[Sadd]

Hello foamers,

currently I'm trying to simulate a super-sonic jet in (near) vacuum. The application is a gas target in an heavy ion accelerator. I'm interested in what density distribution the ion beam sees. I do not aim for perfect reproduction of reality, but to get a general gist of it, as the density in the accelerator is not easily measured. Later on the simulation should get more sophisticated of course (geometry and so on). I want to focus now to get the simulation stable with realistic parameters and go for more accurate schemes, models, and so on later.

If anyone has already general advice on how to simulate such a setup I would appreciate it very much. Below I will describe more detailed my current problem/situation.

So my domain looks like this:



Bottom is a symmetry plane, right and top are outlets, left bottom is the inlet, otherwise left is a wall. It's 2D (front and back are empty).

For now I have chosen the sonicFoam solver with laminar turbulence model.

My boundary conditions are mainly
p: fixedGradient inlet, wavetransmissive outlet
u: pressureinletVelocity inlet, zeroGradient outlet
T: fixedGradient inlet, zeroGradient outlet

FvSchemes are mainly linear or first order schemes.

I think the main problem in my simulation are the high pressure gradients (up to ~10MPa at the inlet, vacuum something like ~1Pa), so I was trying to increase the inlet pressure slowly from run to run and see what resolutions (dt,dx) I need to increase or which problems pop up.

What I observe in my latest run is that the simulation runs fine (no errors), but the calculated pressure just "freezes" at some point. It looks like this



and for some reason doesn't advance further. So why is that? What do I have to focus on to get my simulations stable?

Finally some of my questions are:

1. Is the solver fine or should I use a different one?
2. Are my boundary conditions in principle fine?
3. Should I focus and using different fvSchemes?
4. I don't really get the "normalized" gas. Yes I know sonic speed 1 m/s and so on, but how would I relate that to real gas parameters?

I'm currently running a simulation with higher resolution (takes quite a while already though) to see if that helps.

Thank you very much in advance for any advice.


EDIT: Btw while there are some posts I found on similar topics, they didn't help me too much. I tried using the knowledge given there and basically got to the results above.

[mkraposhin]

Hi, i'm interested in testing my compressible solver. If you will share your case data with me, i can try to run it

[Sadd]

Originally Posted by mkraposhin

Hi, i'm interested in testing my compressible solver. If you will share your case data with me, i can try to run it

Hello,

thank you for the answer. Sure I can share my case data with you. However, it is not a realistic case as I'm currently still trying to figure out OpenFOAM, stability, typical errors etc. What kind of solver are you working on?


Below I summarized some points I learned in the past week. These focus mainly on simulation of high pressure gas injection into near vacuum. Hopefully this helps people running into the same problems. Forgive me (and correct me) if I'm wrong. I'm nowhere near my goal in terms of knowledge and results.

• Can't reproduce the error I got above. So forget it...
• A good book for CFD is Ferziger J.H., Peric M.: Computational methods for fluid dynamics. It's not perfect but up to now the most helpful on the basics. But I wish there was a book which gave some basic guidelines which methods to use ("When you have problem X, try ansatz Y first because ..." "If instability occurs due to A, try B to do C because ...").
• Crashes in my runs are usually due to pressures/densities < 0 which show as "FOAM FATAL ERROR: Maximum number of iterations exceeded" of thermoI.H. This is caused by high pressure/density gradients in shocks and the pressure then "undershooting" in the low pressure region.
• Simulations can quite easily be made stable when using "upwind" schemes everywhere, even with turbulence models. However, this is very dissipative ("diffusive", "washed out" you might call it) so results are not so nice.
• I tried a lot of better schemes (TVD, etc.). The only one not crashing beside "upwind" is "limitedLinear 1" (1 can be usually smaller than 1, but not close to 0). This produces "shaper" results. Not sure what "limitedlinear" actually does different to all other schemes so it's not getting p<0 even though it's TVD as well.
• For sonicFoam try using higher nCorrectors (3 or 4). Often helps a lot against crashes.
• Increasing mesh and temporal resolution (beyond something like Co = 0.5) often has only minor effects. However, this might be a wrong for even higher resolutions than I tried, but my "best" 2D simulation takes already a night.
• Ramping inlet pressure helps sometimes against crashes (-> lower gradients).
• Density based solvers are supposed to be better - in principle - in resolving shocks and high Mach number flows (like in my case) than pressure based solvers. So in principle rhoCentralFoam is more suited than sonicFoam. Weird though that the name and description of the latter implies something else... In openFOAM-extend there solvers called "rhoSonicFoam" or similar, but there is even less documentation on them than for the standard solvers.
• Both rhoCentralFoam and sonicFoam have similar stability for me, but produce quite different results. Given the above I trust rhoCentralFoam more and use it as my "main" solver for now.
• All (I think) solvers in OpenFOAM are segregated solvers (meaning velocity/pressure/density are solved separately, not in one matrix). Other kind would be coupled solvers. For steady-state simulations there are some guidelines when and why each one of them is a better choice. There is no really conclusive information for transient simulations. Coupled solvers are most likely better but not easily implemented in OpenFOAM due to limited flexibility of the matrix format in OpenFOAM.
• There are some extensions to solvers or better solvers out there (like in OpenFOAM-extend), but I couldn't really figure out too much for now. I'm guessing that something like a density based coupled solver with AUSM, RK4, LES (just to mention some keywords) would be the best models for my problems, however until I have more conclusive information I'm kinda hesitant diving into implementing a solver...
• LES simulations should be full 3D (no wedge symmetry!). Did not test this however.

Cheers

Oli

[chirag]

Hi mkraposhin,
Thank you for your attemp to look into the testing of the solver.
I have uploaded my case file and I am simulating it in pisoCentralFoam developed by you.
The solver produces unrealistic results near the shock wave region.
Can you please look into it. I have generated the geometry exactly similar to the experiments and validated it using fluent.
"Stationary supersonic plasma expansion: continuum fluid mechanics versus direct simulationMonte Carlo method" by S E Selezneva et.al. 2002 J. Phys. D: Appl. Phys. 35 1362
I have uploaded the case file here describing the error observed.
I have also attached the small modification done for rho and P for avoiding negative pressure value and hence divergence of simulation.
http://www.cfd-online.com/Forums/ope...ntralfoam.html

I have uploaded the final data file to after simulation was completed in the below link
in google drive: https://drive.google.com/file/d/0B5_...ew?usp=sharing

Thank you,
Chirag

[chirag]

I will also share the fluent files if required which will help in the complete validation with commercial and openfoam.
I have validated the case with both steady and unsteady simulation using both pressure and density based solver.