# Heat transfer coefficient - what is waht

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

 April 13, 2006, 18:45 Heat transfer coefficient - what is waht #1 Stan Guest   Posts: n/a Hello I am solving heat flow problem between two rotating cylindrical surfaces (part of my master thesis). The gap between them is more less 0.075 (depends on case) . As far as i know this heat flow can be modeled in analitic way by miechiejew equation (Nusslet number is function of Reynolds; Prandtl_fluid; Prandtl_wall). The Heat transfer coefficient obtained on paper is arouns 850 W/m^2/K. In Fluent i obtain Surface heat transfer coefficient around 68 W/m^2/K. But the Wall Func. Heat transfer coefficient is 1530 W/m^2/K. My sense tells me that is the result of different aproach of calculating heat transfer coefficient by Fluent. I tried to find anwser in help but i did'n manage to find it. Does anybody can redirect me to source where is the description how heat transfer coefficient is calculated and what is Wall Func. Heat transfer coefficient . Thank you in advice. PS: details about solver settings: Standart k-epsilon model with viscous heating with standard wall functions. Regards Stan

 April 14, 2006, 08:01 Re: Heat transfer coefficient - what is waht #2 Chandra Murthy Guest   Posts: n/a Fluent directly calculates heat flux on the boundaries. In Fluent, heat transfer coefficient (h) is a derived quantity using reference temperature, adjacent fluid temperature and heat flux. In the actual scenario, the reference temperature should be the wall temperature. Therefore, the values reported by fluent will be an indicative values. To get the actual h values you need to write a UDF according to your need.

 April 14, 2006, 10:37 Re: Heat transfer coefficient - what is waht #3 Stan Guest   Posts: n/a Thank you very much. Now i understand how h is calculated. According tp help this is the way of calculating it in laminar flow. For turbulent flow it uses wall functions which are beyond my borders of understanding, at this momemnt. I do not understand at all second part of your post. Anyway my question was touching the difference between two values available for postprocessing: Wall Fluxes\Surface heat transfer coefficient Wall Fluxes\Wall Func. heat transfer coefficient Additionaly I wolud like to know how they are calculated (my thesis supervisor wishes that because difference between analitical model and numerical are to big and he do not buys that this is caused by material data).

 November 23, 2009, 14:39 #4 New Member   Join Date: Oct 2009 Posts: 24 Rep Power: 8 Hi, I have identical problem. How to find actual h values by UDF? Best regards, doodek

 April 7, 2011, 10:47 #5 Member   Join Date: Mar 2011 Posts: 50 Rep Power: 7 The h values reported by the fluent are wrong. It has something to do with the reference temperature which can be different for different models. Ask fluent engineer. To get the right h value you need to write a udf. h = heat_flux / (T(z) - Tbulk(z)) Tbulk = SUM mu*cp*rho*Tf dA / SUM mu*cp*dA

 May 13, 2011, 16:46 #6 New Member   Zi Jian Join Date: Apr 2011 Posts: 4 Rep Power: 7 Hi, following the above discussion, therefore is Fluent overestimating the h value, or underestimating? Because I have h value (surface heat transfer coefficient) of about 400, and it is natural convection

 May 13, 2011, 23:34 #7 Member   Join Date: Mar 2011 Posts: 50 Rep Power: 7 Can you describe what you are modeling, such as geometry details? Also the 400 value, is that a constant h value across your fluid domain?

 May 14, 2011, 05:18 #8 New Member   Zi Jian Join Date: Apr 2011 Posts: 4 Rep Power: 7 It is a natural convection in an enclosure (with heating element at the center). The heating element is a square, with heat transfer coefficients at the top, left, and right surface are about 150-400 W/m^2.K. My question is...normally surface heat transfer coefficient in Fluent will be difference by how much from reality (as in using UDF)?

 May 19, 2011, 01:46 #9 Member   Join Date: Mar 2011 Posts: 50 Rep Power: 7 Your natural convection is very high. Such high convection is only found in micro and nano channels. As far as the difference between fluent h and real h is concerned, there is no specific number. If you raise or lower your reference temperature, the difference that you are asking will change. Thats why I suggest you make planes across your fluid domain and use the formula above to get Tbulk and then h = q/T(z) - Tbulk.

