Hi Razvan, I saw the post you wrote about polyhedral meshes. Very very interesting, I think that you wrote something very useful for all of us!! I have a question about the lift/drag forces that you explained Carlos about a racing car. Is the method you described suitable to get the Cl and Cd from a 2d airfoil simulation? I hope it is! because I was dealing with that problem for a while without good results (regarding the Cd).

Thanks for your help!

Hy HSeldon,

I'm glad that I can be of any help for somebody in need. I remeber myself having problems years ago and not being able to request any help from anyone at all!

Now about your problem, I can say that it is a lot more difficult to get quantitatively correct results for global forces and moments with a aero/hydro-dynamic body/shape than in the case of a bluff body! It could sound stupid to you, but you have to take a closer look to the two types of bodies and their related flow patterns:

- the aerodynamic bodies drag is determined mostly by friction drag and a lot less by the the pressure drag; friction drag is highly dependant on B-L modeling (e.g. turbulence model, wall functions, etc.), especially in the presence of adverse pressure gradient, shocks and other phenomena that can lead to B-L separation;

- the bluff bodies, on the other hand, have similar importance of pressure and friction drag forces, the B-L is always separated and the separation point/line is most of the times clear and almost fixed (except maybe sphere-like shaped objects); also, pressure drag is far better predicted by CFD then friction drag, consequently the global forces are better predicted (the viscous errors are less important...).

For example, in the case of NACA0012 2D airfoil, the best result I could obtain using classic RANS approach was +20 percent error for Cd at null incidence! But for DLR-F4, even for a y+=40 grid I could get only +5 percent for Cd! And that because pressure drag is much more important in the DLR-F4 case than in the NACA0012 case.

So you see that this is not an easy task. To be able to improve that +20% Cd, you MUST use at least DES. And that of course, implies that you have to reconsider many things:

- first of all, the usual structured grid, with highly streched cells in the B-L is no longer appropriate. DES grid must use little streched cells, B-L included: you must not exceed a 10:1 ratio. But you will immediately reply that it will lead to an excessive number of cells in the rest of the domain, because a 10:1 ratio in the B-L grid needs a too high number of nodes on the airfoil. That's true, you could need about 300-400 nodes on the airfoil alone!

- second, the growth ratio must be very low, not to exceed 1.05 actually! This too leads to astronomical cell counts.

- third, the simulation must be unsteady, and the lower the stretch ratio, the lower the time step needed due to CFL limitation!

One solution could be to use a hybrid grid, structured in the B-L region only, and unstructured in the rest of the domain, with very small cells behind the trailing edge.

Anyway, I have to warn you that even this approach is not good enough, and that is true because 2D DES or LES is not advisable, due to high three-dimensionality of the phenomena. A much more correct approach would be to make the problem 3D by sweeping the airfoil for about one chord, and the mesh can be easily created in the same way, using Cooper scheme.

If you think that you want to try this, then let me know, and I'll do my best to help you.

All the best, Razvan

Thanks for the fast response Razvan. I see very clear what you mean... so it looks like a difficult problem in general, huh? But I will give it a try anyway to see what happens.

I´ll tell you when I get the first results. By the way, how small the time steps could be, and what´s the propper value of Y+ for DES?

Thank you!!

You don't have to acurately calculate a value for the time step. For the start of your simulation, simply choose it using this: delta_t=chord_leght/(n*V_mean), where n=0.5*total number of points along the airfoil. This should give you a value for delta_t very close to CFL=1. Actually, near the leading edge, CFL might be a little over 1 , but that you will immediately see if plotting Courant Number in the flow field.

After all, CFL does not have to be less than 1 all over the airfoil. The really important region is near laminar/turbulent transition point. For example: for NACA0012 at Re=500,000, transition point is somewhere about 65-75% chord lenght. So the best time step would be the one that will give you CFL=1 at approx. 50% chord leght.

As I already mentioned, the easyest way to verify CFL is to plot it in Fluent, after taking a few time steps. Of course, before activating DES, you should already have a fully converged solution, and my advice would be to calculate it with SST-kw (transitional) turbulence model. Also, when activating DES, you should coose SST-kw DES, although S-A DES will do a good job too.

In my calculations I found that y+ should be around 1 for the best results, even if it is DES. S-A and SST-kw need y+=1 for best results, they are Low-Re turbulence models, and they best behave on a fine mesh.

All the best, Razvan

Thank you!! I have a lot of info in order to start. I´ll let you know ASAP.

Thanks again.

Thanks for the very interesting response.

However, I'm not that convinced that you have to do a transient DES simulation in order to predict fairly correct friction forces on a streamlined body like a wing.

My experience is that transient DES simulations are necessary mainly when you try to predict unsteady flows, like for example a large separated region at off-design condition or transient vortex sheddings etc.

For a steady on-design flow around a stream-lined body I would guess that a good two-equation model or a RSM model would predict as good results as a DES model based on Spalart-Almaras or SST k-w. Have you got any examples on steady flows where a DES model gives superior results? If the flows are unsteady then where are the unsteadiness aside from the low-scale turbulent motions? Do you have some kind of large unsteay vortexes that you claim to be able to resolve with DES and which are important for the end results?

