[fivos]

Hi to everyone,

I am trying to simulate the flow inside a Diesel injector. An indicative view of the area of interest to be simulated with CFX is shown in the attached - the greyed part is the area where fluid is flowing. The geometry is axis-symmetric, with the exception of the holes; there are 6 holes in the injector, every 60deg. The length scale of this image is of the order of several mm (the hole diameter is ~200μm). At the inlet the injector has a pressure of 2500bar and at the outlet 20bar. Normally the needle is moving up-down, but for now this is ignored, since it is only going to make things more complicated...

The complexities here are:
a) due to extreme pressure difference, Diesel cannot be considered incompressible. There is significant variation of its density that causes some side effects (cooling due to the depressurization). I have a library for Diesel properties implemented as expressions in CFX for all properties (density, heat capacity, conductivity etc..).
b) inside the injector and at the injector hole there are very large velocities, more than 500m/s, and large accelerations so in practice cavitation occurs. Moreover, since the speed of sound of the vapour is less that the velocities occurring inside the injector, the vapour should be considered compressible (ideal gas).

I have tried the following, with increasing complexity:
a) simulated single phase incompressible flow. It went fine, easily converged.
b) the results from the above simulation were used for a single phase compressible liquid Diesel simulation. For heat transfer the total energy model has been used, in order to take into account both variations of enthalpy and kinetic energy. The simulation worked fine, results have been checked in respect to simple 0D thermodynamic calculations (energy conservation) and mass conservation with less that 0.5% error.
c) Simulation (b) was used as an initial condition for simulating cavitating Diesel. Diesel was assumed compressible, but vapour incompressible, with total energy model. This simulation also went fine.
d) Simulation (c) was used as an initial condition for simulating cavitating Diesel, with all phases compressible with total energy model. I cannot make this simulation converge despite having tried a lot of things such as:
- lowering the physical timescale to very low values e.g. 10^-10s
- enabling high-speed numerics
- setting the volume fraction coupling to Coupled (generally I found that it is more stable than the segregated, but still blows up after some time)
- reduced the cavitation rate URF
- increased the max-continuity loops to 2 rather than 1.

Always, at some point, I get problems with the convergence; some value gets outside bounds.

I understand that this is probably one of the toughest simulations, since it involves two compressible phases at transonic Mach for the gas phase and very high Mach for the mixture (the mixture Mach may reach 60 or more..). I want to know if anyone else has tried something similar with CFX and any suggestions on the solver settings to get a convergent solution.

Thanks in advance
Fivos.

[ghorrocks]

Yes, this is a very complex model. Good to see you have taken a step by step approach to get there - you would be completely lost without it.

I would have a look at the compressible cavitation model but on a simpler geometry. This will give you an idea whether mesh quality is something you should look at.

I would also contact ANSYS support on this, I suspect there will be some undocumented stuff which might assist.

[fivos]

Thanks Glenn for your reply, I was planning on contacting CFX support for some feedback on that anyway..

[krapic]

Hi fivos,

I am currently running the same case as you did and I'm encountering the same problem - it is impossible to get to a converged solution with two compressible phases. Did you manage to get a good solution and could you share some advice on it?

Regards,
Kristijan

[fivos]

Hi Kristijan,

No, I have not managed to run successfully a case with both compressible liquid and vapour with cavitation enabled in CFX. A colleague of mine has managed to run high lifts operation in steady state only (no needle motion), after playing a lot with the relaxation factors at the expert section (he has discussed that with ANSYS support and they suggested him to do so). Unfortunately, these tricks were not successful at low lifts and they are not suggested for transient simulations as well. Eventually we had to resort to the vapour being incompressible..

However, I have to mention here that treating the vapour phase as incompressible is not a very incorrect assumption. The reason is that if you assume you have thermodynamic equilibrium, then cavitation zones should be at vapour pressure, thus the density of vapour is approximately constant. Compressibility of the mixture is represented with the mass transfer, so the mixture behaviour is reasonably accurate. The problem with this treatment is if you have large and well defined cavitation structures, where you might end up with pure vapour; at that point the mixture is no longer compressible since you end up with a pure incompressible phase. In any case, I think this is a compromise one has to live with..

After my work on this subject, it is apparent for me that such flows are somewhat beyond the current capabilities of the software and, I am afraid, beyond the current state of the art of CFD. Even in research papers I have not seen proper representation of the thermodynamics of all phases; if compressibility is examined, the liquid is treated as stiffened gas at most (which is a simplistic linear relation like the ideal gas, with many known deficiencies) ..

I wish you good luck.
Fivos