For a high Reynolds Number (in the order of 10^8) incompressible (steady) flow problem, I have used different decritisation schemes - 1st order Upwind, 2nd order Upwind and QUICK. I am surprised that 1st order upwind scheme is giving more accurate result in terms of drag when validated against experimental results. As higher order upwind schemes are supposed to be more accurate, the result is bit confussing to me. The trend of result is consistant and compared with number of experimental results.

I understand, by default, fluent uses central difference scheme for defussive fluxes and the scheme user chooses is applied for convective fluxes.

Experts may please comment and advise.

Hey, Sorry i am not an expert of discretization scheme but I could give you an opinion. By default I never use the 2nd order upwind scheme (not well developped in fluent). Then I do think that the Quick scheme cannot be applied to every type of mesh. You should check on the Fluent online-documentation if your mesh fits to a quick scheme use.

Hope this help. thomas

I don't think it's a problem of implementation, maybe of stability. Also, as said in the manual, the second order discretization scheme is implemented in order to reduce numerical diffusion, so it should improve accuracy.

However, the QUICK scheme implemented in FLUENT can be used on all kinds of grids (structured and unstructured). It's more accurate on structured grids, if they are aligned with the flow direction.

If you have an unstructured grid or a hybrid one, FLUENT applies the second order discretization scheme at the faces of non hexahedral cells.

First order is suitable only in simple cases, with grids aligned with flows. But if the flow doesn't follow this behaviour, second or higher order schemes should give better results.

Try doing a calculation using first order (you can use the one you've already done). When converged switch to second order scheme to see what happens.

Hi

ap

I agree with ap. I believe from my experince the 2nd order scheme should give better results. What turbulence model are you using? this will also change your results considerably.

Thanks Mr Thomas. My mesh is aligned to flow and fluent on line documentation says that 1st order upwind can be used for this type of mesh.

My problem is when I use second order upwind or QUICK for the same problem (same mesh), my results deviate from experimental results. I am unable to understand why 1st order upwind scheme is giving better result than 2nd order.

Das

I have used k-e (all three standard, RNG and realizable), k-w and RSM models. Except k-w all the models have given similar results.

In all the instances, when I use 2nd order upwind scheme my results starts deviating from experimental results.( Results with 1st order upwind scheme is close to experimental findings).

I am using a structured grid aligned to flow. It is a convection dominated flow, Reynold's No is very high. Das

General speeking results from 1st order scheems must be the same as from 2nd order scheems when you have an infinite fine mesh.

From this it is clear that a coarser mesh will give different results using different discretisation scheems if the solution is mesh-dependent.

So before looking into turbulence models you should try to obtain a mesh independent solution. Using a 2nd order scheme, you will reach this state on a coarser mesh compared to a 1st order scheme.

If you have access to solution dependent mesh refinement this feature will help you saving elements.

If a finer mesh brings you into trouble regarding the validity of your turbulence model (i.e. y+ gets too small) you have of course to use an appropriate turbulene model which can handle high resolution grids.

Hi Helge, Do you know how to get mesh independent solution? Thanks. Zwdi

A solution is said to be grid independent if a further refinement of the grid doesn't implicate a change in the solution.

So, to obtain a grid independent solution, you have to refine your grid until the solution stops to change in consequence of grid refinements.

Hi

ap

Thanks.Is mesh independent solution equal to true solution? Thanks again. Zwdi

Hi Helge, As you said, "If a finer mesh brings you into trouble regarding the validity of your turbulence model (i.e. y+ gets too small) you have of course to use an appropriate turbulene model which can handle high resolution grids". Could you give me guides which kind of turbulence model efficiently handle high resolution grids? Thanks. Zwdi

Just check turbulence models limitations in FLUENT manual.

For example, if you adopt k-eps models with wall-functions, y+ have to be between 30 and 60. So you can't refine your grid too much in order to respect that condition.

Hi

ap

The grid-independent solution is just the solution you obtain when your space discretization doesn't influence the solution anymore.

This doesn't mean it's the physical solution of your problem.

Hi

ap

Turbulence Models are not spesific to resolution of grid. I mean, a same turbulence model can be used for a coarse mesh or a fine mesh. You have to look for an appropriate WALL FUNCTION to match with your resolution (in terms of y+). For example, standard wall function works well within a range of y+ between 30 to hundred. Any wall function, based on log law, is suitable for that y+ range. For mesh of higher resolution ( Y+ < 5), you can use two layered wall function like enhenced wall treatment.

You can also use turbulence model like, v2f, to avoid use of turbulence model. I hope this info may be useful for you.

Das

Thanks. I could not find v2f model available in the VISCOUS list. Do you know how to make it work by using text commands in Fluent? Zwdi

I have never used v2f model while working with fluent. As far as I know, Fluent 6.0 does not contain this model. You have to ask support group of fluent, if it is available with any of Fluent version.

I would recommend the SST model. It blends the k-e with a k-w model near the wall. The k-w behaves well on fine grids (y+ around or below 1). The normal k-e low reynolds model from my experience converges very slow.

Hi Helge, I tried SST before. But there are many large shoots and vibration during converge process. Could you give me good suggestions about using SST model? So that I can made solution smoothly converged. Thanks a lot. Zwdi