CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Fluent Pressure outlet b.c. (http://www.cfd-online.com/Forums/fluent/101516-fluent-pressure-outlet-b-c.html)

beanlee999 May 6, 2012 07:55

Fluent Pressure outlet b.c.
 
Hi all,

i am doing a simulation for flow expansion within an exhaust nozzle, using Fluent 6.3.

i used pressure inlet b.c and pressure outlet b.c. (with target mass flow).

I am doing simulation for a compressible subsonic flow. For the nozzle exit, i used 101325Pa for the static gage pressure for pressure outlet, but the simulation always give me a static pressure that is either higher or lower than this value! Can anyone kindly give me some advice on what happened and what should i do if i want to make the exit pressure fixed at 1 atm?

thank you all!

Zigainer May 6, 2012 08:53

I also had problems with pressure outlet and traget mass flow rate (see mass flow inlet and pressure outlet with target mass flow rate)

and here is how fluent does it:
https://www.sharcnet.ca/Software/Flu...ug/node244.htm

So if you waqnt to fix the pressure deactivate the "target mass flow rate"
To get the right mass flow rate you have to change your inlet pressure (if your outlet pressure is fixed)

beanlee999 May 6, 2012 09:17

Reply
 
Hi Zigainer,

So does it mean that i cannot get the desired outlet pressure, and the desired mass flow both at the same time?

Will the mesh affect the simulation results as well? i have tried previously running without target mass flow, with meshes of different grid density. All give me different outlet pressure.

My simulation this time gives me an outlet mach number of 0.3, but the flow is not expanded to atmospheric pressure, which i think is not theoretically possible. Any advice?

LuckyTran May 6, 2012 14:08

Quote:

Originally Posted by beanlee999 (Post 359550)

i used pressure inlet b.c and pressure outlet b.c. (with target mass flow).

I am doing simulation for a compressible subsonic flow. For the nozzle exit, i used 101325Pa for the static gage pressure for pressure outlet, but the simulation always give me a static pressure that is either higher or lower than this value! Can anyone kindly give me some advice on what happened and what should i do if i want to make the exit pressure fixed at 1 atm?

thank you all!

The pressure outlet boundary condition (with target mass flow) will iterate the pressure at the outlet until the desired mass flow rate is achieved. In other words, it is an iterated/variable pressure outlet. If you want to fix the outlet pressure at 1atm, then use a pressure outlet and disable the target mass flow option.


Quote:

Originally Posted by beanlee999 (Post 359560)
So does it mean that i cannot get the desired outlet pressure, and the desired mass flow both at the same time?

You need to use a mass flow inlet and pressure outlet if you want a specified outlet pressure and specified mass flow rate.

Quote:

Originally Posted by beanlee999 (Post 359560)
My simulation this time gives me an outlet mach number of 0.3, but the flow is not expanded to atmospheric pressure, which i think is not theoretically possible. Any advice?

You can have a mach number of 0.3 at many different pressures depending on the density/temperature. It is theoretically possible & allowed.

beanlee999 May 6, 2012 21:10

2 Attachment(s)
Hi all,

i tried both methods already i.e. mass flow inlet with pressure oulet and pressure inlet with pressure outlet (no target mass flow).

The first failed to converge due to divergence (floating point number exceeded). the second converged with weird results.

below shows the convergence results for the 2nd simulation run.

If anyone knows what is the problem, mind sharing with me?

thanks!

LuckyTran May 6, 2012 21:35

Are you using the pressure or density based solver? Spatial discretization?

Try better initialization or reducing under-relaxation factors? If possible, you can try solving it using the pressure based solver first and then switching to the density based solver once you have a somewhat converged solution using the pressure based solver.

How are you judging that the flow is converged with weird results? If so, what are the results? All you showed is a residual plot.

Quote:

Originally Posted by beanlee999 (Post 359550)
For the nozzle exit, i used 101325Pa for the static gage pressure for pressure outlet, but the simulation always give me a static pressure that is either higher or lower than this value! Can anyone kindly give me some advice on what happened and what should i do if i want to make the exit pressure fixed at 1 atm?

What is your nozzle exit static pressure, 1 atm? The default operating pressure is 101325Pa. If you set your exit gage pressure to 101325Pa without changing the operating pressure then you have mistakenly applied the exit pressure to be 2 atm and not 1 atm. The incorrect boundary condition with the wrong initialization can cause the simulation to diverge.