Predicting correct Cd on a wing can be quite diccult though as you say. As you mention friction forces are important and this makes the turbulence modeling and the turbulent inlet conditions especially important. One some wings you might even have laminary regions followed by transition. Predicting transition is very difficult and will of course affect the friction forces significantly.

Hi Jonas,

Thank you for your gentleman attitude.

In theory you are perfectly wright. There should be no need for DES or LES in the simulation of airfoils at low angles of attack. Unfortunately, practice says different. The case I studied for a long time was the NACA0012 airfoil at Re=500,000. The initial approach was: fully structured grid + all RANS turbulence models, from S-A to RSM, including "hidden" low-Re k-e models. All the efforts were more or less in vain, the best result I could obtain after perfecting the grid up to excess (mean y+=0.8, max. growth ratio=1.05, 130,000 cells for the 2D grid) and refining the Fluent model at max. available (PRESTO for pressure, MUSCL for momentum and turbulence), was +23% for drag (0.00889 instead of exp. 0.00725). And that using SST-kw. RSM made a complete fool out of itself, was literally just as bad as any two-equations k-e model!

At that moment I decided to switch sides an see what DES and LES have to offer. I was tempted to skip DES at first, due to lower quality results I had obtained for a backstep configuration simulated previously, and to go directly to LES. But in this specific case, DES proved to be more than OK. Unfortunately, not for 2D... 2D DES (and LES) underpredicted Cd too much (by almost 10%), so I decided to go for 3D. And the results were much closer to experiment this time.

The most important thing that I noticed with DES&LES was the much more accurate transition point prediction than all RANS models. SST-kw predicted transition point at about 40% chord, and DES&LES moved it back to approx. 70-75% chord. The natural immediate conclusion would be that even if LES is limited to outer B-L in DES formulation, it has a very significant influence on RANS calculated inner B-L. And that could be explained this way: toward the leading edge of the airfoil B-L is very thin and LES dominated region is closer to the airfoil, so turbulence production/destruction is heavily influenced by it (turbulence level is kept low). And transition point location is directly dependant on turbulence production/destrucion, as we all know. All RANS models suffer (more or less) from overproduction of turbulence at leading edge, no matter how complicated they are.

With the introduction of Fluent 6.3, low-Re k-w RSM became available. I had already tested it, but the results are not even as good as SST-kw's! And that inspite of the more accurate transition point prediction. I am speechless...

All the best, Razvan

If you have a wing where a large part of the boundary layers are laminar (you mention results from 40% to 75%) then I think that you need to use some kind of separate transition model that has been tuned to similar cases.

From my experience it is virtually impossible to predict transtion with a two-equation model on cases with a blunt leading edge, like for example a NACA arifoil. To predict transtion you also need very good information about the incoming turbulence level and length scale. If it is an aircraft wing in atmosphere you will also have so low turbulence levels that the boundary layers migt undergo natural transition caused by instabilities in the laminar boundary layers, as opposed to a by-pass transtion caused by diffusion and convection of free-stream turbulence into the boundary layers. Natural transition is definitely impossible to predict with a two-equation model. By-pass transition some people claim to be able to predict using models like the SST k-w model, but my experience is that you still require a separate transtion model also for high turblence cases with a more simple by-pass transition.

I don't think that a DES model should be able to predict transtion better than a SA or SST k-w model. It might by chance give different results. Without knowing anything about your results, I would even dare to suggest that it migt be luck that the DES model happens to predict a more correct transtion location in your case.

The fact that you obtain too high Cd levels with most turbulence models is quite natural since a large part of the boundary layers on your airfoil are laminar. Most turbulence models have a tendency to predict turbulent boundary layers. One reason is, as you say, that most two-equation models based on the bousinsesq approximation have a tendency to predict too high turbulence levels in regions with large normal strain, like in the leading edge region. This will often cause a too early transition location and too high Cd values. Note that the DES models should have a similar problem. The SA based DES model might have less leading-edge problems since SA is not as affected by this as a two-equation model.

By the way, running 2D DES is in my world not very physical. If you want to predict transient large-scale vortices you need 3D to get any physical results.

Have you got any experimental results for your case which shows transition locations? Perhaps you even have boundary layer profiles from the laimnar and the turbulent parts? How accurate incoming turbulence levels and length-scales do you have? Do you have any transient measurements? Did you make any simulations where you by-force (using a UDF or so) specified the transition location based on measurements?

You are practically taking the words out of my mouth/mind! Everything you have written, I agree.

