CFD Online URL
[Sponsors]
Home > Forums > FLUENT

Fluent Pressure outlet b.c.

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By LuckyTran

Reply
 
LinkBack Thread Tools Display Modes
Old   May 6, 2012, 08:55
Default Fluent Pressure outlet b.c.
  #1
New Member
 
Choon Yee
Join Date: May 2012
Posts: 13
Rep Power: 4
beanlee999 is on a distinguished road
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!
beanlee999 is offline   Reply With Quote

Old   May 6, 2012, 09:53
Default
  #2
Senior Member
 
Join Date: May 2011
Location: Germany
Posts: 130
Rep Power: 5
Zigainer is on a distinguished road
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)
Zigainer is offline   Reply With Quote

Old   May 6, 2012, 10:17
Default Reply
  #3
New Member
 
Choon Yee
Join Date: May 2012
Posts: 13
Rep Power: 4
beanlee999 is on a distinguished road
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?
beanlee999 is offline   Reply With Quote

Old   May 6, 2012, 15:08
Default
  #4
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 526
Rep Power: 10
LuckyTran is on a distinguished road
Quote:
Originally Posted by beanlee999 View Post

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 View Post
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 View Post
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.
LuckyTran is offline   Reply With Quote

Old   May 6, 2012, 22:10
Default
  #5
New Member
 
Choon Yee
Join Date: May 2012
Posts: 13
Rep Power: 4
beanlee999 is on a distinguished road
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!
Attached Images
File Type: jpg 1.JPG (26.0 KB, 27 views)
File Type: jpg 2.JPG (27.2 KB, 29 views)
beanlee999 is offline   Reply With Quote

Old   May 6, 2012, 22:35
Default
  #6
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 526
Rep Power: 10
LuckyTran is on a distinguished road
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 View Post
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 View Post
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.
delaneyluke likes this.
LuckyTran is offline   Reply With Quote

Old   May 6, 2012, 22:47
Default Reply
  #7
New Member
 
Choon Yee
Join Date: May 2012
Posts: 13
Rep Power: 4
beanlee999 is on a distinguished road
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?
beanlee999 is offline   Reply With Quote

Old   May 6, 2012, 22:50
Default
  #8
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 526
Rep Power: 10
LuckyTran is on a distinguished road
Quote:
Originally Posted by beanlee999 View Post
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.
LuckyTran is offline   Reply With Quote

Old   May 7, 2012, 10:28
Default
  #9
New Member
 
Choon Yee
Join Date: May 2012
Posts: 13
Rep Power: 4
beanlee999 is on a distinguished road
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!
Attached Images
File Type: jpg velocity.jpg (33.3 KB, 29 views)
beanlee999 is offline   Reply With Quote

Old   May 7, 2012, 13:19
Default
  #10
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 526
Rep Power: 10
LuckyTran is on a distinguished road
Quote:
Originally Posted by beanlee999 View Post
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?
LuckyTran is offline   Reply With Quote

Old   May 7, 2012, 19:55
Default
  #11
New Member
 
Choon Yee
Join Date: May 2012
Posts: 13
Rep Power: 4
beanlee999 is on a distinguished road
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?
beanlee999 is offline   Reply With Quote

Old   May 7, 2012, 20:16
Default
  #12
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 526
Rep Power: 10
LuckyTran is on a distinguished road
Quote:
Originally Posted by beanlee999 View Post
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.
LuckyTran is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
operation pressure and pressure outlet BC Lilly FLUENT 4 May 8, 2013 10:57
VOF Outlet boundary condition in cfd - ace JM Main CFD Forum 0 December 15, 2006 09:07
Which B.C. i should apply for this problem?urgent raivish FLUENT 0 January 6, 2006 09:48
Gas pressure question Dan Moskal Main CFD Forum 0 October 24, 2002 23:02
Hydrostatic pressure in 2-phase flow modeling (long) DS & HB Main CFD Forum 0 January 8, 2000 16:00


All times are GMT -4. The time now is 02:02.