# Heat Transfer Coefficient

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

 March 10, 2000, 09:10 Heat Transfer Coefficient #1 Alberto Schroth Guest   Posts: n/a Can anyone tell me how Fluent calculates the heat transfer coefficient along a surface? In the manual, it shows a definition of heat transfer (h eff) coefficient based on user defined temperature reference and a calculated heat flux. Is this the actual equation used by Fluent to calculate heat transfer coefficient. Tell me its not true... Alberto Schroth laxwendrofzx9r likes this.

 March 10, 2000, 09:53 Re: Heat Transfer Coefficient #2 Jonas Larsson Guest   Posts: n/a This is a big problem in Fluent - if you have a well defined bulk temperature all is well, but if you have a more complex flow, with combustion and a strongly varying bulk-temperature then things aren't that easy. We have discussed a lot with Fluent to get them to implement some kind of function to extract more realistic bulk-temperatures. I'm not sure if we have managed to convince them though. Our suggestion was that they should implement a function to pick the bulk-temperature at a certain y+ away from walls. That would be much better than using a global bulk temeperature that has little to do with the local condition in that region (using a global bulk temperature can even gives you negative heat-transfer coefficients sometimes - not exactly realistic!). In order to do thermal analysis in, for example, Ansys you need a fairly realistic bulk temperature and heat-transfer coefficient and today that is very difficult to extract from Fluent if you have a complex case with combustion.

 March 10, 2000, 12:49 Re: Heat Transfer Coefficient #3 Sung-Eun Kim Guest   Posts: n/a Jonas, The "bulk temperature" can be unequivocally defined in the case of simple flows where you have a dominant flow direction (e.g. duct flows). However, I and we developers have really hard time to understand what you mean by bulk temperature in massively complex flows involving recirculations, separation, impingement, etc. How can y+ be any indicator for an appropriate location representing "bulk" temperature ? As you know, for complex flows, y+ which is defined in terms of turbulent kinetic energy, is not a monotonically increasing function of the distance from the wall. We believe that all this is a matter of selecting a "reference" temperature and I still believe that the temperature at wall-adjacent cells can be a good reference temperature.

 March 10, 2000, 13:07 Re: Heat Transfer Coefficient #4 Fred Uckfield Guest   Posts: n/a .......the temperature at wall-adjacent cells can be a good reference temperature. But surely a function of near wall cell size? Fred.

 March 10, 2000, 13:24 Re: Heat Transfer Coefficient #5 Alberto Schroth Guest   Posts: n/a In my problem, my geometry is a closed tube with an inlet boundary condition described by an UDF which varies the velocity as a function time (sin[wt]). All the walls are adiabatic except for the end of the tube which is maintained at constant temperature equal to the inlet temperature of the fluid. I would expect the temperature to vary at the surface of the end of tube thus allowing for the calculation of heat transfer coefficient. I still haven't hear how Fluent magically calculates the heat transfer coeffient. Also, what is the relationship of heat transfer to nusselt number? Alberto

 March 10, 2000, 15:29 Re: Heat Transfer Coefficient #6 Sung-Eun Kim Guest   Posts: n/a FLLUENT doesn't do any magic in computing heat transfer coefficient. FLUENT just computes, in a simple-minded way, heat transfer coefficient from h = q"/(T_ref-T_w), where q" is the heat flux at wall, T_ref is a reference temperature, and T_w is the wall temperature. You can use, as T_ref, a meaningful reference temperature, if any(e.g., mixing cup temperature in pipe flows, freestream temperature in boundary layer flows). But we should keep in mind that h is a "derived" quantity who value totally depends on how we define it. In your case, the heat trnasfer is zero on the adiabatic wall because there's no heat flux through it. And, on the end-wall where you specified a constant temperature, FLUENT should give you a spatially varying heat transfer coefficient, because the heat flux doesn't vanish and will be a function of the flow and turbulence field near the end wall.

