what is meant by Operating Pressure in Fluent?
 

hello all,
i am a new user in Fluent.
i want to know what exactly is meant by operating pressure in fluent?
its default value is 101325 pa, is it atmospheric pressure? but sometime we also assume 0 as operating pressure, its making me feel dizzy....
what will be the operating pressure in 10 meter depth of a pool?
:confused:

It depends on how you model the density. It is always valid to set the operating pressure to (approximately) the mean pressure of the flow field. But it is only when you model the density using incompressible ideal gas law, or you are dealing with low-Mach-number compressible flow that the value of operating pressure is important.

The operating pressure is not used if the density is modeled to be constant.

You should check the Fluent user manual because it has more detailed and accurate description of the operating pressure.

in my case density is constant so it means i can take operating pressure as zero??????

dear ....
 

when you set pressure of operation condition 0 pascal, you prevent reverse flow in your domain.

Yes. You can set operating pressure to any value because it is not used in case of constant density.

Thank you :rolleyes:

what is that value in VOF model? (water+air)

vof
 

if you set value of water 1 in a zone,value of air will be 0 at same zone.

hi blackmask,
can you tell us how do we know the mean pressure of the flow field in fluent. in my case i simulate 2d vawt in a wind tunnel. is there any consideration when we want to specify certain value of operating condition in fluent for incompressible ideal gas air. what about reference pressure location? its default value is [0,0,0]. how to specify the right reference pressure location in our simulation? please help us

is there any help?

i am trying to simulate flow over blunt bodies my conditions are 100500pa, 303k,1.1551 density, what should be my operating pressure and guage pressure?

You choose!

Real pressure = operating pressure + guage pressure.

If you want the real pressure to be 100500 Pa, you can set operating pressure at 100500 Pa, and then at the boundary set 0 Pa.
Or set the operating pressure at 100000 Pa, and the pressure at the boundary at 500 Pa.
Or the operating pressure at 0 Pa, and the pressure at the boundary at 100500 Pa.

Physically, it is all the same. Exactly the same, identical.

Only numerically, it is helpful to have smaller numbers for guage pressures, so put your operating pressure close to the 'average' pressure in your system. Extreme example: don't set your operating pressure at 10000100500 Pa, and your guage pressure at -10000000000 Pa, you will get numerical problems.

Also is prism layer generation necessary for supersonic speed?.
Without using prism layer mesh can I use k omega or k epsilon turbulence model?

A Question regarding this Operation Pressure:

I have a low-Mach-No. Simulation and i know that the pressure inside my geometry should be s.th. about 7-8bar. So i set the operation Pressure to 7 bar. As result I got a pressure value of 1bar in the interior. So does this mean that I have to add 1 bar to the operation pressure to get the "real" value of pressure?

Actually I have 1 bar beyond the inlets and outlets. Does this operation pressure influence my "outside"-conditions? So if I want 1 bar outside, do i have to set the pressure boundary condition to -6bar because 7bar minus 6 bar is 1bar?

Best regards

“ANSYS Fluent provides a “floating operating pressure” option to handle time-dependent compressible flows with a gradual increase in the absolute pressure in the domain. This option is desirable for slow subsonic flows with static pressure build-up, since it efficiently accounts for the slow changing of absolute pressure without using acoustic waves as the transport mechanism for the pressure build-up.

Examples of typical applications include the following:

1.combustion or heating of a gas in a closed domain

2.pumping of a gas into a closed domain

Limitations:

The floating operating pressure option should not be used for transonic or incompressible flows. In addition, it cannot be used if your model includes any pressure inlet, pressure outlet, exhaust fan, inlet vent, intake fan, outlet vent, or pressure far field boundaries.“

From ANSYS FLUENT help document.

Suppose I have set intet pressure = 405300 Pa (Fluent solver)
Outlet gauge pressure = 4000 Pa
Operating pressure = 0 Pa
Then A/C you Real Pressure at inlet = 405300+0 = 405300 Pa
outlet pressure gauge pressure = 4000 + 0 = 4000 Pa only ?

Yes if you are using 0 operating pressure the you have to apply absolute value of pressure at outlet also

Thank you Kushal.

Operating pressure
 

Hi Bholu,
Did you get the desired result.

Hi all,

Thanks for all your answer. What about if i want to calculate in a bend pipe the pressure losses and the poutlet is 10bar in a incompressible fluid?
From what i understood:
a) operating pressure= 10 bar
b) gauge pressure = 0 bar?
Correct?
Why my pressure in CFD post is not considering the operating pressure?

Thanks