CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

a problem of nozzle simulation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 25, 2010, 13:16
Default a problem of nozzle simulation
  #1
Member
 
chenkai
Join Date: May 2010
Location: munich
Posts: 44
Rep Power: 7
xck1986 is on a distinguished road
Dear OF Users

I want to simulate a laval nozzle wit OF.
I have already simulate this case in StarCCM+, and it works well. But when we swith to openFoam, it always stop up to a certain iteration.

I have create the Mesh using HyperMesh, then save it as StarCD format, and convert it into OpenFOAM.

The solver we have chosen now is sonicFoam.

The setting of the boundary condition is in Folder 0 in the attached files.
For the boundary condition we have set a pressure boundary condition, the absolute pressure in inlet is 2bar and outlet is 1bar. Other setting is all in the Folder 0.

I think it is a problem of setting the boundary condition. Because when we decrease the initial velocity, e.g. from -100m/s to -10m/s (the fluid flow in -Z direction,so the velocity is negativ), and also decrease the inlet pressure e.g. from 2bar to 1.1bar, it can finish all the iteration.

Here I have copy here two folder:
1: Nozzlesimulation_stop_with_error: in this case we have set the pressure in inlet is 2bar, outlet is 1bar and initial velocity is -100m/s, but it always stop up to a certain iteration.

2: Nozzlesimulation_no_error: in this case we have decrease the the initial velocity from -100m/s to -10m/s, and also decrease the inlet pressure from 2bar to 1.1bar,so it can run the simulation up to the last iteration.

Because the mesh is too large, so in the folder constant I have not copy the file polyMesh.

I don't konw where exactly the problem is. I am so appreciate that if anyone can help me.
Thanks a lot for you help.


Chenkai


The error is
--> FOAM FATAL ERROR:
Maximum number of iterations exceeded
From function specieThermo<thermo>::T(scalar f, scalar T0, scalar (specieThermo<thermo>::*F)(const scalar) const, scalar (specieThermo<thermo>::*dFdT)(const scalar) const) const
in file /home/armin/OpenFOAM/OpenFOAM-1.7.1/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 67.
FOAM aborting
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/armin/OpenFOAM/OpenFOAM-1.7.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/armin/OpenFOAM/OpenFOAM-1.7.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Foam::ePsiThermo<Foam:ureMixture<Foam::constTran sport<Foam::specieThermo<Foam::eConstThermo<Foam:: perfectGas> > > > >::calculate() in "/home/armin/OpenFOAM/OpenFOAM-1.7.1/lib/linuxGccDPOpt/libbasicThermophysicalModels.so"
#3 Foam::ePsiThermo<Foam:ureMixture<Foam::constTran sport<Foam::specieThermo<Foam::eConstThermo<Foam:: perfectGas> > > > >::correct() in "/home/armin/OpenFOAM/OpenFOAM-1.7.1/lib/linuxGccDPOpt/libbasicThermophysicalModels.so"
#4
in "/home/armin/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linuxGccDPOpt/sonicFoam"
#5 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#6
in "/home/armin/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linuxGccDPOpt/sonicFoam"
Aborted
Attached Files
File Type: zip nozzle.zip (15.7 KB, 136 views)
xck1986 is offline   Reply With Quote

Old   November 26, 2010, 01:55
Default
  #2
Senior Member
 
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 7
nakul is on a distinguished road
Hi

The problem is definitely with your BC. For pressure try "zeroGradient" at the oultet. If however outlet pressure specification is really crucial to your test case, try wave transmissive. I would however recommend zeroGradient only.

Similarly you may specify zeroGradient at outlet for T and U also, if you are sure that supersonic flow will be established in the nozzle for your pressure ratio. Otherwise you may try "inletOutlet" for U.

One more advice try simulating with rhoCentralFOAM, because in my opinion it gives better results.

