[Martin121]

Hello,

I want to simulate an array of 9 jets (diameter 0.8 mm, velocity: 0.2 m/s, oxygen) issuing into a counterflow (velocity 0.02 m/s, CO2). The inlet of the counterflow is in the top left-hand corner, the outlet is at the lower right-hand corner. The sidewalls are periodic.

The Reynoldsnumber is rather low, about 12 for the inlet tubes. Do I need to use a turbulence model? Which would be the best one. And which model constants should I use? I observed differences for the stagnation point for different models. The Reynolds number is low, but I think there is still some turbulence and streamline curvature involved, especially in the mixing layer.

Thanks for your help!

[fluid23]

Large Eddy Simulation.

[Martin121]

I think large eddy simulation is beyond my available computation power. I calculate on a 4 processor desktop computer using Ansys Fluent.

The numerically predicted stagnation point is nearer to the injection point than the experimentally meassured. What justified changes can I make to the turbulence model to move the numerical stagnation point further away?

[fluid23]

Yes probably so...

I would maybe go with SST (a form of k-w).

[fluid23]

I am not sure I would look to change the turbulence model in any significant way.

If you have experimental data you can see which one gets you closer, but unless you have a very good understanding of how the changing constants will affect your model I wouldn't play around too much. You may cause more problems than you solve.

[FMDenaro]

Originally Posted by Martin121

I think large eddy simulation is beyond my available computation power. I calculate on a 4 processor desktop computer using Ansys Fluent.

The numerically predicted stagnation point is nearer to the injection point than the experimentally meassured. What justified changes can I make to the turbulence model to move the numerical stagnation point further away?

on your 4-processor system, what is the finest grid you can use? This case seems resolvable in DNS ...

[Martin121]

Originally Posted by MBdonCFD

I am not sure I would look to change the turbulence model in any significant way.

If you have experimental data you can see which one gets you closer, but unless you have a very good understanding of how the changing constants will affect your model I wouldn't play around too much. You may cause more problems than you solve.

I know...I just think that the cases the model was callibrated with might be far away from my 0.8 mm jet I use the model for.

What do you think about a Reynolds number of 12? Normally that would mean no turbulence?

Reynolds-stress Models opposed to others do account for streamline curvature right? I think this is important in my simulation, as the streamlines for the jets are bend by 180°. That's why I tried them at first.

If I use k-w SST the streamline curvature would not be taken into account - so even if I got closer to the experimental data I would neglect an important physical phenomenon.

[fluid23]

Turbulence is always a part of the flow at some scale. Plus the boundary layer of the jet is going to mix as it diffuses and that mechanism (if I recall properly) was turbulent mixing.

SST isn't the best choice by anyone's measure. It will be better than k-e and standard k-w but it is known to over predict turbulence in high gradient regions (so near stagnation). What options do you actually have available to you?


FMDenaro, please correct me if I am wrong, but if LES isn't an option due to resource availability DNS should be off the table as well, no? DNS requires resolution of all length scales and is even more computationally expensive than LES, or so I thought.

[fluid23]

Also, is my understanding of SST flawed? I thought it was formulated to do a better job with curved flow than traditional k-w. Do I have that backwards?

[FMDenaro]

Originally Posted by MBdonCFD

Turbulence is always a part of the flow at some scale. Plus the boundary layer of the jet is going to mix as it diffuses and that mechanism (if I recall properly) was turbulent mixing.

SST isn't the best choice by anyone's measure. It will be better than k-e and standard k-w but it is known to over predict turbulence in high gradient regions (so near stagnation). What options do you actually have available to you?


FMDenaro, please correct me if I am wrong, but if LES isn't an option due to resource availability DNS should be off the table as well, no? DNS requires resolution of all length scales and is even more computationally expensive than LES, or so I thought.

indeed I asked for the finest grid you can use...Re=12 at the inlet is small, 4-processor system should be able to solve grids number O(10^6)

[sbaffini]

If your Re is really 12, no matter what, any turbulence model is gonna give you garbage. It simply seems a laminar unsteady flow, there would no reason to simulate it as turbulent.

This, obviously, doesn't mean that the simulation is feasible...

[Martin121]

Originally Posted by sbaffini

If your Re is really 12, no matter what, any turbulence model is gonna give you garbage. It simply seems a laminar unsteady flow, there would no reason to simulate it as turbulent.

This, obviously, doesn't mean that the simulation is feasible...

So you mean I should try to simulate it as an unsteady laminar flow without any turbulence model? The Reynolds number is calculated using the tube diameter of 0.8 mm. Is this the right reference for this case?

[Martin121]

Originally Posted by FMDenaro

indeed I asked for the finest grid you can use...Re=12 at the inlet is small, 4-processor system should be able to solve grids number O(10^6)

At the moment the grid has 515000 nodes with 5e-5 as the smallest element size.

I started an LES. I'll see wether it converges in a reasonable time

[Martin121]

Originally Posted by MBdonCFD

Also, is my understanding of SST flawed? I thought it was formulated to do a better job with curved flow than traditional k-w. Do I have that backwards?

SST is some kind of a mixture between k omega and k epsilon. k omega near the wall and k epsilon in the free stream. All are first moment closures, meaning that according to the Bousinesqu hypothesis the Reynolds stress tensor is proportional to the mean strain rate....I thought as I have a reverted flow with a more complicated flow field I should take the Reynolds stress model.

[Martin121]

Originally Posted by MBdonCFD

Turbulence is always a part of the flow at some scale. Plus the boundary layer of the jet is going to mix as it diffuses and that mechanism (if I recall properly) was turbulent mixing.

SST isn't the best choice by anyone's measure. It will be better than k-e and standard k-w but it is known to over predict turbulence in high gradient regions (so near stagnation). What options do you actually have available to you?

I have a Desktop computer, 4 processor and Ansys 15 Workbench as available options.

[sbaffini]

Sorry, but this post got lost and i couldn't see it anymore.

Yes, i mean "to simulate it as an unsteady laminar flow without any turbulence model", exactly. Which, you should be aware, is nothing different from DNS. Just that, in this case, there should be no inertial range... that is, your solution stays (mostly) "calm".

The fact about RANS/URANS is that they assume the flow to be turbulent, fully turbulent. Which is not your case, at all (yes, inlet diameter and mean velocity should be the relevant parameters for the Re number). A more complicated model (e.g., Reynolds stress) does not add anything to this.

In 2009 i could run 1Mln cells on the four cores of a Q6600 processor for enough time to do time statistics on a synthetic jet case (8 cycles, LES)... still, the job took 1 month. According to your processor, cache, RAM, code, you might be quite above that number.