# Heat Transfer Coefficient of water

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Search this Thread Display Modes
 October 11, 2013, 13:24 Heat Transfer Coefficient of water #1 New Member   Join Date: Oct 2013 Posts: 13 Rep Power: 11 Hi everyone I am doing a conjugate heat transfer (CHT) analysis where I have a solid body being cooled by a jacket which has water passing through it. The inlet velocity of the water is 0.832 m/sec and the inlet temperature is 17 deg C. There is a certain heat load of 1.7 kW on the surface of the solid body. After solving, CFX tells me that the heat transfer coefficient of water on the fluid-solid interface side 2 (Fluid domain) is around 12000 W/m^2K. Is this value realistic for water? Shreesha

 October 11, 2013, 17:16 #2 Senior Member   Erik Join Date: Feb 2011 Location: Earth (Land portion) Posts: 1,114 Rep Power: 21 That heat transfer coefficient is using the adjacent wall temperature for the fluid temperature, not you standard engineering "bulk" temperature, so the values are not comparable, and will also depend on your mesh size since that influences the "adjacent wall" temperature. CFX htc = HeatFlux / (Twall - Tadjacent) Standard htc = HeatFlux / (Twall - Tbulk) There are options to change this, or easier, just write your own expression to find the htc.

 October 11, 2013, 23:07 #3 New Member   Join Date: Oct 2013 Posts: 13 Rep Power: 11 Hi Evcelica Thanks a lot for the reply. Actually, I tried to get the htc based on the bulk temperature via the expert parameter in CFX. But, in that case, the heat transfer coefficient ranged from -15000 to 30000 W/m^2 K. I am not sure why it calculated negative values since it doesn't make sense right? Thanks Shreesha

 October 12, 2013, 07:42 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,229 Rep Power: 135 I would have a look at your HTC (using a sensible reference temperature) to see if it is realistic. I would then do a sensitivity analysis to see if it is accurate. I suspect the results you have so far are not accurate.

 October 12, 2013, 18:58 #5 New Member   Join Date: Oct 2013 Posts: 13 Rep Power: 11 Hi ghorrocks Thanks a lot for the reply. I took 300 K (27 deg C) as the reference bulk temperature for the htc calculation. This is sensible right? Also, is this due to the mesh in the boundary layer? Do you suspect that the boundary layer is not accurately modeled? Thanks Shreesha

 October 13, 2013, 02:20 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,229 Rep Power: 135 You should define whatever reference temperature makes sense in your simulation -probably the inlet temperature, the initial temperature or something like that. Inadequate mesh resolution is the most common form of simulation inaccuracy. And it can affect the results anywhere in the simulation, not just the boundary layer.

December 3, 2013, 20:45
#7
New Member

Nicholas Lee
Join Date: Oct 2010
Posts: 18
Rep Power: 14
Quote:
 Originally Posted by shreesha87 Hi everyone I am doing a conjugate heat transfer (CHT) analysis where I have a solid body being cooled by a jacket which has water passing through it. The inlet velocity of the water is 0.832 m/sec and the inlet temperature is 17 deg C. There is a certain heat load of 1.7 kW on the surface of the solid body. After solving, CFX tells me that the heat transfer coefficient of water on the fluid-solid interface side 2 (Fluid domain) is around 12000 W/m^2K. Is this value realistic for water? Shreesha
dear shreesha, sorry to trouble you. at present i am doing the conjugate heat transfer simulation using CFX like you.
In my model, the temperatuire for air should be up and the temp. for cooling water should be down. Detailed desciption can be found in my thread that i have posted a thread in the forum, http://www.cfd-online.com/Forums/cfx...-problems.html
could you tell me how you defined heat transfer between solid and fluid in you CFX analysis? just to apply Domain Interface and Conservative Interface FLUX is enough? do i have to do it with Interface model Thermal Contact Resistance or Thin Material?

your reply will be appreciated.

 December 3, 2013, 21:04 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,229 Rep Power: 135 You will get heat flow between the solid and fluid domains when you use the default Conservative Interface flux model on the interface. The Thermal contact resistance model will add thermal contact resistance to the interface if that is relevant. A thin material will disconnect the two domains and not allow heat transfer.

