# Problem in getting mesh independent soluiton for flow over flat plate

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

 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/m2-kCf2.58E-03 Mesh Size: 31680 cells Nu459.55h307.90w/m2-kCf0.0025898 Mesh Size: 106480 Nu460.54h308.56w/m2-kCf0.0025923 Mesh Size: 225280 Nu460.84h308.76w/m2-kCf0.0025931 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
Posts: 3,909
Blog Entries: 6
Rep Power: 38
Quote:
 Originally Posted by BHE 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/m2-kCf2.58E-03 Mesh Size: 31680 cells Nu459.55h307.90w/m2-kCf0.0025898 Mesh Size: 106480 Nu460.54h308.56w/m2-kCf0.0025923 Mesh Size: 225280 Nu460.84h308.76w/m2-kCf0.0025931 Can these results be called mesh independent ?

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
Quote:
 Originally Posted by BHE 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?
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
Posts: 3,909
Blog Entries: 6
Rep Power: 38
Quote:
 Originally Posted by BHE 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?
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
Posts: 3,909
Blog Entries: 6
Rep Power: 38
Quote:
 Originally Posted by BHE 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!
The exact results and mesh independent results are two different things. Mesh independent results mean that you are converging to the solution which does not change with further increase in mesh size.

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...CrqZSu-mmtaB8Q

 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
Posts: 3,909
Blog Entries: 6
Rep Power: 38
Quote:
 Originally Posted by BHE 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 ?
No . For laminar case, mesh independence should be with laminar solver. Above guidelines are general in nautre and applicable to both laminar and turbulent.

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 !!! cfd seeker, BHE and Crank-Shaft like this.

 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/repair-wall-distance using the text user interface to switch to the alternative algorithm. So Can this warning be neglected for Laminar Flows ?

 September 29, 2012, 13:00 #16 Super Moderator     Sijal Ahmed Memon (turboenginner@gmail.com) Join Date: Mar 2009 Location: Islamabad Pakistan Posts: 3,909 Blog Entries: 6 Rep Power: 38 neglect it

 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/((Twall-Tb)*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:
 Originally Posted by BHE 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/((Twall-Tb)*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.
Fluent can report Nusselt number directly but:
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 re-write your relation to use the reference temperature instead?

Quote:
 Originally Posted by BHE 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.
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 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 Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20 sam1364 OpenFOAM 2 May 14, 2012 15:54 pankos Main CFD Forum 3 August 9, 2011 17:37 Michele FLUENT 0 July 3, 2006 08:42 Frank Muldoon Main CFD Forum 1 January 5, 1999 11:09

All times are GMT -4. The time now is 04:02.