 May 19, 2011, 06:09 #10 New Member   Zi Jian Join Date: Apr 2011 Posts: 4 Rep Power: 7 Hi, I am new to UDF. So, in order to write these functions.. "h = heat_flux / (T(z) - Tbulk(z)) Tbulk = SUM mu*cp*rho*Tf dA / SUM mu*cp*dA" how to I define these variables "mu, cp, rho"? and is this equation applicable for 2D problem? Thank you.

 May 24, 2011, 23:00 #11 New Member   Oky Andytya Join Date: Nov 2010 Posts: 26 Rep Power: 7 Hi, everyone. I need help, How to get the value of convection coefficient [h] from Fluent directly ? Thank you,

 May 20, 2013, 19:57 I also need help for that. #12 Member   Elina Mathew Join Date: Mar 2013 Posts: 47 Rep Power: 5 Hi I am using a heat transfer problem where there is hot water flowing above a sphere...And have to find the heat transfer coefficient from fluent which has to be used for other calculations...kindly help me...

 May 21, 2013, 03:09 #13 New Member   Join Date: Oct 2009 Posts: 24 Rep Power: 8 Elina, You should modify 'reference temperature' under 'Reference values' tab in Fluent. As 'reference temperature' you can use other value, which is commonly used as a bulk temperature for your case. Fluent uses this temperature to calculate heat transfer coefficient based on heat flux through a cell boundary and temperature difference between wall temperature and the 'reference temperature'. Then, you can calculate area-weighted average of heat transfer coefficient on a sphere surface. Hope it will help. Regards, Marcin

 February 17, 2014, 15:25 Effect of velocity on h #14 New Member   Walder Ruis Join Date: Jan 2014 Location: Canada Posts: 23 Rep Power: 4 Hi everybody, I have a question: When simulating a simple forced convection in Fluent (heated wall, velocity inlet, pressure outlet). I want to know if the convection heat transfer I assign to the wall in the BC is automatically going to grow because of the velocity of the fluid or what I assign in the BC is already the forced convection heat transfer itself ? Thanks a lot in advance Loffy

 February 18, 2014, 06:31 #15 Senior Member     Flavio Join Date: Sep 2011 Location: Brescia, Italy Posts: 181 Rep Power: 7 Hello zomayabssa, Have you defined an Heat flux or an Heat Transfer Coefficient?. Regards __________________ Bionico

 February 24, 2014, 12:28 #16 New Member   Walder Ruis Join Date: Jan 2014 Location: Canada Posts: 23 Rep Power: 4 Hi Bionico, Thanks for your interest. Actually Yes I added a heat flux generation and fixed a convection coefficient of 20 w/m2K. What I wanted to know is if this coefficient is supposed to grow with the velocity inlet or it's gonna be fixed. I am not able to check that because I don't know what the "wall func. heat transfer coefficient" in fluent takes into consideration. Any idea? Thanks a lot

 February 25, 2014, 03:08 #17 Senior Member     Flavio Join Date: Sep 2011 Location: Brescia, Italy Posts: 181 Rep Power: 7 Good morning, Wall function heat transfer coefficient takes into account the temperature of the cell next to the wall (the first): this method works well only with certain values of Y* (Y_star) Regards rajann_786 likes this. __________________ Bionico

 February 27, 2014, 09:18 #18 New Member   Walder Ruis Join Date: Jan 2014 Location: Canada Posts: 23 Rep Power: 4 Thanks a lot Flavio. What about the velocity? do you think that Fluent increase the "h" value you define consedering the velocity imposed as a BC ? thanks a lot in advance

 February 27, 2014, 10:00 #19 Senior Member     Flavio Join Date: Sep 2011 Location: Brescia, Italy Posts: 181 Rep Power: 7 Well, it depends on the type of boundary condition: 1) if you fix the Heat Transfer Coefficient then it won't change during the simulation, because it's a boundary condition! 2) If you fix the Heat Flux, instead, "h" will change of course, but it depends on how you calculate it (with reference temperature or bulk temperature...). Regards __________________ Bionico

 March 11, 2014, 11:32 Bulk Temp #20 New Member   Amer Join Date: Mar 2014 Posts: 1 Rep Power: 0 Hi What do you mean the Bulk Temp.?? is it inlet fluid temp?? thanks

 Thread Tools 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 On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Attesz CFX 7 January 5, 2013 04:32 Sas CFX 15 July 13, 2010 08:56 enigma Main CFD Forum 2 November 1, 2009 23:53 Benny FLUENT 7 June 7, 2005 09:25 Mark CFX 6 November 15, 2004 16:55

All times are GMT -4. The time now is 05:41.