For example:

- free stream level of turbulence, in the experiments is not pointed out, but based on all other exp. wind-tunnel measurements I know about, I set it identical for all simulations, RANS or DES&LES: 0.2% Tu_intensity;

- transition point is also not specified, I simply deducted it using this judgement: first simulation was a forced laminar one (not to mention that this was just as difficult as any DES simulation, because of the impossibility to obtain steady results, and the need to calculate it with unsteady solver), and the resulted Cd was compared to exp. Cd, RANS and DES&LES Cd; obviously, laminar Cd was under the exp. Cd, RANS was way over, and 3D DES&LES were very close, so I simply considered DES&LES transition location to be nearly correct, give or add 5%;

- I already said in my previous post that 2D DES&LES were not at all satisfactory for this case (although for that backstep configuration, 2D LES was quite good, beat the hell out of RANS).

These answers might be disappointing to you, but I have to warn you that I am just a passionate young man who's mouth might go ahead of his knowledge sometimes, who has a lot more to learn form people like yourself. All I know (or think I know) is based on self-taught experience, I seldom had the chance to learn something, anything at all, from an highly experienced an good-willing person. I do not work in a big and renowned profiled institute or company (and I might not get to, anyway). So you see, I'm actually nobody. All I am, after all is just a name on a very respected CFD forum, giving advice at my best, and in the same time picking valuable information from interesting posts.

If you think that all this was just a waste of time, I beg for your forgiveness, but for me it was a rich and honourable discussion.

Thank you, Jonas,

Razvan

Hi again Razvan,

Please don't judge my comments about your messages as any kind of complaint. I thought that your messages were very interesting and I wanted to learn more about it. Has anyone else made any kind of transition simulations using a DES model? I haven't really thought about that before.

Some time ago people started running LES simulations without any explicit sub-grid model, they just used the numerical diffusion as sub-grid model. This was joked at by many experts then, but now it has become a well regarded technique that many use and many do research on. So you shouldn't judge new experiences too easy in the tricky field of CFD. It is often good to listen to what other people say. The fact that someone does not work for a highly regarded university does not make his experience incorrect. The willingness to learn new things, try your own things and share your results is more important than the university or company you work for

It is a pity that you dont have either inlet turbulence conditions or measured transition locations for your airfoil case. That makes it kind of difficult to use this case as a validation case for CFD and turbulence models since the main problem is transition prediction which most often requires a separate transition model to be predicted correctly.

About 2D LES. That is definitely not physical at all. I'm surpriced that Fluent actally allows you to run LES in 2D. LES requires you to resolve eddies in 3D in order to obtain correct vortex dynamics (decay, stretching, ...)

Hi Jonas,

Thank you so much for your kind comments.

Sometimes I look behind and see all this work I have done in the past, that now just lies there on those hard-disks or DVDs, piling up dust and not hoping anymore to see the light of sharing, and I say just like that: it's a pity... But what can I do? You see, that's exactly where those great universities or companies could have miraculously intervened to repair this situation. At this moment, it exists just for me, and worths nothing for anybody else.

And about Fluent and 2D LES: it does not actually allow everyone to use it, it was implemented just for testing and learning purposes, not for real life use. Therefore, one can access it only through a specific scheme command, never mentioned in the docs, even 2D LES capability is not at all evidenced anywhere in the official docs.

Thank you again,

Respectfully,

Razvan

Hi Razvan, Thanks for your input. It has been very useful since I am trying to validate the flow solver against experimental solutions. So far my airfoil calculations have been limited to 2D RANS solver with k-w SST model for a NASA LS airfoil. For a linear angle of attack range of 0-12 degrees based on chord Reynolds number of 6.0 million and Mach 0.32, I have obtained Cd data that is within 7-10% of experimental solutions. However in this case the transition point was known from the experiment and I was able to input this into my simulations. However for the case, where transition had to be estimated, RANS model fails miserably.

As a result I am now examining the prospect of using DES to observe solution converge for the same case study with hope that it can a) predict the onset of boundary layer transition and b) provide reasonable Cd predictions compared to RANS model particularly at higher angles of attack.

For the RANS model I utilized a simple structured grid and for a DES model a hybrid grid is modeled. I have implemented a structured B-L over the airfoil and a tri mesh over the remaining domain. I just want to be clear as to the 'suitable' mesh requirements for a DES case, hence seek your advice.

In your previous statement you mentioned a 10:1 ratio over the B-L. What is this referring to? Also I am not sure why an unsteady model is required? Any suggestions/feedback would be greatly appreciated. Look forward to hearing from you soon.

one more question Razvan! How is the B-L transformed when the 2-D model in tranformed to 3-D through the sweep functions in GAMBIT. The B-L is no longer tranferred to the new volume from the 2D case when the sweep function is employed. Any suggestions? Thanks

Delete the B-L and keep only the face(s) mesh, then create volume(s) by sweep-face operation, "with mesh" option being activated.

If you need a certain nodes distribution in the sweep direction (default will be uniform, with interval size = 1), you should create an edge (by sweep-vertex operation, for example) in the needed sweep direction (usually z direction), with the required lenght and nodes distribution. Then, when using sweep-face operation, choose "edge" instead of "vector", and pick the previously created edge. The volume mesh that will be created, will match the nodal z-direction distribution of the selected edge.

All the best,

Razvan