[Bisht]

Hi I am simulating a multiphase problem on fuel tank filling process. with VOF method
I have pressure sensor experimental value which is located at the top of the fuel tank surface. As flow starts, pressure remains zero in tank for a time period of 0.2 s and than starts increasing because of compression of air inside the tank.
But during simulation, pressure is kept fluctuating between 250 to 500 pascal for the whole time period from the starting point.

I am taking pressure outlet and mass flow inlet. Initial condition and boundary condition is zero pascal with reference pressure of 101325 pa.

Please find the attached images of the pressure graph.
Why simulation value is so different from experimental result?

[me3840]

This could just be noise in the numerics, those are really small pressure values. I would ensure:
1. Your CFL is good during the run
2. Your timesteps are converging
3. Your timestep is small enough
and you can consider running double-precision.

[Bisht]

Hi, thanks for your suggestion.

I tried it with finer mesh also and a smaller time step but still the minimun pressure value I am getting during my simulation as 170 Pascal which is certainly very wayward to the experimental minimal value of the Pascal. As you can see in previous attachment maximum experimental value is increasing continuously to 1400 Pascal because of the compression of air but in simulation I can't see this effect.

I am using double precision for my simulation.

[kirrer]

I'm not quite sure of the boundaries and/or the assumption that air is compressing. If you have a pressure outlet, this should prevent air from compressing as it can leave the control volume. On the other hand, if you have compressing air, you cannot have a pressure outlet. Are you able to share a rough schematic of your tank?

[devesh.baghel]

Hi Kamal,

1. Is your test model and simulation model stand at same plateform while start of filling of tank i.e. empty tank or prefilled in both test and simulation ?

2. Are you modeling carbon canister into your simulation ? also outlet is just air vent defined as pressure outlet ?

3. If you have smooth air out with empty tank, dome will not experience pressure at initial time-steps as shown in test results.


Regards
Devesh

[Bisht]

Hello,

Air is compressing in the tank domain because outlet is not big enough to let all the air escape from domain.

I have done experimental test with empty tank and for simulation also I am considering tank to be empty.

Yes Outlet is defined as pressure outlet with volume fraction of air as one and fuel as zero. Inlet is a mass flow inlet with fuel volume fraction as one and air as zero. Intitial condition and pressure outlet is at zero pascal relative pressure, environmental pressure 1 bar.

Please find my domain geometry in the atthment for your reference.

[triple_r]

Are you using ideal gas law or real gas law for air? or are you assuming the air to be incompressible (constant density)?

[Bisht]

I am using constant density Model for both air and fuel (which has same density as of water).

[triple_r]

If you want to model air pressure correctly, then you need to use at least the ideal gas law for air.

By definition, an incompressible fluid (constant density) has to have the same mass flow rate in the inlet and outlet boundaries of the solution domain. So, any pressure difference from inlet to outlet is due to velocity differences and/or viscous effects. So, the phenomenon that you mention: "air is being compressed in the tank as it cannot escape fast enough" cannot be modeled by an incompressible fluid model.

[Bisht]

Oh I see... But isn't Reynolds no. has to be above a specific value to use ideal gas model? I am not using any temperature model for my simulation as it doesn't effect the fluid property but is it same for ideal gas?

Actually I want to simulate the filling process of tank for the first 1s. In that time air is not compressed and leave the domain as desired. But as you can see in previous attachment of the geometry that after sometime air outlet pipe hose is filled with the fuel and then this compression of air phenomenon comes in to effect.

But I am more concerned about the first second of simulation.

[triple_r]

It usually depends on the Mach number, and by rule of thumb, if Mach number is larger than 0.3 you should use compressible fluid. However, if the physics needs compressibility, no matter what Mach number, you should use a compressible fluid.

With regards to temperature, you can still have a constant temperature (isothermal) flow, but that doesn't mean density in constant, as in gases density is a strong function of pressure as well.

I don't know about the duration, but if we look at the extreme case where there is no outlets, just one inlet for air. Then, even a very small velocity (mass flow) at inlet will cause the problem to be ill-posed when using incompressible fluid. That is just how the math works out with continuity. In your case there is an outlet, so it is not as extreme as this limiting case, but this might cause instability in solution.