Problem in getting mesh independent soluiton for flow over flat plate
 

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!

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

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...............

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

For your case difference is less than 1% for the successive meshes, therefore solution can be considered as mesh independent.

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.

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

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

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 :eek: . 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

ok Sir, Thanks a lot for your replies... :)

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 !!!

http://imageshack.us/a/img821/6131/meshvsaccuracy.png


http://imageshack.us/a/img812/1221/meshvsaccuracy2.png

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 ?

neglect it

ohk Sir! :)

Calulation of local Nu directly from FLUENT (ANSYS13.0)
 

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?


This should have "somewhat" worked. Is it not returning any report? If no, then your points are not on any surface.

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.

Fluent also uses the reference length to normalize the heat transfer coefficient to arrive at Nusselt number. You can't get Nux only NuL from the simple reports. Again, you can cross-compare but it looks like your code is working.

grid independence studies
 

Hi,

I am working on semi-confined jet impingement cooling. My impingement surface (bottom of cylinder) is at 3mm from the nozzle exit (vertical jet)and at 600k. When I do grid independence studies , the nusselt number value at stagnation keeps increasing as the mesh gets finer. I plot - nusselt number vs radial distance.
Coarse mesh gives better result than finer mesh. How to get stable values!
Need Help!!!