Fundamental mistake in mesh
 

Hi,
I have attached my completed 3D mesh in the below link..
https://dl.dropbox.com/u/79881940/CFD%20online.rar
Even though the quality is pretty good, the residuals start diverging even at low angles of attack such as 10 or 12degrees.
Can someone please check and tell me if there is any fundamental mistake in it.

Thanks..

try this mesh https://dl.dropbox.com/u/68746918/CFD%20online.zip

. Could you tell me the Y + and turbulence model

Okie.. i am running it now.. will let you know what happens

the mean wall Y+ is around 5 or 4.. Its S-A model with 1% turbulence of 0.015m length scale..

http://www.cfd-online.com/Forums/flu...re-outlet.html
this is what is happening to the residuals..

Hi far,
You are a saviour once again.. so far its working beautifully.. just crossed 500 iterations... will keep you posted about the developments when i switch to second order equations..
just to let you know.. all the residuals are decreasing regularly except for continuity which jumps up and down (but keeps decreasing ultimately)
Can you please tell what you did to the mesh..:D

minimum angle was less than 18 deg. So I just open up the blocking in far field

In this latest blocking min angle is 24 and quality is 0.6. In last blocking I have just uploaded min angle was 24 and quality was 0.4

https://dl.dropbox.com/u/68746918/CFD%20online2.rar

okie... in that case what are the other important pre mesh quality options that i need to take care of.. can you also please explain what you mean by opening the block in the far field..

thanks..

Most important parameters are quality and min angle. Quality should be > 0.3 and angle should be > 18.

By opening I mean, instead of vertical lines form wing to far field, I give them some angle (> 90 with respect to horizontal plane parallel to symmetry), which enhances the quality of mesh in far-field, where few elements are used to discretise the non important flow areas.

okie...
now i am running the same mesh with second order equations.. just to let you know,the residuals are all confused.. its increasing for some time and decreasing and then increasing.. i will anyway wait for another 600-700 iterations..
Do you want me to improve any of the pre mesh quality options further or shall i just wait!!

it may be possible that the problem is transient in nature and you are running steady state !!!

yes the problem is transient, but i need to converge it in steady state before moving ahead..!!!
and the residuals have started decreasing uniformly as well,, hope it sustains.. :)

The latest blocking which you gave still contains the quality at 0.4.. the block name is project1_improvment2.. but there was not geometry in the folder so i used the previous one..

This one ? https://dl.dropbox.com/u/68746918/CFD%20online2.zip

http://img29.imageshack.us/img29/5275/48714815.png

http://img715.imageshack.us/img715/1530/17850178.png

Far can you please explain what is the effect of minimum angle being less than 18 and what is the effect if its greater than 18 on the solution?

mate how can you get the converged solution for steady state if the problem is transient in nature? I think you are wrong here....if the problem is transient in nature then you will never get the converged solution in steady state.......

as in, i am looking for at least a third order convergence.. I am actually trying to find out the level of unsteadyness in the flow.. The amount of difference in accuracy of steady simulation and unsteady simulation..

Just for information. I think i found out the solution.. I was initially using Pressure outlet but later i tried with outlfow as the outlet boundary condition. This along with reduced under relaxation factors for pressure and momentum helped converge the solution.