need help with fluent/restrictor analysis...

[mnowicki]

We're trying to analyze some restrictor designs in fluent, however we're having some issues. We're using a viscous k-e model, with density dependent upon the ideal gas law. The inlet boundary condition is set to a pres-inlet with Pgauge=0. The outlet boundary condition is set to pres-outlet with a constant gauge pressure of -80,000 Pa. The discretization parameters are all set to first order. Now when we try to run it, we get an amg solver error: pressure/temperature. I assume this error shows up either because the solution is diverging or the pressure/temperature limits have been reached. However, I don't understand why this would be happening.

Does anyone know what could be the issue? Or could you let us know what works or how you guys set your boundary conditions/settings when you do an analysis. Thanks in advance for any help.

Matt Nowicki
University of Pennsylvania

[mnowicki]

We're trying to analyze some restrictor designs in fluent, however we're having some issues. We're using a viscous k-e model, with density dependent upon the ideal gas law. The inlet boundary condition is set to a pres-inlet with Pgauge=0. The outlet boundary condition is set to pres-outlet with a constant gauge pressure of -80,000 Pa. The discretization parameters are all set to first order. Now when we try to run it, we get an amg solver error: pressure/temperature. I assume this error shows up either because the solution is diverging or the pressure/temperature limits have been reached. However, I don't understand why this would be happening.

Does anyone know what could be the issue? Or could you let us know what works or how you guys set your boundary conditions/settings when you do an analysis. Thanks in advance for any help.

Matt Nowicki
University of Pennsylvania

[Krautsalat]

Are you sure with 80000Pa pressure difference? Remember that the boundary condition is set in reference to your operating pressure and is not the absolute pressure.
For simulations like this I normaly start with an velocity boundary and a constant density to get an initial solution with small mass flow rates. From there you can switch to variable density with pressure bnds and ramp up the pressure difference.

Krautsalat

[Dallas Blake]

Try Setting your operating conditions to 0Pa and then setting your pressure inlet to 101325Pa and your pressure outlet to 80000Pa. Thats what I have been doing with the K-Epsilon solver with no problems. Other things to consider are what is your mesh structure? What sort of size interval are you using? any gradienting? Are you running segregated or coupled equations? have you set your solver to axi-symmetric?

[mnowicki]

Thanks for the help krautsalat and Dallas. I have gotten the simulation to work and my model is telling me that the restrictor is choked flow at 73 g/s. So at least thats a start. Now, I have brought down the pressure difference to about 6kpa before the restrictor's mass flow decreases from its choked value. Is this pressure difference in the ball park of what it should be because it seems low.

Dallas, I'm doing this model in 3d (i know its a waste of computation time since its a 2d problem but we just got fluent at my school and the lab professor wanted some pretty 3d flow figures for the lab's opening day, so i figured i might as well). So i'm using tetrahedral/hybrid mesh with a mesh size of 1.5 mm. I'm also using the "green-gauss cell based gradient". Are there other settings that you would recommend in order to get more accurate results?

Thanks again.

Matt Nowicki
University of Pennsylvania

[Krautsalat]

<BLOCKQUOTE class="ip-ubbcode-quote"><div class="ip-ubbcode-quote-title">quote:</div><div class="ip-ubbcode-quote-content">Now, I have brought down the pressure difference to about 6kpa before the restrictor's mass flow decreases from its choked value. Is this pressure difference in the ball park of what it should be because it seems low. </div></BLOCKQUOTE>

That depends on the geometry, but the order of magnitude is ok.

As for the mesh, it should not to be to hard to mesh a simple geometry like the restrictor with hex only. That should help with accuracy/stability and also needs less cells for a given accuracy.
Definitly use second order discretization for the solved equations.

Krautsalat

[Dallas Blake]

A question for the people using Fluent,

on your outlet conditions, if you are using a pressure outlet are you targetting a mass flow or are you setting just the pressure outlet and seeing what the mass flow turns out to be with that pressure differential

[Krautsalat]

I use pressure outlet and see what the massflow is, if you set a target massflow higher than the max. flow through the restrictor fluent would try to achieve the target massflow by lowering the outlet pressure to unfeasible levels.

Krautsalat

[per]

I have a question about the "operating pressure" input in Fluent. Is that pressure used as a reference pressure when Fluent calculates the gauge pressure? for example, if i would like to calculate some air flow through a jet engine on ground, then the operating pressure is equal to the atmospheric pressure on the ground?
I have also another question about the "outlet pressure" boundary condition. if i have a pipe with some air flow and I use a motor driven engine that sucks the air out from the pipe, then the outlet pressure is not necessary equal to the atmospheric pressure?