CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

Am I right?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 1, 2005, 03:22
Default Am I right?
  #1
DAK565656
Guest
 
Posts: n/a
I'am modelling flow over the airfoil (in CFX). It's taken about four month already. I am constantly approaching to adequate results for Cd at high angle of attack before stall. Now I have a presumption that can explain a little increase in Cd (about 20-30%). Please tell me, can this fact influence on results. It is obviuos that if we increase mesh division on the surface of airfoil it should lead to better forces and, consequently, Cp values. As we know, cell size (I will talk only about surface flat cells) should be smaller on high curvative surfaces. It we consider airfoil - it is leading and trailing edge. Surfaces which are located along stream can be meshed with bigger cells. If I follow to these simple rules I get bad results: very big values of pressureForceX near big cells. To reduce such big values on surfaces that are almost parallel to flow I have to increase cell resolution. Doing this I get better results, big values of force are decreasing, but the negative side of this is extremely increasing of quantity of cells. How can I escape this? If I want to get good results I have to increase the number of cells. But it is limited by RAM. As an explanation, I can propose this: The biggest values of forces are located just on surfaces that are parallel to flow. So if we have bad resolution where, we can achieve force with small, neglegible error in ForceY, but very big error for ForceX. If we increase resolution, we have a very little correction of force vector, but this very little correction can lead to big change of ForceX, because ForceY is thousand times larger that ForceX. Also I noted, that if I set resuduals for convergence criteria thousand times smaller, I get more precise Cd (for instance from 0.023 to 0.019 - big change)

  Reply With Quote

Old   November 1, 2005, 14:45
Default Re: Am I right?
  #2
Mani
Guest
 
Posts: n/a
The cell size required for good resolution and convergence depends not only on the surface curvature. Resolution is required wherever you have strong gradients in the flow, and those may exist even near flat surfaces, e.g. in case of flow separation or compression shocks. And then there is also the numerical issue of cell aspect ratios and stretching... For ideal numerical behavior, your grid should be as smooth and regular as possible (neighboring cells are almost identical in size, and each grid cell is nicely dimensioned). Smoothness, combined with resolution, certainly implies a requirement of high cell count. There is no magic to get around this, unless you use higher-order methods to allow all your cells to be larger.

If by ForceX, ForceY,... you mean actual force (pressure times surface), you would certainly expect a larger force on a larger cell surface... but I suppose that's not what you meant.

As you found out, it's important to monitor your convergence, and you're bringing up a very good point. If your interest is mainly in drag, it seems natural that you would observe the evolution of Cd during the computation. You should be able to see the drag coefficient level off indefinitely, as the flow solution converges. "Converged" is a subjective term. Monitor the information of interest (Cd) to define that term for your case. It seems obvious that you cannot assign some arbitrary convergence criterium and assume everything to be fine, based on questionable prior experience, although I understand that this appears to be common practice. Usually, flow convergence is measured by some generic single parameter (maybe the R.M.S. density or pressure residual), which may not be the most appropriate in your case, because surface pressure may have converged long before the shear stress does. Every case is different, and requires you to monitor convergence of the various parameters of interest -- I cannot state this often enough. It should be considered common sense, but I don't think it's common enough, yet.
  Reply With Quote

Old   November 2, 2005, 01:27
Default Re: Am I right?
  #3
diaw
Guest
 
Posts: n/a
Mani wrote: Every case is different, and requires you to monitor convergence of the various parameters of interest -- I cannot state this often enough. It should be considered common sense, but I don't think it's common enough, yet.

--------------------------------------------------

It does appear that 'common sense' is usually a very rare & scarce commodity - 'uncommon sense' generally seems to prevail...

diaw...
  Reply With Quote

Old   November 2, 2005, 02:15
Default Re: Am I right?
  #4
zxaar
Guest
 
Posts: n/a
it is not hundred percent true, we been doing cylinder and sphere calculation for now more than a year, the worst results in terms of mesh sizes is the one i got with meshes more than 5 million, i get good results with mesh around 3 million cells and best with meshes around 2 million cells. and yes, in the meshes more than 5million cells we have yplus as small as 0.1 (other meshes yplus is around 1) and we were working with LES models using Fluent. I chaned the default wall functions to Werner-Wengle wall functions(alternate option for LES), but no change in results. Yes Cp values did get improved, but Cd Cl were 100% wrong.

It all depends on the cases , can not generalise.
  Reply With Quote

Old   November 2, 2005, 10:18
Default Re: Am I right?
  #5
diaw
Guest
 
Posts: n/a
Zxaar, for your 5 million cell cylinder model, what visual effects were noticed?

Did you perhaps try a pressure contour plot at say 512 contours per model space? Did you investigate the y-velocity component over the model - again, in high number contour plots?

Was the fringe-plot for pressure smooth, or did it contain small 'wrinkles'?

I would be very, very interested in seeing some of your plots.

What level of convection-stabilisation did you use - hopefully nil...

diaw...
  Reply With Quote

Old   November 3, 2005, 08:21
Default Re: Am I right?
  #6
DAK565656
Guest
 
Posts: n/a
To Mani: 1) I understand that high resolution is required in "special" zones of high gradient or flow separations and etc. But how can I correlate flow transition zone, where high resolution mesh required, with ability of transitional SST turbulence model to predict its location? Should I predict it by myself of should I apply high resolution mesh to all part of airfoil top surface? I guess that I should predict it by myself. 2) ForceX is the projection of Force vector on X-axis. And of course that's not what I meant. I meant high values of ForceX in regions, where I have bad resolution (on surfaces that are parallel to flow). And the remedy is high resolution of mesh. I cannot see physical explanation of increasing resolution in these regions (except transition). That is why I'm asking you. To diaw and Mani: You see, when you are experienced in some kind of knowledge, everything seems to be very easy and understandable and everything can be explained only if we apply common sense. The lack of knowledge cause uncommon sense. That's why I'm here, in forum

  Reply With Quote

Old   November 3, 2005, 08:51
Default Re: Am I right?
  #7
diaw
Guest
 
Posts: n/a
DAK565656 wrote: To diaw and Mani: You see, when you are experienced in some kind of knowledge, everything seems to be very easy and understandable and everything can be explained only if we apply common sense. The lack of knowledge cause uncommon sense. That's why I'm here, in forum

------------- That's excellent...

My take on the issue is simply this (I know not everyone will agree, but here goes):

I believe firmly that wave phenomena exist at a level below that of the typical 'bulk-flow' level on which we all work. This 'wave nature' of the N-S can evidence itself at times - especially if aroused by oscillatory pressure-gradients - either naturally-generated, or as the result of a mis-behaving numeric scheme.

I have found that one can use 'too small' a spatial dimension, with accompanying time-step & end up simulating the underlying 'wave field' instead of the bulk field.

I perceive that typical convection-stabilisation schemes actually act as 'wave suppression mechanisms' so that the bulk-flow field can be computed.

I firmly believe that wave-phenomena bring on the onset of instability & take it to its logical conclusion - the fully-turbulent flow field.

If a convection-scheme interferes with the very mechanism which induces the onset of instability, then how would it be possible to ever predict it?

I have been able to isolate the N-S singularity (in 1D so far - for 2D it is just a lot more maths & pde manipulation - 3D brings on a migraine) which I perceive to herald the onset of instability. This event occurs at ridiculously low velocities. I believe that it is precisely this 'beast' that convection-stabilisation schemes have been trying to 'smudge' out for so long, because no-one ever believed that a singularity could exist at such low speeds.

So, yes, it is possible to go too small in element size...

diaw...
  Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On



All times are GMT -4. The time now is 19:56.