by defining the thickness and thermal conductivity of the material properly. Hope that helps.
ubadekemerli is offline   Reply With Quote

Old   October 25, 2022, 16:02
Default
  #9
Senior Member
 
Join Date: Jun 2009
Posts: 1,804
Rep Power: 32
Opaque will become famous soon enough
- Open the solid-solid domain interface
- Go to the Additional Interface Models tab
- Select Heat Transfer/Interface Model option = Thin Material
- Select Material name
- Set material thickness.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque 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
Two-sided Wall Heat Transfer BC - No Separate Solid Mesh and No Heat Transfer Coeff swahono OpenFOAM Running, Solving & CFD 10 October 15, 2018 05:43
Constant velocity of the material Sas CFX 15 July 13, 2010 08:56
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 15:55
Conjugate Heat Transfer between fluid and solid Li Yang Main CFD Forum 8 March 27, 2004 11:05
Replace periodic by inlet-outlet pair lego CFX 3 November 5, 2002 20:09


All times are GMT -4. The time now is 07:22.