 March 13, 2000, 03:55 Re: Heat Transfer Coefficient #7 Jonas Larsson Guest   Posts: n/a Hmm, I'm quite sure that Y+ is monotonically increasing with wall distance, at least as long as we are only talking about one wall which isn't "too curved". You probably mean Y*, which is dependent on the turbulent energy and thus can have local minima/maxima further out. In fully developed equilibrium turbulent boundary layers Y+ and Y* are the same, but they are defined differently. Anway, this doesn't affect the main problem - How to extract a realistic bulk-temperature. Of course, in a complex flow, there is no correct way of doing this - you simply can't define a bulk-temperature which will be fully represantative all the time. However, fact remains, in order to do thermal analysis in, f or example, Ansys, you need a bulk-tempereture and a heat-transfer coeffiecient which is fairly realistic. Choosing the first cell next to the wall as bulk temperature will only work if you are using wall-functions and have a good grid with fairly constant y+ for your first cell-layer. It will also make your extracted heat-transfer coeffiecients very grid dependent. I think that a better way would be to use a temperature at a y+ further out. If you use the first cell you will get the temperature at, say y+=50, which is where your first cell should be if you use wall-functions. This is too close to the wall I think. Don't you agree? Using the temperature at a y+ location further out would be one way to find a more realistic "local bulk temperature", representing the temperature outside the boundary layers. Has anyone else got any good tricks on how to export realistic bulk-temperatures and heat-transfer coefficients from Fluent in a complex flow with combustion (highly varying "bulk" temperature)?

 March 13, 2000, 07:23 Re: Heat Transfer Coefficient #8 Volker Pawlik Guest   Posts: n/a Hi Jonas, I had a similar problem in the past where I had to export heat-transfer coefficients for thermal analysis of a heat exchanger with the CSM(computational structural mechanics)-code NASTRAN. At first the problem of the exchanger was decoupled into two fluid zones and one solid zone due to the restriction of RAM. The simultion started with the calculation of the flow and temp. field of the fluid zones (Walls with const. Temp.). The results in form of heat-transfer coefficients and a reference temperature were exported to Nastran in order to calculated new wall tempeartures for the solid. With a test model (adiabatic boundaries for the walls facing enviromnment) the temperature field looked converged after three "iterations" between the fluid and solid solving process. The real life problem included ambient heat loss. Hence the difficulty was not to calculate realistic coefficients acoording to the typical range for the fluid I was considering, but to avoid negative values. The absolute value of the heat-transfer coefficient is not of interest for the CSM-code (Nastran) because it is always related to the / a reference temperature. Both together (temp. and coeff.) will lead to a new correct wall temperature. But the negative values are not defined and it was /is not possible to define a reference temperature in that way that negative values are avoided for zones which gain energy and lose energy at the same time. For that reason it would be really a goal if there would be an implementation in FLUENT for the post-processing of local heat-transfer coefficients depending on the wall closest cell. Maybe it is already possible by defining a custom field function which uses the static temperature of the the wall (which should be the the center value of the wall closest cell???) instead of a reference temperature. Problems may occur for tetrahedral grids. Maybe that is a reason why it is not implemented yet.

 March 13, 2000, 11:11 Re: Heat Transfer Coefficient #9 Alberto Schroth Guest   Posts: n/a Sung: Thank you for responding to me regarding the calculation of heat transfer coefficient (effective). However, the heat flux that you mentioned, must be calculated using a heat transfer coeffient. If not, can you describe to me exactly how Fluent calculates the heat flux on a surface. The reference manual does not indicate an equation, but only a definition. Regards, Alberto Schroth

 March 13, 2000, 12:22 Re: Heat Transfer Coefficient #10 Sung-Eun Kim Guest   Posts: n/a As a thermal boundary condition, you specify either wall temperature or heat flux. For tubulent heat transfer, there are three scenarios thta can happen. They are; 1) When you specify heat flux, q", FLUENT uses the heat flux directly to solve the enery equation, and compte the wall temperature, T_wall, using the temperature law of the wall. For post-processing, FLUENT uses q" and T_wall to compute the heat transfer coefficient, h, from; h = q"/(T_ref - T_wall) where T_ref is a reference temperature you specified 2)When you specify a wall temperature, T_wall, FLUENT uses the temperature law of the wall to compute q". q" thus computed gets used in the energy equation. For postprocessing, FLUENT uses q" and T_wall to compute the heat transfer coefficient, h, from the same definition as above. The temperature wall function FLUENT uses can be found in the User's Guide (Eq. 9.7-5 in Volume 2) Ice man likes this.

