CFX Turbulent flow modeling Problem
 

Dear everybody,

Can anybody tell me that in CFX, for Large eddy simulation it is recommended to use Central Difference Advection Scheme.

What is the disadvantage if I use High Resolution Advection Schema with LES?

By my experience, the time steps should be smaller in Central Difference then High Resolution.

I am simulating flow dynamics in Cyclone Separator.

Thanks.

Traditional LES requires low dissipation in the numerics so the dissipation can be controlled in the sub grid model. If you use an advection scheme with upwinding it will put additional dissipation in.

But some LES approaches choose not to use a sub grid model and use a dissipative advection scheme to provide the dissipation. While this approach is a little scary because you are not controlling the dissipation, it has provided results which are just as good as the explicit sub-grid models in some occassions. I used this approach as a trial in my PhD thesis: http://hdl.handle.net/2100/248 (see Ch6).

Dear ghorrocks,

Thanks a lot.. You are helping me a lot..

Actually I used upwind scheme first, but CFX solver output file always motioned to use CDS. Then I canged upwind to CDS, but it seems for CDS, it required more memory than others. Still my simulation is running and now the file size is 308GB (Only one simulation is running)

For upwind, I did not get more realistic results.

I used LES Smagorinsky turbulent option.

Thanks a lot for your PDF thesis and I am now going through it.

I would really grateful for your helps as I am very new to CFD.

Upwinding has lots of dissipation. Way too much. Your results will be very inaccurate.

Dear ghorrocks,

Sorry for the late reply and thanks a lot.

Actually I did not apply upwind condition, I applied CDS and it allocates a huge memory even to solve up to 0.01S. Then, I decided to use data from steady state as initial conditions. Simulation is still running and but I think there is no significant memory save. :(

I am crazy about this.

LES simulations require big meshes and massive memory. That is unavoidable in this type of simulation.

Or are you saying CDS uses more memory than UDS? How much more?

yes definitely. I tried Upwind and Highresolution to same model before. Then simulation required only around 80GB capasity.

But now to simulate 0.535S time duration it has been exceeded 100GB.

May be it is due to smaller timesteps in LES upwind. But all have same number of grid points.

I tried with Upwind and High resolution for LES.

It is unusual for the advection scheme or time step size to change the memory requirement. Something must be a bit unusual in your simulation to make this occur.

dear ghorrocks,

Really??? That means something worng with my setup???

I only changed High Resolution to Central Difference..

There is possibly something wrong with you setup. It is also possible that the solver senses that CDS is going to be harder to solve and grabs extra memory. Could be either. If you have enough memory to run the larger simulation I would not worry about it too much.

But I would check your setup to make sure it is correct.

Dear ghorrocks,

Thanks a lot. I checked my setup again, but I couldn’t find any mistake.
I would be much grateful if you can check it.
Please find the attachment herewith.

Can you post just the CCL?

Dear ghorrocks,

I would be really really grateful for your helps.

Please fine the CCL file attached herewith.

Often LES is highy sensitive to the inlet conditions. I note you have just used a simple inlet velocity - in LES you often need to put a turbulence field on top of that, at least the turbulence resolved by the LES model.

Are you sure your time step size is suitable? LES is very snesitive to time step size as well. Adaptive time steps, homing in on 3-5 coeff loops per iteration is a good starting point.

Your residual target is loose. That may need to be tightened up. Do a sensitivity study to check this.

Dear ghorrocks,
Thanks a lot for your kind attention.

But please consider followings.

01. Inlet velocity: I have used Cart. Vel. Components. Here, I have used an extended inlet 600mm than the actual one, to have a fully developed steady state conditions, when it reaches to real inlet position. As your suggestion, I can use Normal velocity component. But, do both of adjustment same with extended inlet? I meant when the flow reaches to real inlet position.

02. Timesteps: I think 0.001s is sufficient and I will adjust iterations. I prefer to use a smaller timesteps. But the problem is even with this timesteps, simulation allocates a huge memory.

I am very thankful for your advices.