-Nakul
nakul is offline   Reply With Quote

Old   November 26, 2010, 06:05
Default
  #3
Member
 
chenkai
Join Date: May 2010
Location: munich
Posts: 44
Rep Power: 7
xck1986 is on a distinguished road
Quote:
Originally Posted by nakul View Post
Hi

The problem is definitely with your BC. For pressure try "zeroGradient" at the oultet. If however outlet pressure specification is really crucial to your test case, try wave transmissive. I would however recommend zeroGradient only.

Similarly you may specify zeroGradient at outlet for T and U also, if you are sure that supersonic flow will be established in the nozzle for your pressure ratio. Otherwise you may try "inletOutlet" for U.

One more advice try simulating with rhoCentralFOAM, because in my opinion it gives better results.

-Nakul


Hallo Nakul,

Thanks a lot for you help.
I have use you suggestion to set the outlet presuure as zeroGradient and also for the T and U.
It works better than before and it can finish more timestep, but still stop at one timestep with the same error.

--> FOAM FATAL ERROR:
Maximum number of iterations exceeded
From function specieThermo<thermo>::T(scalar f, scalar T0, scalar (specieThermo<thermo>::*F)(const scalar) const, scalar (specieThermo<thermo>::*dFdT)(const scalar) const) const
in file /home/armin/OpenFOAM/OpenFOAM-1.7.1/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 67.
FOAM aborting

I have copy here the results and parameters from another software StarCCM+. Could you pleasure do me more favour?
Thanks again!!!

Chenkai
Attached Images
File Type: jpg presuure and velocity simulated with StarCCM+.JPG (35.0 KB, 208 views)
File Type: jpg parameter set in StarCCM+.JPG (69.1 KB, 132 views)

Last edited by xck1986; November 26, 2010 at 10:04.
xck1986 is offline   Reply With Quote

Old   November 26, 2010, 07:45
Default
  #4
Senior Member
 
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 7
nakul is on a distinguished road
Sorry, I can't help you here becuase I have never worked on StarCMM and I also don't have that software.

However I will help you with your problems in OpenFOAM.

You may try wave transmissive for p and inletOutlet for U at the outlet and telll me what results you get.
nakul is offline   Reply With Quote

Old   November 26, 2010, 10:02
Default
  #5
Member
 
chenkai
Join Date: May 2010
Location: munich
Posts: 44
Rep Power: 7
xck1986 is on a distinguished road
Quote:
Originally Posted by nakul View Post
Sorry, I can't help you here becuase I have never worked on StarCMM and I also don't have that software.

However I will help you with your problems in OpenFOAM.

You may try wave transmissive for p and inletOutlet for U at the outlet and telll me what results you get.

hallo Nakul,
Thanks a lot for your help.
I have set the Outlet of P and U like you tell me.
1. zeroGradient for P and U
2. transmissive for p and inletOutlet for U
But it still stop up to a timestep, here I past the residuals files of the two case. It likes like very strange, and at time step 0.0001 the result is divergent.
Thanks a lot for your time!

Last edited by xck1986; November 26, 2010 at 10:52.
xck1986 is offline   Reply With Quote

Old   November 29, 2010, 01:00
Default
  #6
Senior Member
 
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 7
nakul is on a distinguished road
Hi,
I went through the attached case files that you sent. I think you may try doing the following

1) Reduce your maxCo =0.5.
2) Run "checkMesh" command and see if your mesh is satisfactory. Since you didn't upload your blockMeshDict, so I wasn't able to do this.
3) Don't specify fixedValue at outlet for any of the parameters. Change BC of k, epsilon and T also at outlet to inletOutlet/zeroGradient. They can have their BC similar to U.
Try these things along with p as transmissive/zeroGradient and tell me if you face any other problems.
nakul is offline   Reply With Quote

Old   November 29, 2010, 11:43
Default
  #7
Member
 
chenkai
Join Date: May 2010
Location: munich
Posts: 44
Rep Power: 7
xck1986 is on a distinguished road
Quote:
Originally Posted by nakul View Post
Hi,
I went through the attached case files that you sent. I think you may try doing the following

1) Reduce your maxCo =0.5.
2) Run "checkMesh" command and see if your mesh is satisfactory. Since you didn't upload your blockMeshDict, so I wasn't able to do this.
3) Don't specify fixedValue at outlet for any of the parameters. Change BC of k, epsilon and T also at outlet to inletOutlet/zeroGradient. They can have their BC similar to U.
Try these things along with p as transmissive/zeroGradient and tell me if you face any other problems.

