OpenFOAM supersonic Nozzle rhoCentralFoam
 

Hi.

I am simulating the flow inside and at the exit of a supersonic nozzle (convergent followed by a long straight tube - no divergent) using rhoCentralFoam.

My inlet BC is totalPressure = 5.00bar and the oulet BC is waveTransmissive = 1.01bar.
To take advantage of the geometry, I am solving the flow with axisymmetric BC. My domain is then a simple wedge - of less than 5°.
rhoCentralFoam is used as a density-based solver and the turbulent model used here is k-omega SST.

The issue I have is that the simulation evolves a lot between the first iterations, the iterations in the middle and the last iteration. Of course, I know rhoCentralFoam is a transient solver, but my system should be steady, when the right regime is reached. The solution I get seems to give me pretty good results according to experimental results at step 2000 but the solution at final step 38600 is far from the experimental results.

I attached figures showing the pressure gradient at step 2000 and step 38600 as well as the "numerical schlieren" and my experimental schlieren results.

Does anyone have a clue ?

Best

*pressure field
not "pressure gradient"

Any thoughts ?
 

Has anyone any idea by any chance ?

I would try first without any viscosity, Euler equations.

Also I don't know precisely what is behind the outlet bc you use, but if flow is mostly supersonic there I would give a shot to a supersonic bc, which is basically an extrapolation of all interior variables, e.g. all waves going out of the domain. If your outlet is not truly transmissive it will reflect waves and spoil the shape of the jet. Alternatively you can try to increase the size of the "receiver", e.g. place the outlet further away from the jet and use bigger cells close to the outlet to damp spurious waves.

Thanks for your insight, I will follow your recommandations.

What do you mean by supersonic bc? Do you mean 'supersonicFreestream'?

What do you mean with "iteration"? It is a transient solver. So we are talking about timesteps, time-step-size, countant-numbers ....

Yeah yeah, sorry. I meant time-step.
I was mistaken because my solution should be steady (solver should converge towards a steady solution) but the solver is transient.
Thanks

Here you have an example with a "subsonicSupersonicPressureOutlet". It was used for the following paper:


https://ieeexplore.ieee.org/document/8636345

We used rhoPimpleCentralFOAM from:

https://github.com/unicfdlab/hybridCentralSolvers

and the libcompressibleTools (contains this BC) from:

https://github.com/unicfdlab/libcompressibleTools


It was done with OF4.0. I did not check with a new version.

Would you verify that the solution at 38000 is still supersonic near the dump? Do you have a train of curved bow shocks or did the solution revert back to a subsonic solution? If subsonic then we need to steer the solution towards the supersonic case. If you have bow shocks then we need to think whether it is just an issue of discretization or the BCs needing to be adjusted to get the overexpanded jet which will give you the shock diamonds you are looking for (i.e. increase or lower the back pressure).

It might be easier to visualize if you plot density or Mach number instead of the pressure. Obviously plotting the Mach number would directly answer my question. Pressure is fine too but you have to really zoom in to see the gradient and then do the logic in your head.

The problem might be the waveTransmissive BC. There is a parameter "lInf" which specifies a virtual length, which is added to the outlet, where the pressure has its specified value. If you don't explicitly set the value of "lInf" to something meaningful, it is assumed to be very large (infinity ??) and your solution is very stable but wrong.