December 3, 2013, 22:27
#9
New Member

Nicholas Lee
Join Date: Oct 2010
Posts: 18
Rep Power: 14
Quote:
 Originally Posted by ghorrocks You will get heat flow between the solid and fluid domains when you use the default Conservative Interface flux model on the interface. The Thermal contact resistance model will add thermal contact resistance to the interface if that is relevant. A thin material will disconnect the two domains and not allow heat transfer.
dear ghorrocks, following you instructions, i have just applied Conservative Interface Flux in CFX but without interface model, and eventually it worked that the outlet air temperature is coming down and that for water is up.
but i have another question for you. when i changed the mass flow rate for water inlet (from 0.15kg/s to 0.3kg/s) toghet with other settings kept unchanged, the simulation result was hardly affected. i can see the outlet air temperature and outlet water temperature remained the same.
I am confused, could you give me some explaination or help me how to handle it? thank you !

 December 3, 2013, 22:43 #10 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,229 Rep Power: 135 You often have to use a solid time scale factor in steady state simulations to accelerate convergence in solid regions. If you are not using this parameter convergence can take forever and it can seem like nothing is happening after you make the the change. But if you look at the post processing you should see that the change has started and is flowing through the domain. It just has not reached the exit yet and certainly has not achieved steady state.

December 3, 2013, 23:15
#11
New Member

Nicholas Lee
Join Date: Oct 2010
Posts: 18
Rep Power: 14
Quote:
 Originally Posted by ghorrocks You often have to use a solid time scale factor in steady state simulations to accelerate convergence in solid regions. If you are not using this parameter convergence can take forever and it can seem like nothing is happening after you make the the change. But if you look at the post processing you should see that the change has started and is flowing through the domain. It just has not reached the exit yet and certainly has not achieved steady state.
dear ghorrocks, in the CHT simulation done in CFX, Solid Timescale Factor was applied that was set to 60, and it converged normally when it RMS residuals became less than 1e-4.

so where do i have to reset or to pay special attention and restart the simulation?

December 3, 2013, 23:34
#12
New Member

Nicholas Lee
Join Date: Oct 2010
Posts: 18
Rep Power: 14
Quote:
 Originally Posted by dingsheng1206 dear ghorrocks, in the CHT simulation done in CFX, Solid Timescale Factor was applied that was set to 60, and it converged normally when it RMS residuals became less than 1e-4. so where do i have to reset or to pay special attention and restart the simulation?

Attached are the basic structure, related settings and RMS converging history, hope it can make you understand better that you can help me, thank you!
Attached Images
 Solid Timescale Factor.jpg (96.4 KB, 19 views) Momen Mass RMS.jpg (63.7 KB, 15 views) Outlet Air Temp..jpg (62.3 KB, 10 views) Turbulence RMS.jpg (61.1 KB, 10 views) HT RMS.jpg (69.1 KB, 11 views)

 December 4, 2013, 00:27 #13 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,229 Rep Power: 135 Did you include imbalances as part of your convergence criterion? This is very important for CHT simulations - residuals are not a reliable guide of convergence for many CHT simulations.

December 4, 2013, 01:12
#14
New Member

Nicholas Lee
Join Date: Oct 2010
Posts: 18
Rep Power: 14
Quote:
 Originally Posted by ghorrocks Did you include imbalances as part of your convergence criterion? This is very important for CHT simulations - residuals are not a reliable guide of convergence for many CHT simulations.
dear ghorrocks

sorry i do not know where to set imbalances convergence criterion? it is set in Solver Control/ Equation Class/ Energy ?

thank you!

December 4, 2013, 02:16
#15
New Member

Nicholas Lee
Join Date: Oct 2010
Posts: 18
Rep Power: 14
Quote:
 Originally Posted by ghorrocks Did you include imbalances as part of your convergence criterion? This is very important for CHT simulations - residuals are not a reliable guide of convergence for many CHT simulations.
dear ghorrocks.
i can set imbalance as convergence criterion, but i got the imbalance of domain in the monitor.

attached are the imbalance of domain, if there is error with imbalance of domain, how to handle it? many thanks!
Attached Images
 imbalance.jpg (86.0 KB, 14 views)

 December 4, 2013, 07:25 #16 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,229 Rep Power: 135 Imbalances are just another measure of convergence. If they are not tight enough then you converge tighter. And you should do a sensitivity study to determine how tight you require.

 Tags heat transfer coefficient

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 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 OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Karkoura CFX 0 March 10, 2011 16:35 andred FLUENT 0 November 16, 2010 22:13 Sas CFX 15 July 13, 2010 09:56 los OpenFOAM Running, Solving & CFD 5 January 31, 2010 18:44 doodek Main CFD Forum 2 November 23, 2009 09:48

All times are GMT -4. The time now is 08:37.

 Contact Us - CFD Online - Privacy Statement - Top