Numerical diffusion is a very simple but damnable mechanism:

- Fluent stores variables values in cell center, but when passing these values to surrounding cells, it uses cell faces;

- you can easily imagine that when flow is not normal to cell faces, there is always a normal and a tangential component of any variable flux;

- these tangential fluxes are "lost" by the discretisation scheme, and although taken into account by the solver through other corrections, they are never completely recovered, so the smaller vortex, or other flow structures (compared to local grid size) are, the faster they will be shut down by this phenomena.

One way to deal with this problem is to locally refine grid (now you realise why everybody say "refine the grid in the wake of the car"), this way a certain flow structure will be covering more cells at a given moment and numerical diffusion will have a smaller impact on it. Another way is to use higher order discretisation schemes, which approximate much better the information exchange between cell centers through non-perpendicular cell faces. These two methods are someway competitive: a certain refined grid could give you same good results using 1st order discretisation as a less refined grid but using 2nd order discretisation. So, what you have to do is to find the compromise grid: good results using 2nd order discretisation and lowest number of nodes possible! Tough job!

Now you see that using the same grid with 1st order and then 2nd order dis., will always give you better results on second run.

Another pertinent observation: when using structured grid and the flow is aligned with the grid lines AND cells have good quality (low skewness), there will be normally a low numerical diffusion (small tangential components of fluxes). On this type of grid, 1st order is many times enough. But with unstructured grid this will never happen. So you MUST always use 2nd order dis. in that case.

A final word. You said that you are using QUICK scheme. I am not convinced that you use structured grids on your cars, so I must warn you: QUICK scheme is functioning only for structured grids and is actually a 3rd order scheme (locally). For unstructured grids, only 2nd order dis. scheme is working (in 6.2 they introduced MUSCL scheme, which is 3rd order and is noticeably better when used with these grids, than 2nd order). So don't use QUICK in this case, it will eat your computer memory and CPU time for same accuracy as 2nd order scheme.

I am sure this will be enough for you.

As for vortex shedding, it's easy to imagine that for a brick tipe geometry, when flow is aligned with the long side (like in a car case), there will exist lateral and vertical vortex shedding, but no longitudinal. Vortex shedding occurs only "behind" objects.

Best whishes, Razvan

Thank you very much for your advices, Razvan: they go allways to the point! Now, I cought a bit the idea of numerical diffusion: it could be compared in a some way to the roundoff error made by computers while making some hard calculations; at the end, the real solution is lost in the process and only an increase of the resolution in the number of bits (equivalent to switching to 2nd or 3rd order schemes) makes the solution to be more precise.

Yes, you're right: I'm using unstructured (tetrahedra) grid, and for the boundary layer I made prisms from the extrusion of the surface of the car: 3 layers with the first layer being 3mm. I used QUICK because it is suitable with hexa and hybrid meshes, but I wasn't sure the use prismathic elements in my grid would be a good reason to switch on the QUICK scheme... but I didn't find any reason to not to use QUICK, so I switched it at the end, understanding that in tetrahedra Fluent will use allways the 2nd order upwind as habitual (as it says in Fluent user's manual). Do you know if QUICK could give more benefits to grids having prisms than using "only" the 2nd order upwind or QUICK does not count these kind of elements as it happens with tetrahedra?

Thaks a lot for your dedication.

Regards, Freeman.

Onestly, I do not know the answer to your question about QUICK's benefits on prism meshes, but one thing I know: 3 layers B-L is too few! Take my advice and if you really want your B-L to have an impact, make it 6-7 layers, at least! On tetrahedral grids I ALWAYS used 10 layers B-L with a 90% under 0.1 skewness surface mesh!!! This is more important than you can imagine. Of course, such a B-L is hard to extend without intersections or big deformations, but I have a secret: I always construct a offset, shell of the original geometry and split the flow volume with it. In this new volume, by judiciously partitioning, I can create a high quality prism mesh (with triangles and quadrilaterals also, in the appropriate regions!).

Try this. You won't be dissapointed.

