
[Sponsors] 
June 19, 2019, 13:23 
NO Heating of Fluid regime

#1 
Member
Mayank
Join Date: May 2019
Location: India
Posts: 30
Rep Power: 6 
Dear All,
I am simulating a Pipe flow with pipe inner and outer diameter 0.02 & 0.025 m I have generated a pipe in ansys DM by slicing the body to get a quality mesh with patch conformation method now I simulating flow for RE 30000 with all properties as a polynomial function of temperature but after solutions are completed the fluid inside the pipe (water is fluid) is not heated the bulk temperature & outlet temperature all are same as inlet temperature even though desired flux is being obtain at wall and shadow wall but heat is not been transferred into fluid I have given a constant heat flux condition at outer wall Also the problem occurs only when I use polynomial function of properties with properties remain constant the parameters such as nusselt number, heat transfer coefficient are very precise within 3% error.. Please tell what can I do to resolve the same. Thanks in advance 

June 20, 2019, 12:49 

#2 
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,154
Rep Power: 22 
First off, that is not a quality mesh at all. Automesh with no slicing would have been better than that. Use sweep or multizone method. mapped faces. Define number of elements along your lines.
Check your polynomial functions, are you defining every property using poly functions? What are they? Do you have the interface between solid and fluid set up properly? WHith Heat Transfer Activated? Are you using thermal energy model? What is the point of modeling the pipe? Couldn't you just use an increased heat flux (reduced area) on the fluid interface instead? Why not use 1/4 symmetry? 

June 20, 2019, 13:38 

#3 
Member
Mayank
Join Date: May 2019
Location: India
Posts: 30
Rep Power: 6 
Dear evcelica,
First of all thanks for your reply, now the i have resolved the issue of no heating of fluid regime prior to your reply, but now I have been stuck with a new challenge the Cp value after some iterations get negative also the Amg solver get diverge and report temperature divergence I have reduced under relaxation factor to 0.4 for energy thereby there is very little convergence in energy and after 50 iterations too get diverge.... can you please suggest something more in that I will do whatever you suggest for meshing but very sorry about your symmetry idea I do have that in my mind by this a task for me get results by constructing the whole pipe... Thanks in advance 

June 20, 2019, 14:47 

#4 
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,154
Rep Power: 22 
What are your polynomial functions? Probably an error in there somewhere.
Do you have both density and Cp functions of temperature? 

June 21, 2019, 03:43 

#5 
Member
Mayank
Join Date: May 2019
Location: India
Posts: 30
Rep Power: 6 
for thermal conductivity
p1 =1.557e06 p2 = 2.507e06 p3 = 8.76e06 p4 = 1.378e06 p5 = 0.0004687 p6 = 0.009557 p7 = 0.6273 for density p1= 4.163338140310400e09, p2= 2.288685213418900e05, p3= 0.022795985738390, p4= 7.673279806950824, p5= 1.619465248545898e+02 for Cp I have p1 = 1.466e06 p2 = 1.07e07 p3 = 1.049e05 p4 = 4.457e05 p5 = 0.0005408 p6 = 0.0002127 p7 = 4.179 For Mu p1 = 7.183e09 p2 = 1.789e09 p3 = 4.529e08 p4 = 8.544e07 p5 = 8.943e06 p6 = 8.642e05 p7 = 0.0006821 with equation as P1 x^7 + P2 x^6 + P3 x^5 +.........and so on, if you do not mind then I have one more doubt before using variable properties I check the the result obtain by my mesh for constant properties the results for patch confirming method are within 3% but for hexa mesh by sweep method are very over predicting (results here are Nusselt Number and Heat transfer coefficient) the results with a tetra mesh are more precise than a hexa mesh by sweep method in spite of the fact that the average skewness for hexa is of order 10^2 and for tetra is 0.2 aspect ratio for hexa is 2.86 and for tetra is 4.98 and orthogonal quality for Hexa is 0.987 while for tetra is 0.887 I was aspecting that results for Hexa will be more precise then terta can you suggest something on this as well the picture of the mesh hexa one is uploaded with this reply 

June 24, 2019, 14:12 

#6 
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,154
Rep Power: 22 
You should not define both Cp and density as functions of temperature. This will result in thermodynamic inconsistencies.
Also you specific Heat function is negative everywhere Temperature is above 0. The solver uses Kelvin as default units, did you make your curve fits using Celsius or something else? You can check them by plotting you expression. You also need to include a lot more digits in your polynomials, you get large truncation errors. The equation you gave me is also incorrect, I believe you mean P1 *T^6, not T^7. This looks like water? Still, it goes negative above 13K. you may want to consider using tables (user functions) instead of polynomials if you are having trouble with them. Also make sure if you do use polynomials, you have some padding on each end of you function so the number doesn't shoot off to something totally wrong if you are a bit above or below your temperature range during at iteration. I would recommend user functions instead of polynomials, and use the extend min/extend max options. The standard variable for HTC are completely mesh dependant, as it uses the adjacent wall node temperature for the bulk temperature. A smaller mesh = a higher HTC. See the FAQ's for info and ways of calculating HTC and Nusselt number the more accurate way: https://www.cfdonline.com/Wiki/Ansy...ficient_in_CFX 

June 25, 2019, 13:17 

#7 
Member
Mayank
Join Date: May 2019
Location: India
Posts: 30
Rep Power: 6 
Thanks sir for you help you are exactly right the problem is with function only and taking Cp and Density as function of temperature both simultaneously I need your slight help in postprocessing now I want to generate multiple surface nearly about 600 and wanted to compute areaweighted  avg of thermal conductivity on each surface I want to get a print only of those properties with surface name and indicated average of thermal conductivity on it.
(Do ((x 0.00333 (+ x 0.00333))) ((> x 600)) (Timenuloadstring (format #f “surface/isosurface zcoordinate zplane~a () () ~a” x x)) ) (DO ((x 0.00333 (+ x 0.00333))) ((> x 600)) ( Timenuloadstring (format #f "report/areaweighted average/zplane~a () / temperature" x)) ) I am Using this command the surface are created as desired but the average is not been generated and shows invalid command can help me out in corrections for avg calculation command. Thanks in advance... 

June 27, 2019, 12:35 

#8 
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,154
Rep Power: 22 
I have no idea, I have never done anything like that. You should start a new thread for this.
I would have meshed it orthogonality to your planes, then exported the results (x,y,z,variable) and done this post processing and averaging elsewhere (like excel). 

June 28, 2019, 08:11 

#9 
Member
Mayank
Join Date: May 2019
Location: India
Posts: 30
Rep Power: 6 
Okay no problem I managed to get it solved it but Thanks for your help and replying on my thread.


Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Physics of an incompressible fluid  Jonas Holdeman  Main CFD Forum  87  April 22, 2019 10:40 
Error in Two phase (condensation) modeling  adilsyyed  CFX  15  June 24, 2015 19:42 
Water subcooled boiling  Attesz  CFX  7  January 5, 2013 03:32 
My Revised "Time Vs Energy" Article For Review  Abhi  Main CFD Forum  2  July 9, 2002 09:08 
Terrible Mistake In Fluid Dynamics History  Abhi  Main CFD Forum  12  July 8, 2002 09:11 