[gustavosimiema]

Hi,

I have a mass flow as BC of the inlet measured in a atmospheric environment of 200 cm3/min.
If I would like to run a simulation in 1Pa, than I need to set the Operating Pressure condition to 1Pa and the pressure outlet to 0Pa. Doing that, Fluent automatically convert this mass flow in the inlet to this 1 Pa Pressure? Or should I manually calculated and input it?

[LuckyTran]

It's not entirely clear what you are trying to accomplish, but please verify:

If you set the operating pressure to 1 Pa and then set the exit pressure to 0 Pa then the absolute pressure at the exit will be 1 Pa. This means that the pressure in your domain will be greater than 1 Pa.

Is this a constant density case? 200 cm^3/min is not a mass flow rate, that is a volumetric flow rate. But 200 cm^3/min @ ~1kg/m^3 is a mass flow rate of ~0.012 kg/hr. Now if you specify 0.012 kg/hr at ~ 1Pa pressure, what is your density? If you are using say ideal gas law your velocity would increase by a factor of 100,000 and you would probably be supersonic? If you are running constant density, what then pressure doesn't affect the density/velocity.

What fluent does is it solves for velocity and pressure and then calculates the mass flow at the inlet to see if they match. If not, it adjusts the boundary conditions accordingly. When you specify the mass-flow rate, you do exactly that. Fluent does not convert mass-flow into anything. And mass-flow is mass-flow regardless of what the pressure is. 0.012 kg/s is 0.012 kg/s.

[gustavosimiema]

Sorry, based on the volume flow rate I calculated the mas flow rate. I´m working with gas nitrogen.
I´m using ideal gas law. So, Nitrogen at STP has a density 1.2506 kg/m3. At 1 Pa it´s density is 1,129E-05. For 200 cm^3/min in STP the mass flow rate would be ~3,81293E-06 kg/s. At 1 Pa the mass flow would be ~ 3,76307E-11 kg/s. So this would be the BC at my inlet, correct? With this input, can I ensure that I´m taking into consideration the expansion of the gas once the reference volumetric flow rate I have it´s in atmospheric pressure and my domain is in low pressure (~1Pa)?
Because when I read your comment, I didn´t understand why I would have a supersonic velocity using ideal gas model. I found 0,17 m/s for velocity in my inlet (Diameter = 5mm) with this mass flow rate 3,76307E-11 kg/s.
Regarding the pressure in my Domain, if I would like it to be 1Pa what should I do? Because you said that with Operating Conditions as 1Pa and pressure outlet as 0Pa the pressure in my domain will be higher than 1Pa.

Just for you have in mind what I´m simulating I attached a scheme. I have a chamber with an outlet in the top (middle). On the base of the cahmber there is a pipe with some holes in the top face. And I have one inlet in the middle of the bottom face of this pipe. I´m using laminar flow model.

[RodriguezFatz]

Gustavo do you want to simulate a compressible or an incompressible gas?

[gustavosimiema]

I would like to simulate a incompressible gas... because as it´s low pressure I don´t believe the density will variate...

[RodriguezFatz]

Ok, for such a setup you usually set the gas density by hand in fluent to a fixed value (create/edit materials). Now, you set the outlet to pressure outlet. Basically you can set any pressure you want here, but usually just leave the "0". The inlet is either a velocity inlet or a mass-flow inlet. You don't need to set any "operating pressure" here.

In your first post you write about a mass flow ... and then in units of a volume flow rate. This is confusing.
In your second post you write that the mass flow at different pressures changes. But it doesn't. If the flow is 200 cm^3/min under atmospheric conditions, the mass flow is the same for 1Pa, 1000Pa, and so on. It's always the same mass flow.

[gustavosimiema]

Sorry for the confusion.
Actually I have a volumetric flow rate of 200 cm3/min measured at Atmospheric Pressure. What I have in mind to do is to set the gas as ideal gas. With this selection, I think Fluent will calculate the density of the gas based on the pressure of my domain, right? But I want the pressure of my domain to be 1 Pa. To have that pressure shouldn´t I need to set operating pressure as 1 Pa and outlet pressure as 0 Pa? Because if I let as standard Fluent will calculate as atmospheric pressure. Am I wrong?

[LuckyTran]

Originally Posted by gustavosimiema

But I want the pressure of my domain to be 1 Pa. To have that pressure shouldn´t I need to set operating pressure as 1 Pa and outlet pressure as 0 Pa? Because if I let as standard Fluent will calculate as atmospheric pressure. Am I wrong?

You need to realize that this sets only the exit pressure as 1 Pa. Do you want the exit pressure or inlet pressure to be 1 Pa? Or do you want a fixed density throughout your domain? If you want to fix the density, then you should calculate yourself what the density is at 1 Pa and do a constant density simulation. You can't fix the pressure in the domain at 1 Pa because there's flow obviously. And also don't forget about temperature. I guess you're trying to do a 300K 1 Pa simulation.

If you decide to go the ideal gas route, then definitely set your operating pressure to be ~the pressure in the domain which is ~1 Pa. Otherwise you'll have problems with the truncation error.

Also if you have volumetric flow rate, it could be easier to just use a velocity inlet rather than a mass flow inlet, since that's exactly what you're trying to impose with a volumetric flow rate is velocity.

