Hi all

I am using the Detached Eddy Simulation model for predicting the three-dimensional flow field of a round jet in crossflow. The velocity range is from 15-20 m/s and the domain dimensions are 0.75x0.3x0.3 m. I am using a relatively coarse grid of about 90000 nodes, because the simulation is done on a PC. The unsteady parameters that I have used are:

Time Step Size: 0.0001 No. of Time Steps: 1000 No. of Iterations per Time Step: 20

I have compared the mean results of the DES and results from steady RANS based simulation using standard k-epsilon model against experimental data, and I found that the steady k-epsilon simulation results are slightly in better agreement with the measurements; however both methods highly over-predicted the velocity profiles (with an error of about 250% for the wall-normal velocity).

I would like to know, whether this model (DES) is appropriate for my case and could I get better results by using smaller time step?

Thanks a lot. Maged

DES uses a automatic grid-dependent switch between RANS and LES-mode. Consequently you will have a RANS simulation if your grid is too coarse. From this point of view it is not surpirsing that you get similiar results.

If your code provides this feature you should have a look on the controlling functions.

A couple of decades ago I also performed a range of simulations of jets in cross flows. These were holes through casings rather than straight tubes venting into a chamber. The interest was in discharge coefficients, pressure drop and passive scalar transport. If I recall correctly:

* grid resolution was important particularly in resolving the flow through the hole and the formation of the vena contracta.

* eddy viscosity models could go horrendously wrong and generate enormous spurious turbulent viscosity through the hole. This was due to large (incorrect) generation due to normal rates of strain and not shear. An LES simulation is not going to suffer from this. Personally I would avoid DES unless properly formulated.

* the penetration of the jet was pretty insensitive to everything being determined by a gross momentum balance.

* the transport/mixing of a passive scalar was sensitive to numerical errors and turbulence model failings.

I do not understand what you are describing as going wrong. How can a wall have something other than zero as a normal velocity? What is driving your jets if you can see 250% differences in velocity?

Thank you so much for your valuable comments.

What I meant by wall-normal velocity is the velocity component in the direction normal to the wall (normal to the crossflow also) not the velocity at the wall. In my case, the positive y-axis is the direction of the jet and the positive x-axis is the direction of the crossflow. So what i meant is that the profile of the velocity component in the y-direction has a very large error.

In fact, I have found only one study in the literature that uses DES for jet in crossflow. But they have used a very fine mesh of about 2100000 cells. Their simulation on 64 parallel processors took about 4000 hrs (~166 days!!). For my case I am using a single Pentium 4 processor with 1 Giga RAM memory. So it may take something like three years or more to perform such a simulation. (I am just an MSc student

I would just like to know: What is the minimum possible grid size and maximum possible time step that I can use and still get results with reasonable accuracy?

Thanks again for your help. Best Regards. Maged

P.S: I will be so grateful, if you can send me any scientific papers that study jets-in-crossflow numerically.

The trajectory of the jet is almost impossible to get wrong because it is determined by the relative momentum of the two streams. Is the inviscid core of your simulated jet in the same place as the measurements? If not, you have something grossly wrong in your boundary conditions or the properties of the two streams. I would sort this first before optimising your grid distribution or choice of turbulence model.

4000 CPU hours is about 2.5 days which is reasonable for an unsteady simulation. 2 million grid points is also a typical size possibly a bit small but it depends what is being resolved.

The time step and grid size are determined by the effect of the numerical errors in the simulation. The accuracy of the overall simulation will also be influenced by the assumptions in your turbulence model. If the numerical errors are large they are likely to swamp the differences in the turbulence models leading to erroneous conclusions (very common in CFD).

If I was performing the task I think you are performing I would first perform a RANS ke simulation and a RANS laminar solution to get a feel for the influence of the turbulence model in the presence of the numerical errors. Then repeat using half the grid resolution (1/8th the number of grid points) to get a feel for the size of the numerical error. This will help put any differences using DES in perspective.