# Wall Transfer Coefficien - Heat Transfer Coefficient - CFX

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

 November 2, 2011, 18:49 Wall Transfer Coefficien - Heat Transfer Coefficient - CFX #1 New Member   Join Date: Oct 2011 Posts: 7 Rep Power: 13 Dear friends, I have simulated the flow in a simple geometry (like 2 paralel walls - "2,5D" case). My BC are (for laminar flow): In - low velocity and fixed temperature; Wall - no slip and fixed temperature; Out - Openning with static pressure. In CFX-Post: I have created a line in wall position, through the length. When I plot the variable (Wall Transfer Coefficien), the value found isn't the value hoped. 1) Why this happen? But when I take the Heat Flow "q" (in same line created) and temperature average of section "Tav" (with formulas in own CFX-Post)... I can obtain "h" correctly: q /(Tw-Tav) = h 2) Why "q" is correct, but "h" isn't? 3) How can I obtain "h" directly? 4) I have seen thread about that. Some users has talked about reference temperature.. But I don't understand that... Someone can explain it for me? and how can I change this reference temperature? I'm starting to study the CFD world... Thanks in advance everyone.

 November 2, 2011, 21:58 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,230 Rep Power: 135 I would start by working through this FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

 November 2, 2011, 23:25 #3 New Member   Join Date: Oct 2011 Posts: 7 Rep Power: 13 First of all, thanks for answer. I liked the link! There are a lot of good things over there! but... don't worry... I have done all steps, mainly for to learn how the software works. My results aren't inaccurate. I'm using: RMS = 10^-09 and highresolution for advection and couple velocity-pressure. The simulation doesn't need great adjustments.. So highresolution scheme is good. I have problem just with Heat Transfer Coefficient, even the "q" seem is right. The manual doesn't let clear about "h". There said some thing about: "... using an external heat transfer coefficient, hc...". As am I getting the value of "q" correct, while the value of "h" seem being wrong? How can I obtain the truly value of "h"? *I did the same simulation on FLUENT software and I obtained the "h" correct there! Last edited by Gargioni; November 2, 2011 at 23:34. Reason: I forgot some things =/

 November 2, 2011, 23:49 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,230 Rep Power: 135 There is more to accuracy than convergence tolerance and differencing scheme. h is referenced to a ambient temperature. By default CFX uses a function of the local fluid temperature which is usually quite different to the engineering definition (which is usually inlet temperature or far field temperature). To get h as engineers understand it have a look in the output file. There is a discussion in there about HTC reference temperatures and how to define your own temperature.

 November 3, 2011, 00:25 #5 New Member   Join Date: Oct 2011 Posts: 7 Rep Power: 13 "There is more to accuracy than convergence tolerance and differencing scheme." I said just for let clear that I don't have problems with accuracy. May you help me to find this thread about HTC? Thanks in advance =]

 November 3, 2011, 00:28 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,230 Rep Power: 135 It is in the output file. Have a look in your simulation. It is not a thread, but there are plenty of threads in the forum which have discussed the issue.

 November 4, 2011, 16:34 #7 New Member   Join Date: Oct 2011 Posts: 7 Rep Power: 13 I changed the expert parameter tbulk for htc. And I think CFX considers the tbulk value like constant How I said: I have simulated the flow in a simple geometry, like 2 paralel walls - "2,5D" case. I have created a line in wall position, through the length, for captures the "h", however the value of "tbulk" is variable along the length. What can I do when the tbulk value isn't constant?

 November 6, 2011, 05:57 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,230 Rep Power: 135 If you have set the tbulk parameter then tbulk will be constant and the value you define, otherwise it will depend on local flow conditions. You can easily extract h for a constant tbulk anyway. The local tbulk temperature used is an available variable, so between that and the wall heat transfer variable you can calculate h based on any tbulk you like.

 March 7, 2012, 01:19 #9 New Member   Join Date: Oct 2011 Posts: 7 Rep Power: 13 I solved my problem... doing a CEL routine. __________________ -- Gregory T. Gargioni ------><> E-mail: gargionis gmail "dot" com -------------------------------------

 April 15, 2013, 08:46 #10 Member   Join Date: Nov 2011 Location: Germany Posts: 40 Rep Power: 13 maybe u can give a short summary of the steps which u made to help me?

September 20, 2019, 07:23
#12
Senior Member

Przemek
Join Date: Jun 2011
Posts: 245
Rep Power: 14
Quote:

Hi

How did you implement this code into CFX?
__________________
best regards
pblasiak

 September 23, 2019, 17:09 #13 Senior Member   Przemek Join Date: Jun 2011 Posts: 245 Rep Power: 14 Ok I found that it is in Reference guide in Power Syntax chapter __________________ best regards pblasiak