[RodriguezFatz]

1) If you activate "ideal gas" you solve for compressible equations. You need to manually calculate the density and viscosity of your gas and then put it into the form as a fixed value. Then you have incompressible equations at 1Pa.

2) If you do so (1) and have incompressible equations the absolute pressure value becomes insignificant. You should have a look at the Navier-Stokes equations. You will only see the pressure gradient here, not the pressure itself. So if you add something constant to the pressure your equation won't even recongnize. If you set the outlet pressure to 0 Pa or to 10000 Pa will not change the result at all, except the pressure field becomes an offset of 10000 Pa. For better pictures I would set the outlet to 0 Pa. Maybe operating pressure is used for the pictures to show "real pressure" or so... but it won't change the result. I never used it.

[RodriguezFatz]

Originally Posted by LuckyTran

Also if you have volumetric flow rate, it could be easier to just use a velocity inlet rather than a mass flow inlet, since that's exactly what you're trying to impose with a volumetric flow rate is velocity.

I think in his case a mass flow inlet is much easier because he already knows the volume flow rate at atmospheric conditions. So he can calculate the mass flow in one single step.
Velocity inlet needs the face area of the inlet and the density ratio of both high and low pressure to calculate. I wouldn't use it...

[gustavosimiema]

Thank you so much for the replies.
I tried in both conditions:

1)Calculate the gas density in 1Pa - I found 1,13E-05 kg/m3. The velocity calculate by the software in the inlet was 740m/s (Inlet has 5mm diameter). In this way I had problems with convergence.. All parameters were in the range of 1e-3 of residuals. In this case I used constant density, Operating Pressure 1Pa, outlet pressure 0Pa and mass flow on the inlet.

2) I used the same conditions of (1) just change the constant density to ideal gas.. and the results were even worse.

I think I´m making confusion.

The point is: I need to evaluate the behaviour of the gas in 1Pa pressure.

The gas inlet has 5mm diamater, then get into a pipe of 900mm2 section area (first expansion) then through 6 holes of 2mm diameter come into the chamber (2m3 volume) it will have a big expansion. Please see the attachment...
With this velocity so high in the inlet.. I´m having temperature divergence...

How can I evaluate this situation?

[RodriguezFatz]

You don't need temperature equation. Why do you solve it at all?
What turbulence model do you use?

[gustavosimiema]

I´m using laminar model.... I have low Reynolds...

I´m not sure if I can consider it incompressible... Because the gas comes from a small diameter (5mm) than passes to the pipe (square section = 30mm side) and then.. through the holes... goes to the chamber (2m3 volume). So in this sections I think the density will change... What do you think?

If changes, I need to use ideal gas model for the material and then I´m obligated to enable energy equation...

What´s your opinion?

[RodriguezFatz]

They should both converge... Why don't you just try? Start with incompressible and get it running. You can post pictures here... don't forget to post the residual plot.

[gustavosimiema]

So,

please find in attach both residuals.
1) Laminar model, constant density = 1e-5
Operating Pressure= 1Pa
Mass flow inlet = 3,81293E-06 kg/s
Pressure outlet = 0Pa
Residual didn´t go below 1e-6

2) Laminar model, ideal gas
Operating Pressure= 1Pa
Mass flow inlet = 3,81293E-06 kg/s
Pressure outlet = 0Pa
divergence = temperature


Can we conclude something based on this plots?

[gustavosimiema]

Now I was trying to do the following approach:

Laminar model, ideal gas
Operating Pressure= 0Pa
Pressure outlet = 1Pa
Mass flow inlet = 3,81293E-06 kg/s

But when I took a look in the Reference values based on the inlet I faced some errors.. Please see the attachment... What does it means?

[gustavosimiema]

I think I realized what´s my problem.

I know two things:
1) Mass flow inlet – 3.81e-6 kg/s
2) Pressure outlet (Absolute Pressure = 1Pa)

When I set Operating Pressure = 1Pa I think the software understands all my domain is in such pressure, that´s why it calculates the velocity in the inlet as too high ~ 17200 m/s because the density will be two low ~ 1e-5 kg/m3. But in reality the inlet pressure is not 1Pa… it´s higher than that.
So, regarding the scheme I have attached the sequence of pressure will be like this:
Pinlet >>> PPipe >>>>>> PChamber > Poutlet =1Pa

As pressure outlet is 1 Pa, measured data inside the chamber is something about 1.2 Pa.
So, when I set the gauge pressure in the outlet as 0 I would expect the software to calculate the others pressures (Pipe, chamber and inlet) based on that information and in the mass flow. But I think it doesn´t process in such way…

Where is my misunderstanding? How to set the proper boundary conditions?

[RodriguezFatz]

Originally Posted by gustavosimiema

So, when I set the gauge pressure in the outlet as 0 I would expect the software to calculate the others pressures (Pipe, chamber and inlet) based on that information and in the mass flow.

Yes, this is correct. You did something wrong, so the solver could not converge. This could be many things, such as the grid, bad initial guess, some bad numerical settings. You need to post more information about these things to get any help.

[gustavosimiema]

What kind of information?
A print of the reference values?

[RodriguezFatz]

No. Grid, initialization, numerical settings.