[Zigainer]

Hi,

I have a question regarding the boundary condition.

I have a mass flow inlet and three pressure outlets. If assigned a specific target mass flow rate at each of these pressure outlets. But fluent does not always bring up the designated target mass flow rate.
At a first stage my problem is non-rotating. Almost every time I get the target mass flow rate (guess the difference is because the solution is not fully converged - solely increase mass flow rate at the inlet). But if I start to rotate (full mass flow rate at the inlet and increasing rotation speed) I get convergence problems and the target mass flow rate seems to be ignored..... so I asked myself if it would be better to use a pressure inlet and the mass flow will be reached because of the target mass flow rate ... or what would you suggest?

Thanks in advance!

[banty]

Originally Posted by Zigainer

Hi,

I have a question regarding the boundary condition.

I have a mass flow inlet and three pressure outlets. If assigned a specific target mass flow rate at each of these pressure outlets. But fluent does not always bring up the designated target mass flow rate.
At a first stage my problem is non-rotating. Almost every time I get the target mass flow rate (guess the difference is because the solution is not fully converged - solely increase mass flow rate at the inlet). But if I start to rotate (full mass flow rate at the inlet and increasing rotation speed) I get convergence problems and the target mass flow rate seems to be ignored..... so I asked myself if it would be better to use a pressure inlet and the mass flow will be reached because of the target mass flow rate ... or what would you suggest?

Thanks in advance!

Hi,


Actually it depends upon your problem or what u want to achieve.

Mass flow rate allow the total pressure to vary in response to the interior solution. on the other hand the pressure inlet BC, total pressure is fixed and the mass flux varies.
A mass flow inlet is used when it is more important to match a prescribed mass flow rate than to match the total pressure of the inflow stream.

[Zigainer]

Its actually more important to have the correct mass flow. I do simulation on leading edge impingment and therefore a mass flow results in a specific jet Re number, which is important for me.
I just switched off the traget mass flow rate at the pressure outlets and my solution is converged .... But I don't get the mass flow distribution (4 outlets) which I want (to compare my results to an exeriment) ... so I guess I have to adjust the gaug pressure for each pressure outlet until I get my mass flow rate.

[banty]

Originally Posted by Zigainer

Its actually more important to have the correct mass flow. I do simulation on leading edge impingment and therefore a mass flow results in a specific jet Re number, which is important for me.
I just switched off the traget mass flow rate at the pressure outlets and my solution is converged .... But I don't get the mass flow distribution (4 outlets) which I want (to compare my results to an exeriment) ... so I guess I have to adjust the gaug pressure for each pressure outlet until I get my mass flow rate.

yes, i think it will work. But if u are using Density based solver and want to compare the result with experiment data. then set direct pressure specification ( others methods are weak enforcement of avg. pressure(default setting) and strong enforcement of avg. pressure)for pressure calculation at outlet which is default with pressure based solver. this can can be done through TUI.
define>boundary condition>bc-setting no no

[Zigainer]

I am using pressure based solver ..... at the moment it works quite fine. I can use second order solver but if I increase the under relaxation factors to the default values I get divergence.... but I am happy do use 2nd order and no divergence. Probably I have to increase the under relaxation values more slowly

[banty]

For steady state solution, std process to run the simulation with 1st order for some iteration and wait for residuals to come down to certain level (~10^-2 to 10^-3) then switch on to 2nd order.
In transient case, care of the sub-iteration per time step..play with under relaxation factor.

Originally Posted by Zigainer

I am using pressure based solver ..... at the moment it works quite fine. I can use second order solver but if I increase the under relaxation factors to the default values I get divergence.... but I am happy do use 2nd order and no divergence. Probably I have to increase the under relaxation values more slowly

[Zigainer]

I do a steady state simulation and I am running 1st order first (otherwise I can't achieve convergence at all) with under relaxation factor of around 1/3 of the default values. Then I change to 2nd order which works fine, but when I start increasing the under relaxation factors my convergence behavior is really bad (around 1E-1 or divergence) .... but probably I should use more iterations for 2nd order and increase the under relaxation factors more sloley. But actually I can live with these low under relaxation factors. It would be more important to get some specific mass flow rates at the outlet and therefore I have to alter the gauge pressure at each outlet, because the “target mass flow rate” for pressure outlets results in divergence.

[kingjewel1]

Originally Posted by banty

yes, i think it will work. But if u are using Density based solver and want to compare the result with experiment data. then set direct pressure specification ( others methods are weak enforcement of avg. pressure(default setting) and strong enforcement of avg. pressure)for pressure calculation at outlet which is default with pressure based solver. this can can be done through TUI.
define>boundary condition>bc-setting no no

I couldn't quite follow you, would you care to explain your reasoning behin strong and weak pressure enforcement?

A minor tweak:

define bound bc mass no

[banty]

here is the explanation
https://www.sharcnet.ca/Software/Fluent12/html/ug/node244.htm[/URL]

[nsha]

Hi, I have a problem to set the flow rate at the outlet boundary of my geometry. I'm simulation incompressible flow with known pressure at the inlet. I need to set my outlet to be at 0.9kg/s flow rate. What is the most suitable boundary condition should I use? Can I use 'mass flow-inlet' to input the flow rate value at the outlet? (since it is the only boundary condition option that ask for mass flow rate value) Or do I have to set the outlet to 'outflow'?

[Guava Wang]

hi zigainer,

about this questiong, what is your solution in the end? do you mind share your method with me? i have the same question with you, hope i can get some help from you. thank you.