Best whishes, Razvan

Many thanks Razvan! I wanted to try your suggestion before writting here, but as I was afraid, 10 layers increases a lot the final mesh; But you are right, trying with 6 layers the stability of the solution is higher than it was! Residuals are a bit higher than they were with 3 layers simulations (I believe that it is because I haven't tried to make partitions of my volume and the extrusion is in some locations not as good as I desired), but the results oscillates less (specially Cl). As you might now, as my simulations have an academic purpose, I think that the accuracy I got with 3 layers should be sufficient (but at the end, I am limited by the computer of the university)

Could I ask you the last think? I remember the concise but very clear explanation that you wrote few days ago replying to the question I ask you about numerical diffusion, and thinking about it I was wondering if the effect of the skewness has a similar effect in the solution like the numerical diffusion has. I say such thing because in highly skewed cells, flow is not aligned with the faces of the cells and it is easier to the solver to loose the real tangential component information of the flux by making the aproximations you said; is there any other implication to the solution in a highly skewed mesh a part from that (if my statement was right)? And the normal information of the flux is taken "as is" (without aproximations like the tangential component)?

Thank you very much for your kind help.

Regards, Freeman.

Your inference is perfect! Yes, skewness has the same effect on precision as a non-aligned mesh.

Now let me give you some simple but interesting ideas. Let's take the perfect cells: a square and a triangle. What is the worst situation these cells can find themselves in?

- the square is standing with one diagonal along the flow -> angle between flow direction and cell edges = 135 deg.

- the triangle is standing with one edge normal to the flow -> angle between flow direction and the other edges = 160 deg

Now, adding the fact that square cell rotated 45 deg becomes numerical-diffusion-free and the triangle will never reach this state no matter how we rotate it, it is easy to understand why structured meshes will ALWAYS be better than unstructered ones!

Again, let us make things even worse by adding skewness. You can easily imagine the effect of that: increasing the angle, i.e. numerical diffusion. If that cell has a 0.95 skewness and one edge parallel to the flow, the other edges will be close to 180 deg!!! This type of cell is heavily damaging.

Solvers can be compared in terms of stability and convergence using skewed meshes. This "skewness resistance" is one thing I like so much about FLUENT. I can boldly say that it is the most stable solver I had the chance to work with. It will not crash , even if skewness goes close to 0.97, of course using hand-picked settings. Anyway, precision will be strongly affected, so it would be a good idea to avoid placing such cells in important regions (especially B-L).

Good luck and never quit, Razvan

Dear Razvan, I found nothing in your intervention that contradict mine....By the way it is a good and interesting intervention...

1) My intervention was strictly reserved to people who want only a pure "STEADY STATE" solution.

2) I never said Freeman's results are wrong.

3) To sum up, and I only said that if you are looking for a steady state solution, you should do whatever possible to get it...and I think it is possible to get it...specially with eddy viscosity models.

4)The physical unsteadiness is contained in the Navier-stokes equation, in the non-linear terms. But a bad grid generates also unsteadiness. So when you solve a problem with a steady solver you can observe oscillating results.... That's why Freeman's results are not necessarily wrong.

But how can you be sure that those oscillations are physical and not numerical ?

A second question, from a theoretical point of view, do you think that a RANS method can catch phenomena occurring in a turbulent flow with a transient mean flow?

My best regards to you.

By the way, you might have already realized that's I never said that:

"Mr. kharicha's idea of separating the flow domain in two, using the symmetry plane"

My suggestion was to create a full 2D or 3D geometry, but the mesh you use should respect the symmetry of your physical sytem....

a symmetric grid does not mean "use a symmetry plane"!!!

Please read careffully what I have written.

[Shamoon Jamshed]

I believe Freeman getting no oscillations in First order is obvious as first order scheme is the basic considering first order discretization and neglecting higher order powers of grid spacing. thus when grid spacing which is 0.00001 raise to the power of 1 it doesn't matter and can be easily adjusted in the next iteration. when it is higeher power it will get accumulated and solution revolves around a peciifc value. Thats why hihger order shcmes dont converges easily.

Kharicha and Razavan my problem is a bit similar. what i get is after certain iterations my Cl and Cd go stragith and flow also develops but residuals donot converge and fluctuates with an anplitude of 1e-2 to 5e-3. What do you say?