Hello,

I want to model a flow around a plate (Length 100mm and width 3mm) in a domain (Length 1000mm, and width400 mm). As a boundary conditions, I put a velocity inlet and mass outflow. and I kept the operating pressure as atmospheric pressure.

For low velocities (1m/s, 3 m/s), the results seem to be good but for higher inlet velocities (8m/s) I got NEGATIVE absolute pressure??? can someone help me with this????

Thanking you in advance .

Tania.

Hi;

-What's your fluid material? If your fluid is water, in the case of cavitating flow if you turn off the cavitation option you may get negative absolut pressure.

-The outflow B.C. must be in the location of zero gradient. If the location of this B.C. do not have this condition, Fluent forces this condition and wrong results is obtainable. I think that this is your mistak!

Regards

ROOZBEH

Hi again;

What I tell you in the last message is two different mistakes that can be done.

Regards

ROOZBEGH

Hi,

Thanks for your answer. But I must admit that I didn't understand your second Point ???

the fluid is water. when I got absolute negative pressure, I thought if I make computations with the cavitation model ON, cavitation will appear. But I got some Error message (pressure correction) and the computations stopped.

Actually my aim when I increased the velocity inlet (8m/S) is to get low pressures (lower than the vapour pressure) in order to simulate cavitating vortices. but not negative absolute pressure!!!!

Hi!

Try it with pressure outlet b.c.

Your operating pressure should be about a half of the sistem pressure (what you measure at experiments), the other half should be defined as gauge presssure at pressure outlet b.c. (sistem pressure = operating pressure+gauge presure at p.o.b.c).

Hope it helps

mateus

Hi,

First I want to apologize for this long message.

Mateus, I have tried it also with Pressure outlet b.c. I put an outlet pressure 50000 Pa and the operating pressure equal to the atmospheric pressure. And then the minimum absolute pressure was 3.32 E+04 Pa (which is higher than the vapour pressure). then I thought I should decrease the value of the ouletpressure to reach the cavitation conditions. So, I made computations with 25000 Pa as outlet pressure (with the cavitation model OFF) but I got again negative absolute pressure. And I tried also the same case with the cavitation model ON, then I got an ERRor message (pressure correction) and the computations stopped.

1- When I put velocity Inlet and outflow as boundary conditions. I got negative absolute pressure when the inlet velocity is high around 8 m/s. but lower velocities (3.0 m/s and 1.0 m/s ) everything looks good. 2- And when I put velocity inlet and pressure outlet as boundary conditions. with 50000 Pa as outletpressure and operating pressure = Patmospheric, the resulting minimum absolute pressure is not low enough to simulate cavitation. And puting a lower value of the outeltpressure ends up with the same problem (negative absolute pressure).

Mateus, Concerning the operating pressure, I thought it was only a reference pressure used to calculate the absolute pressure, am I right ? so, one can put it equal to zero and then work with absolute pressure unstead of relative (gauge) pressure???

Sorry, again for this looong message !!!

Hi!

The system pressure is equal to operating + gauge pressure. It is good for stability of the solver that the operating and gauge pressure have aproximatelly the same value. Phisically it is the same if you set either one to 0 and the other one to system (absolute)pressure, but the solver will become unstabile.

If you have problems with solver stability you should lower the underrelaxation factors.

What Fluent version are you using? The supercavitation condition can't be modeled with fluent, maybe that's the case when you lovered your pressure to 25000Pa. Try it with the same parameters as in experiment...

regards

MATEUS

I am using fluent 6.1.22.

the problem I don't have any experimental data. But I will try your suggestion and see what happens by lowering the underrelaxation factors.

Hi;

You can get some(many) informations and test cases in sites:

(http://me.engin.umich.edu/CAV2001) (http://iridium.me.es.osaka-u.ac.jp/cav2003)

and you can search in google:

("Inance Senocak" "cavitation") ("Robert Kunz" "cavitation")

they work hard on cavitation numerical modeling and you can find some test cases and experimental data from their papers.

Hope these help you!

ROOZBEH

Hi again;

One years ego Dr. Senocak(I have introduced him to you in my last message) told me that one reason that cause the pressure in the cavity region become lawer than vapor pressure is that you neglect the compressibility effect of cavitation.

Regards

ROOZBEH

My first computations were run without the cavitation model. My aim was to check the values of the absolute pressure to see if the vapour pressure is reached. and then make computations for the same case with the cavitation model ON. I have been struggling with this problem for many days now but I will try the suggestion of mateus and also check the web sites you suggested, thanks a lot.

hi tania,

i have made a one dimensional code for simulating flow in cd nozzle. i am trying to make a two dimensional solver for simulating flow over naca airfoils. can u plz suggest me which scheme should i use and what is the best way out. i am sophomore from india my id is rajx_engg@yahoo.com please help me for this