 March 13, 2000, 13:10 Re: Heat Transfer Coefficient #11 John C. Chien Guest   Posts: n/a (1). I think, this is good enough for the calculation of the h, which is a derived quantity. (2). For this reason, it is probably easier for the users to look at the h definition in terms of the delta_T_at_wall. In this way, delta_T_at_wall=(T_ref - T_wall). (3). The T_wall is needed, because it is a local temperature. And also h is the local heat transfer coefficient. (4). The selection of the T_ref is not arbitrary, becuase one is going to use the formula in a consistent way to provide the heat transfer information. (5). So, if the temperature in the boundary layer is monotomic, then the temperature at the edge of the boundary layer can be used to give consistent information on the heat transfer. Otherwise, some other reference temperature can be used. (6). Obviously, if the user select the T_ref very close to the T_wall, he will run into trouble in certain part of the wall where T_wall=T_ref. (7). So, a non-zero delta_T_at_wall is required for the heat transfer coefficient concept to work. And the selection of the T_ref is important, so that the derived formula for h is useful later on in the global heat transfer applications. In other words, do not try to define the T_ref such that delta_T_at_wall becomes zero. ayad and rajann_786 like this.

August 21, 2013, 04:28
#12
Super Moderator

Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Posts: 3,994
Blog Entries: 6
Rep Power: 39
Quote:
 Originally Posted by Jonas Larsson ;93935 This is a big problem in Fluent - if you have a well defined bulk temperature all is well, but if you have a more complex flow, with combustion and a strongly varying bulk-temperature then things aren't that easy. We have discussed a lot with Fluent to get them to implement some kind of function to extract more realistic bulk-temperatures. I'm not sure if we have managed to convince them though. Our suggestion was that they should implement a function to pick the bulk-temperature at a certain y+ away from walls. That would be much better than using a global bulk temeperature that has little to do with the local condition in that region (using a global bulk temperature can even gives you negative heat-transfer coefficients sometimes - not exactly realistic!). In order to do thermal analysis in, for example, Ansys you need a fairly realistic bulk temperature and heat-transfer coefficient and today that is very difficult to extract from Fluent if you have a complex case with combustion.
1. Any idea if this problem (bulk temp) is fixed in new versions e.g. 14.5?

2. How to find the local heat trasfer coefficient and Nu in Fluent?

January 16, 2014, 04:40
#13
Senior Member

Flavio
Join Date: Sep 2011
Location: Brescia, Italy
Posts: 181
Rep Power: 6
Hi everybody,
I encountered the same your problem trying to define a Reference Temperature
In my simulation (see the attachment) there's a heating radiator with a lot of fins: along the radiator the air of course increase its temperature, so I can't use the same T-ref; probably the best choice should be taking T-ref from the plane between a fin and the adjacent one...
I set Enhanced wall treatment and y+=1 so I can't use Wall Adjacent temperature.
What do you suggest? (Maybe a tricky UDF...)

Best Regards
Attached Images
 1.jpg (21.5 KB, 51 views)
__________________
Bionico

 September 8, 2015, 13:50 #14 New Member   thomas Join Date: Jul 2014 Posts: 17 Rep Power: 3 Hello all, did you have any luck regarding this issue?

September 9, 2015, 10:00
#15
Member

Shaheer
Join Date: Jul 2015
Posts: 33
Rep Power: 2
Hi I have some problems in this zone. I have a straw piece and few high temperature steel particle and i am modeling to see how the heat transfer occurs thus i need bot the temperature change in transient time and the heat transfer coefficient. Now when i do try to find (after i have simulated the case and found the temperature variation at different point of time) the Surface heat transfer coefficient i am getting a blank 0 value. There also is 0 for wall heat flux which i am sure is the reason for this issue. If there was no heat flux how did ansys simulate the changeing heat of the piece ? As it did shuoldnt it also show something when i try to find the q'' of the wall and the surface and wall HTC?
I am almost on the deadline please a prompt reply will be very helpful. i have attached the post processing pictures i got so that what i wrote makes more sense, please a help in this will be highly appreciated.
Attached Images
 scenario 2 temp.PNG (33.2 KB, 9 views) scenario 2 SHTC.PNG (33.0 KB, 7 views) scenario 2 WHF.PNG (31.8 KB, 5 views)

 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 Stan FLUENT 20 March 11, 2014 11:42 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 Mark CFX 6 November 15, 2004 16:55

All times are GMT -4. The time now is 14:56.