
[Sponsors] 
September 14, 2015, 12:37 

#21  
Senior Member
Join Date: Feb 2011
Posts: 496
Rep Power: 18 
Quote:


September 14, 2015, 16:35 

#22  
New Member
Dmitry
Join Date: Feb 2013
Posts: 28
Rep Power: 13 
Quote:
In CFX alpha computed as alpha=Qwall/(TwallT1stLayer)  without 'tbulk for htc' and alpha=Qwall/(TwallTbulkForHTC) with determined T bulk for HTC. Here the T1stLayer is temperature of the first node near the wall, TbulkForHTC is 'tbulk for htc'=300 K. For industrial facilities much more interested parameter is Wall Heat Transfer Coefficient that determined as alpha=Qwall/(TwallAveTLiquid). Sometimes difference in Wall Heat Transfer Coefficient in 2030% is critical. In case of 300% error CFX looks like completely useless CFD code for convective heat transfer simulation opposite to Fluent or StarCCM+. 

September 15, 2015, 03:39 

#23  
Senior Member
Join Date: Feb 2011
Posts: 496
Rep Power: 18 
Quote:
Code:
LIBRARY: ADDITIONAL VARIABLE: Tw Boundary Only Field = On Option = Definition Tensor Type = SCALAR Units = [K] Variable Type = Unspecified END END FLOW: Flow Analysis 1 DOMAIN: HeXe FLUID MODELS: ADDITIONAL VARIABLE: Tw Additional Variable Value = T Option = Algebraic Equation END END END END 

September 16, 2015, 05:13 

#24  
New Member
Dmitry
Join Date: Feb 2013
Posts: 28
Rep Power: 13 
Quote:
I have got Nu~572 (sidewall temperature averaging procedure was Twall=areaAve(Tw)@Sidewall) in case of coarse mesh (y+~45). Theoretical one value is Nu=575. So. The error of wall heat transfer coefficient computation was connected with the sidewall temperature computation. It don't clear for me why averaged sidewall temperature for additional variable Tw different from averaged sidewall temperature for Temperature field. I have read Modelling guide 2.7.5.62.7.5.9 but there is no answer. 

September 16, 2015, 06:22 

#25  
Senior Member
Join Date: Feb 2011
Posts: 496
Rep Power: 18 
Quote:


September 16, 2015, 06:22 

#26 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,728
Rep Power: 143 
Nice work Antanas. Kudos for that one.


September 16, 2015, 08:45 

#27  
New Member
Dmitry
Join Date: Feb 2013
Posts: 28
Rep Power: 13 
Quote:


May 13, 2016, 02:11 

#28  
New Member
Join Date: Feb 2016
Posts: 22
Rep Power: 10 
Quote:
Trying to edit the variable in the command editor results in "The parameter "Boundary Only Field" is present in the object "/LIBRARY/ADDITIONAL VARIABLE:Tw" but it is not physically valid." What am I doing wrong? Edit: Found the problem. I had not enabled Beta features. Now it works fine. Thanks for the posts! 

May 13, 2016, 07:26 

#29 
New Member
Join Date: Feb 2016
Posts: 22
Rep Power: 10 
Hm. This super variable did not help me..
So I hope that some of you guys will have some ideas of where I am thinking wrong. I have a square duct with a specified heat flux from two opposite walls. The fluid is air as an Ideal gas. The duct is approximately 20 hydraulic diameters long with a Reynolds number of 80 000. The mesh has a y+ of ~0.5 and turbulence model is komega sst with reattachement modification (not specifically needed for this smooth channel case, but comes in handy when adding for instance ribs to the walls). The inlet has a boundary condition of fully developed flow profile with an average velocity of 16 m/s and a constant temperature of 293.15 K. The outlet has relative pressure 0 Pa and the heated walls a heat flux of 1000 W/m^2. The unheated walls are considered to be adiabatic. The reference pressure is set to 1 atm. Nusselt number integrated from area averaged values on spanwise sections. Nu = Qwall*Dh/(k*(TwallTfluid)) Tfluid is the average temperature of the temperatures at the inlet and outlet, Dh hydraulic diameter, k average conductivity from inletoutlet and Twall the temperature at the wall. Results: DittusBoelter: Nu ~175 CFX: Nu ~120 When I use the above mentioned additional variable I get almost the same temperatures on the wall. areaAve(Temperature)@wall1 = 342.351 K and areaAve(Tw)@wall1 = 342.539 K. Any ideas of what to test next? Should I expect the Nusselt number to be around the Nu of DittusBoelter even though I only have two heated walls out of four? 

May 13, 2016, 15:41 

#30  
New Member
Dmitry
Join Date: Feb 2013
Posts: 28
Rep Power: 13 
Quote:
1. You have only 2 out of 4 heated walls. That means you should to obtain twice lower Nu number; 2. You didn't have stabilization of thermal field at the inlet of the pipe. This condition lead to incresing of heat transfer coefficient in comparison to stabilized flow. And don't forget that DittusBoelter equation is applicatiable only for the flow with stabilized heat transfer. So, try to compute heat transfer in long pipe (approximately 100 gauges) with uniform wall heating. Then try to compute averaged by perimeter of the pipe wall Nu number in cross section with longitudinal coordinate equal to 80 gauges. I'm shure, you will obtain pretty good coincidence of Nu number with value that you were computed by DittusBoelter equation. You have been obtained low difference between temperatures, computed by common Temperature variable and temperature, that was recorded in Additional Variable, due to low Pr number of air and low value of y+. Try to compute with y+=50, difference will be much higher. And don't worry about quality of computation at high y+. Just beleive in near wall functions ))) 

May 14, 2016, 09:55 

#31  
New Member
Join Date: Feb 2016
Posts: 22
Rep Power: 10 
Quote:
I made a major error when constructing the mesh and with a new mesh methodology I obtain Nusselt values that are + 10% of the DBcorrelation. The mesh was poorly constructed from my side, eventhough the y+ was below 1, the transition from inflation layers to the bulk mesh was not sufficiently balanced. I deem these results as accurate. However, I agree with you regarding the thermal field and that is of course contributing to the results being a bit inaccurate. And regarding the Nusselt number. I do not agree with you that I should expect it to be halved compared to a uniformly heated channel. I have read in literature and made simulations that suggests that the Nusselt number is not highly dependent on the wall temperature. And the DBcorrelation requires no temperature input, which is also pointing towards a Nusselt number being more or less the same, for a fixed geometry, whatever the temperature boundary conditions are. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Separate Convective and Radiative heat transfer in CFD post using fluent as a solver  Lemanes  FLUENT  1  July 6, 2015 10:31 
CFX does not solve heat transfer at fluidsolid interfaces  Ivan Corgozinho  CFX  2  April 7, 2015 00:08 
convergenceof natural convection prob. in cfx  cpkewat  CFX  15  January 31, 2014 06:29 
mixed boundary conditions including heat flux, convective heat transfer and radiation  lotus_blue  FLUENT  0  April 3, 2013 18:55 
Water subcooled boiling  Attesz  CFX  7  January 5, 2013 03:32 