Hi users,, I am working in CFX 5.6 and I am simulating sloshing inside a tank. I got negative pressures in some areas in the domain and positive in other areas. I am using transient simulation and at the initialization I defined the volume fraction of water and air with the pressure. The pressure is atmosphiric in air and atmosphiric plus hydrostatic in water. In the results at zero time, the pressure was zero at the bottom and start decreasing when going up ( maximum = -16 KPa ). Why is that?? thanks in advance,,

Zaher AlHajri

By default CFX solver doesnot include the Hydrostatic pressure in the total pressure. There are definite reasons for this. I will not go into details of these now.

IN order to see the correct values you can do one of the following:

1. Add hydrostatic pressure to the pressure value while post-processing the results. You can create another variable for this purpose which is pressure+hydrostatic head

2. While specifying the Reference specific density, specify the same as zero. this will include the hydrostatic ehad in the pressure equation.

This issue will be sorted out in CFX-5.7...

Hi test,, Thanks for your reply. But you didn't tell me about the negative pressure. Why do I get negative pressure inside the domain and on the surfaces? Is that related to the velocity vectors? Thanks in advance,,,, Zaher Al-Hajri

Hi Zaher,

The negative pressures are relative to your reference pressure. Have a look at the absolute pressure in CFX-Post if this confuses you.

Regards, Glenn

Hi Glenn,, Even the absolute pressure gives me a negative pressure!!! my acceleration gravity is -9.81 because it is in the -(z)axis. Is that the reason for the negative pressure?? best regards Zaher

Hi Zaher,

Negative absolute pressure is only a problem in compressible flows, or runs where you are using absolute pressure to calculate something. If you are only running a standard incompressible simulation the absolute pressure can go negative and the simulation should still proceed OK.

What this indicates is that the fluid would cavitate (if a liquid), or has entered a region where you need to inlcude compressibility or real gas properties (if a gas).

As for how the hydrostatic pressure works, have a look at some technical tips on the CFX-Community web site.

Regards, Glenn

Hi Glenn, I am using water and air at 25 C in this run (sloshing). So Is it possible to have a negative pressure and what it does mean? sorry for repeating the question again and again. thanx in advance,,,,, Zaher

Hi Zaher,

As I said, if you are running an incompressible simulation a negative pressure does not mean anything to the solver. The solver should continue on regardless, and will probably still converge.

As the user you have to decide whether the results for the simulation are realistic. In reality negative absolute pressures are not possible as other physics starts to become important, eg cavitation.

Regards, Glenn

Your hydrostatic head is calculated as (rho - rho_ref)*g*h.

rho is the cell density and rho_ref is the reference density. It's possible, based on this formulation to get negative pressures in some areas. It doesn't mean anything as it's all relative. What's important is the delta pressures in the result.

Also, if you set an outlet or pressure boundary to something unphysical, the delta P can take some of the pressures negative. Again, it's all relative.

If you don't like the way they look in the post processor, create a new pressure variable (like P Adjusted) and set it equal to P - minval(P). All your pressures will then be positive.

Jeff

Hi Glenn and Jeff,, I don't think that my results are realistic because of that negative sign. To clarify my simulation, I will explain it step by step and sorry for my weak English. I have a tank with 2 m in length and 2 m in diameter with a baffle inside it (to be set on a truck). The baffle has two openings, one in the top and the other in the bottom. I did't draw the walls, I just draw the fluid domain. I defined the baffle as a space (I imported from Autocad). Then, I defined a mixture as my fluid ( air at 25 C and water at 25 C) with an approperiate mass fraction. After that I defined the bounding surfaces as walls and gave them a velocity with respect to time (transient) to simulate the tanker movement. However, I got that negative pressure on the baffle and even inside the domain. So do you think that my simulation is rong??? Thanx in advance and sorry for that long message,,,, Zaher

Hmmm, what you're seeing may indeed be wrong because of problem setup. In particular moving walls.

If the fluid and the tank are all in the back of a truck and moving, then the fluid and tanks are in the same reference frame with respect to each other. If truck, fluid, and walls are all moving at a constant velocity, then the walls are stationary with respect to the fluid. In the reference frame of the tank, the walls all have a zero velocity.

What the fluid "feels" is the accelleration of the truck. This will cause the fluid to slosh in the tank. This accelleration should be applied to the fluid as a body force. For example, if the system accelerates from zero to 30 mph with a constant acceleration over 10 seconds, a constant body force of 4.4 ft/s^2 should be applied to the fluid in the opposite direction of the truck motion for a duration of 10 seconds. If the truck then maintains a constant 30 mph, then the body force drops to zero.

Try it like this and see if your solution is better.

Jeff

Thanks.

[Puni1993]

Hi. Can you explain more on the pressure+hydrostatic head. I want to create it but im getting error.

[ghorrocks]

This thread is 13 years old.... all the people posting on it are long since departed, except for me

Hydrostatic head is a very basic fluid mechanics concept which is explained in any introductory fluid mechanics textbook. Have you looked at any textbook? Have you googled it?

[Puni1993]

Actually, im facing a problem in my simulation. I have a tank with a solid inside. I introduced the inflow from bottom and it will exit at the top. Supposely, the solid inside the tank should have high pressure at bottom and low pressure at top. But the pressure contour that i created showing the other way round. I already checked the setup. I dont know why its behaving like this. Any suggestion please?

[ghorrocks]

Have you read the CFX documentation regarding how it handles the hydrostatic pressure in simulations with gravity? The variable "pressure" has the hydrostatic component removed, and if you do not give it a proper reference condition it can cause the pressure to do strange things with height.

[Puni1993]

Thank you so much. The problem is in my reference pressure. Once I change it, now it fine.