
[Sponsors] 
Problem in getting mesh independent soluiton for flow over flat plate 

LinkBack  Thread Tools  Display Modes 
September 22, 2012, 04:23 
Problem in getting mesh independent soluiton for flow over flat plate

#1 
New Member
Baber
Join Date: Sep 2012
Posts: 12
Rep Power: 4 
i am working on laminar flow of water over flat plate. i have defined the properties of water at film temperature to fluent. I am very much confident about the boundary conditions i am using.
BUT The problem i am getting that when i start with coarse mesh and go towards the finer mesh my results for average heat transfer coefficient h gradually come closer to analytical result but then with increasing more mesh size, the values of h exceed the analytical value! why is it so ? how can i get it mesh independent . Help Please! 

September 22, 2012, 07:19 

#2 
Senior Member
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11 
Its a normal situation where you get numerical values greater than the experimental ones say for example if experimental value of heat transfer coefficient is 0.32 it is very much possible to have numerical value of 0.35 at the grid independent solution, hope it helps you


September 22, 2012, 14:25 

#3 
New Member
Baber
Join Date: Sep 2012
Posts: 12
Rep Power: 4 
Thankyou for your reply...
But, i mean the values keep on increasing as i increase the mesh size. If through correlations i want h(overall)= 303.6, Nu= 453.2 & Cf=0.002542 and i am getting it on one of the meshes ( i.e. in mesh size 4200, the result of which i have not shown below) & then with increasing mesh size the values keep on increasing 306,308,309,....! Mesh Size: 7920 cells Nu457.06h306.23w/m2kCf2.58E03 Mesh Size: 31680 cells Nu459.55h307.90w/m2kCf0.0025898 Mesh Size: 106480 Nu460.54h308.56w/m2kCf0.0025923 Mesh Size: 225280 Nu460.84h308.76w/m2kCf0.0025931 Can these results be called mesh independent ? 

September 22, 2012, 14:39 

#4  
Super Moderator
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,909
Blog Entries: 6
Rep Power: 38 
Quote:
yes............... 

September 23, 2012, 02:41 

#5 
New Member
Baber
Join Date: Sep 2012
Posts: 12
Rep Power: 4 
Thankyou Sir for your reply.
But can you kindly tell me what could be the specific reason behind it that instead of converging the soultion towards the correlation results with increasing mesh size, the FLUENT is exceeding or diverging the results from it? 

September 23, 2012, 02:47 

#6 
Senior Member
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11 
If the results for the next mesh are within 5% of the previous mesh results then results can be considered mesh independent


September 23, 2012, 02:51 

#7 
Super Moderator
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,909
Blog Entries: 6
Rep Power: 38 
For your case difference is less than 1% for the successive meshes, therefore solution can be considered as mesh independent.
Last edited by Far; September 23, 2012 at 03:16. 

September 23, 2012, 03:09 

#8  
Super Moderator
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,909
Blog Entries: 6
Rep Power: 38 
Quote:
Now there are many other parameters which affects the solution like flow scheme, turbulence model, geometry simplification, time marching scheme etc. General procedure I mostly adopt is : 1. First get the mesh independence with wall functions, simple turbulence model and simple boundary conditions. 2. Vary the Y+, if you think Y+ will play important role in your case. 3. Change the flow scheme 4. change the turbulence model. 

September 23, 2012, 03:18 

#9 
New Member
Baber
Join Date: Sep 2012
Posts: 12
Rep Power: 4 
o yahoo!..
Thankyou! Just one more thing...Do i need to Discritization error analysis now (although, till now i dont know how its done) as its done here in the following paper through Richardson Extrapolation Technique. I mean will i be at any advantage in doing that? http://www.google.com.pk/url?sa=t&rc...CrqZSummtaB8Q 

September 23, 2012, 03:23 

#10 
Super Moderator
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,909
Blog Entries: 6
Rep Power: 38 
It is always good idea to perform the Discritization error analysis using Richardson Extrapolation Technique, but taking the three meshes with smart guess from available literature is not bad idea.
http://journaltool.asme.org/Content/JFENumAccuracy.pdf 

September 23, 2012, 03:43 

#11 
New Member
Baber
Join Date: Sep 2012
Posts: 12
Rep Power: 4 
Thankyou Sir !
As you said in your reply post # 8.....So it means my results can be considered mesh independent but actually they are not ? Secondly, i should first go to turbulence modelling, get there mesh independent results & then i will be able to get mesh independent results for my laminar case? Lastly, the main advantage of doing discretization error analysis is, that it tells you what the grid independent solution would be ? 