Quote:

Originally Posted by beanlee999 (Post 359620)
i tried both methods already i.e. mass flow inlet with pressure oulet and pressure inlet with pressure outlet (no target mass flow).

The first failed to converge due to divergence (floating point number exceeded). the second converged with weird results.

The pressure inlet & pressure outlet combination is by far the most robust of boundary conditions. You should have no trouble getting this one to converge (with accurate results, not weird ones) unless you messed up terribly somewhere else.

beanlee999 May 6, 2012 21:47

Reply
 
Hi LuckyTran,

I am using density-based solver.

The results are weird basically because they don't give me any actual results. Taking my exhaust nozzle for example, the simulation does not give me the velocity distribution of flow within the nozzle. I will upload the results once i have my simulation files with me. Fluent also reports fragmentation error/violation whenever i try to get the flow analysis (e.g. surface integral, contour etc)

Will solving using pressure based solver help a lot?

LuckyTran May 6, 2012 21:50

Quote:

Originally Posted by beanlee999 (Post 359624)
Will solving using pressure based solver help a lot?

The segregated pressure based solver is much more stable than the coupled density based solver. It will not be as accurate for compressible flows as the density based solver but you can temporarily use it to get a better initialization before switching to the density based solver.

beanlee999 May 7, 2012 09:28

1 Attachment(s)
Hi Luckytran,

i have attached a screen shot of the velocity magnitude from my simulation results.

I am dealing with a flow that ranges from Mach 0.25 to Mach 0.35. The operating pressure that i set is 0, and the exit gage pressure i set is 101325Pa.

I previously used density based solver, with energy equation turned on. The material set is ideal gas (since i do not know exactly what the density of the flow is).

I will try your suggestion to adjust the under-relaxation rule and see how the simulation goes.

Thanks!

LuckyTran May 7, 2012 12:19

Quote:

Originally Posted by beanlee999 (Post 359735)
i have attached a screen shot of the velocity magnitude from my simulation results.

Your velocities are 0 everywhere. Did you perhaps plot wall velocity?

beanlee999 May 7, 2012 18:55

Nope. The simulations dont't seem be complete running as seen in the mass flow diagram previously.

I tried reducing under relaxation but doesn't help.

I couldn't change to pressure based solver directly because the simulations cannot even start running. I guess it might be because the flow is a compressible flow? I tried changin the material, but realized I do not know its density and ideal gas calculation might be the best option for me.

I tried changing the inlet b.c to mass flow inlet but the simulations cannot be completed as well. The same case happened, like what you see in the residual picture.

I suspect it could be the problem with my nozzle design. What do you think?

LuckyTran May 7, 2012 19:16

Quote:

Originally Posted by beanlee999 (Post 359826)
I couldn't change to pressure based solver directly because the simulations cannot even start running. I guess it might be because the flow is a compressible flow? I tried changin the material, but realized I do not know its density and ideal gas calculation might be the best option for me.

The numbers that your computer is cranking have almost no meaning in the physical world. The flow does not know that it is compressible/incompressible. That is entirely up to your modelling. There's no such thing as a simulation that cannot start running because of a reason such as this. You must be doing something else wrong.

How can a simulation not start? If all the boundary conditions are present, an the solution is initialize, and the solver setup, if it still does not work then your computer must not have been paid its monthly rent.

How do you not know the density? You have no clue? You should have some guess of what it is. Help the solver any way you can. Although the ideal gas calculation would be better eventually for the compressible flow option, you should have again some idea of what the flow looks like to even setup the initial conditions. It is very easy for a simulation to diverge with the improper initial conditions (such as initializing with the wrong pressure/temperature/density/velocity).

Most importantly, figure out what is diverging in the simulation. Check actual engineering values and not just residuals or simple reports.

Your nozzle design is up to you.

ahmedcfd2013 January 17, 2015 17:56

Fluent natural ventilation pressure boundary condition
 
Hello All,

I have a problem with a pressure outlet. My problem is a natural convection in wall Trombe ,
My question is:
It is possible to set BC type: pressure outlet at the entrance?
Thank in advance


All times are GMT -4. The time now is 17:19.