Hi Nakul,
Thank you very much for your suggestion.
It works very well this time, when I follow your instruction. I have set all the outlet boundarycondition as zerogradient.
But this time I have use the solver rhoPisoFoam instead of sonicFoam. Because with sonicFoam I always have the same error, I think it is the resaon that with sonicFoam, even if I set the maxCo=0.8, the Co is still very lager during the calculation.
So I change the solver and it works with rhoPisoFoam

And I still have a question: When do we need to set the boundary condition of Pressure as Transmissive?
Thanks a lot again!!!
xck1986 is offline   Reply With Quote

Old   November 30, 2010, 00:43
Default
  #8
Senior Member
 
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 7
nakul is on a distinguished road
Hi

You use transmissive for pressure when you want to avoid reflection of pressure waves back into your domain and want them to be transmitted smoothly out of the domain through the outlet.

Read this:
http://openfoamwiki.net/index.php/Ho...dary_condition
nakul is offline   Reply With Quote

Old   February 2, 2011, 12:10
Default Thank you!
  #9
Member
 
Ammar Tareen
Join Date: Jan 2011
Location: Boston University
Posts: 61
Rep Power: 6
atareen64 is on a distinguished road
Thank you so much for this post. It's helping me with my case
atareen64 is offline   Reply With Quote

Old   May 24, 2012, 01:39
Default
  #10
New Member
 
Arif
Join Date: Mar 2012
Posts: 15
Rep Power: 5
upal_arif is on a distinguished road
Hi,

I am looking for a freelancer to simulate supersonic flow through C-D nozzle by fluent 6.2.16

Please contact upal_arif@yahoo.com


Quote:
Originally Posted by nakul View Post
Hi

The problem is definitely with your BC. For pressure try "zeroGradient" at the oultet. If however outlet pressure specification is really crucial to your test case, try wave transmissive. I would however recommend zeroGradient only.

Similarly you may specify zeroGradient at outlet for T and U also, if you are sure that supersonic flow will be established in the nozzle for your pressure ratio. Otherwise you may try "inletOutlet" for U.

One more advice try simulating with rhoCentralFOAM, because in my opinion it gives better results.

-Nakul
upal_arif is offline   Reply With Quote

Old   May 25, 2012, 01:38
Default
  #11
Senior Member
 
Nakul
Join Date: Apr 2010
Location: India
Posts: 147
Rep Power: 7
nakul is on a distinguished road
Hi Arif,

Please provide some more details regarding your problem with supersonic C-D Nozzle
nakul is offline   Reply With Quote

Old   November 27, 2012, 09:22
Default waveTransmissive
  #12
Member
 
Valentin Wibaut
Join Date: Oct 2012
Posts: 45
Rep Power: 4
vwibaut is on a distinguished road
Hi Nakul and other foamers,

I would kike to simulate the flow in a nozzle, specially the case supersonic in all the divergent and the case supersonic with a shock in the divergent. As a shock is possible I use waveTransmissive for the outlet pressure.
My questions concerns linf: when I put a big linf I have a flow wich seems to be good except that my outlet pressure isn't the value I give in waveTransmissive.
when I put a small linf, stall appears. How do I choose linf?

Thanks for your help
vwibaut 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
Domain format problem on airfoil flow simulation andrenonaka CFX 6 December 4, 2014 04:57
convergent_divergent nozzle simulation in CFX-11 sivarama1 CFX 22 February 18, 2013 17:23
For Nozzle fluent problem Jie FLUENT 17 January 11, 2012 14:44
mass balance problem in transient simulation nana84 CFX 2 April 15, 2010 19:53
Star-CD transient simulation, problem of loss of mass kit STAR-CD 3 April 13, 2010 11:34


All times are GMT -4. The time now is 19:22.