September 23, 2012, 03:55 

#12  
Super Moderator
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,909
Blog Entries: 6
Rep Power: 38 
Quote:
Conclusion: Your results are mesh independent. PS. I assume you have significant change in mesh size in successive meshes 

September 23, 2012, 04:13 

#13 
New Member
Baber
Join Date: Sep 2012
Posts: 12
Rep Power: 4 
ok Sir, Thanks a lot for your replies...


September 26, 2012, 17:21 

#14 
Super Moderator
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,909
Blog Entries: 6
Rep Power: 38 
Here are the some results from the official ANSYS CFX simulation around circular cylinder and you can observe that with increasing the mesh size, results are deviating from actual values !!!


September 29, 2012, 12:59 

#15 
New Member
Baber
Join Date: Sep 2012
Posts: 12
Rep Power: 4 
For verification of my average results i need to plot local value results and those are coming with very fine meshing near the leading edge of the plate i.e by using high bias factor value for meshing. But that mesh is giving me the following warning:
WARNING: The mesh contains high aspect ratio quadrilateral, hexahedral, or polyhedral cells. The default algorithm used to compute the wall distance required by the turbulence models might produce wrong results in these cells. Please inspect the wall distance by displaying the contours of the 'Cell Wall Distance' at the boundaries. If you observe any irregularities we recommend the use of an alternative algorithm to correct the wall distance. Please select /solve/initialize/repairwalldistance using the text user interface to switch to the alternative algorithm. So Can this warning be neglected for Laminar Flows ? 

September 29, 2012, 13:11 

#17 
New Member
Baber
Join Date: Sep 2012
Posts: 12
Rep Power: 4 
ohk Sir!


November 25, 2012, 06:30 
Calulation of local Nu directly from FLUENT (ANSYS13.0)

#18 
New Member
Baber
Join Date: Sep 2012
Posts: 12
Rep Power: 4 
Is ther any way to obtain the local Nusselt Number direcltly from FLUENT (ANSYS13.0) ?
what i was doing that i first calculated flux (q) and bulk Temperature (Tb) from FLUENT and then by using the relation Nu= qx/((TwallTb)*K)) , i was able to get Nux (FLUENT). But could it be obtained somehow directly? I tried to use Different Report Types (Vertex Average,....) in Surface Integrals with field variable Fluxes>Surface Nusselt Number on the Points of Plate but it was no use. 

November 25, 2012, 20:23 

#19  
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 594
Rep Power: 11 
Quote:
For calculating the heat transfer coefficient and Nusselt number, Fluent uses the reference temperature specified in the reference values. Hence, a local Nusselt number is reported, but it is a Nusselt number based on reference temperature (not local bulk temperature). If you want a truly locally defined Nusselt number, it is better to use your approach. If you want to just compare, can you rewrite your relation to use the reference temperature instead? This should have "somewhat" worked. Is it not returning any report? If no, then your points are not on any surface. 

November 26, 2012, 14:52 

#20 
New Member
Baber
Join Date: Sep 2012
Posts: 12
Rep Power: 4 
Thankyou for your reply....
It is reporting me a value of Nux but not the correct one although its giving me correct values of hx and Cfx on the same Points along the Plate for the same mesh. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Moving mesh  Niklas Wikstrom (Wikstrom)  OpenFOAM Running, Solving & CFD  122  June 15, 2014 06:20 
High aspect ratio mesh problem for flat plate boundary layer  sam1364  OpenFOAM  2  May 14, 2012 15:54 
Setup of flat plate problem for laminar layer  pankos  Main CFD Forum  3  August 9, 2011 17:37 
Conjugate heat transfer for filmcooled flat plate  Michele  FLUENT  0  July 3, 2006 08:42 
unstructured vs. structured grids  Frank Muldoon  Main CFD Forum  1  January 5, 1999 11:09 