I am a PhD student measuring and modelling the pressure decline in a tank due to air leakage.

My Fluent model of the tank is a realy simple 2D model. The tank is pressurised to a 100 Pa gauge pressure with the operating pressure set at 101325 Pa. This is done for steady state. When the pressure is uniform in the tank I start the transient solution. Due to air leakage the pressure in the tank will decline.

However, the pressure decline and the mass flow rate out of the tank is not consistent with each other. The pressure decline is about 40 percent larger than what it should be according to the ideal gas law. For example, the tank volume is 1 cubic meter, the temperature 295 Kelvin and the pressure decline from one time step (0.002 sec) to the next is 0.56 Pa. At the same time the mass flow rate out of the tank is 4.72 e-6 kg. This change in mass inside the tank should only result in a pressure drop of 0.4 Pa.

I wonder if anyone has encountered this type of problem? I have tried very short time steps, a large number of iterations, different numerical solvers, turbulence and laminar models, coupled and segregated solvers and so on. But all choices give the same results, that is a discrepancy of about 40 percent between pressure drop and the pressure drop calculated by hand according to the ideal gas law.

A couple things... when you calculate what the pressure drop should be, are you getting the new temperature in the tank (since you're using ideal gas law and all...). Also, I'm not sure how you calculated the pressure drop in fluent, but I'm thinking you should be doing a mass-weighted average (since there will be less mass near the leak than at the other end of the tank). One thing you could try would be to open the valve for a certain amount of time and monitor how much flow has left and the mass weighted average of total pressure. Then close the valve and allow it to reach a steady state condition (this way with the fluid not moving, your static pressure = total pressure).

Hope something here was useful. Goodluck, Jason

Make sure you are measuring the pressure in the right area. near the exit, the static pressure will be lower due to the dynamic head. Far away, say near the top of the tank, the dynamic pressure should be insignificant. If the pressure drop is still inconsistant, check the mass holdup of the tank and make sure it is consistant with the mass released. An error in the pressure would indicate that Fluent is not conserving mass.

-Robin

Jason and Robin,

Thank you for your replies. I have checked the change in density in the "tank" and hand calculated the corresponding change in pressure. The simulations that I am performing are of very small air leakage rates and the air velocity is less that 0.1 m/s anywhere in the "tank".

After stopping the air flow out of the tank and simulating for another 0.01 seconds there are no air movements in the tank. The change in density when air is leaking out during 0.02 seconds is â€" 4.8 e-5 kg/cubic meters. This is equivalent of a pressure change of â€" 4.06 Pa. However, the change according to Fluent is â€" 5.69 Pa. That is, the pressure drop is about 40 percent larger than it should be.

Is this due to some kind of round of error in Fluent, when simulating such small quantities?

If you can think of anything else that I am doing wrong, please tell me.

Best regards

Björn

Where are you measuring your pressure, or how are you calculating the pressure in Fluent at the different time steps?

Ideal Gas Law is P=rho*R*T... a .001% change in temp (which is only .00295K) can create a .001% change in P (which for 101425Pa is ~1Pa, which is about how much your pressure if off). Check the temperature changes in your tank as well to make sure you're using the right values when calculating the pressure drop.

It's possible that there is round off error. Gambit always works in absolute quantities, so when you break it down to the difference between two computations, this could make the error look much larger. Being off 1.6Pa with an absolute pressure of 101425 is only an error for the calculation of about 1.5% which is possible. Higher order discretization schemes, and improved mesh may help lower this error.

Thanks, Jason

You are using a 2D model right,but the mass flow rate calculations needs area, if you have not changed the reference depth Fluent take it to be 1.0 M