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

rhoSimpleFoam troubles

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 16, 2010, 12:53
Unhappy rhoSimpleFoam troubles
  #1
New Member
 
Nicola Zanella
Join Date: May 2010
Location: Venice Italy
Posts: 3
Rep Power: 7
Nicola_Z is on a distinguished road
Hi all, I'm new in cfd analysis and I have to model a subsonic airfoil whit rhoSimpleFoam and Spalart-Allmaras turbolence model.
I'have this error:

smoothSolver: Solving for Ux, Initial residual = 0.0718934, Final residual = 0.00354669, No Iterations 6
smoothSolver: Solving for Uy, Initial residual = 0.195708, Final residual = 0.0109704, No Iterations 6
DILUPBiCG: Solving for h, Initial residual = 0.996372, Final residual = 0.0960167, No Iterations 621
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/nicola/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/nicola/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted:
#3 Foam::hPsiThermo<Foam:ureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam:erfectGas> > > > >::calculate() in "/home/nicola/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libbasicThermophysicalModels.so"
#4 Foam::hPsiThermo<Foam:ureMixture<Foam::sutherlan dTransport<Foam::specieThermo<Foam::hConstThermo<F oam:erfectGas> > > > >::correct() in "/home/nicola/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libbasicThermophysicalModels.so"
#5 main in "/home/nicola/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linuxGccDPOpt/rhoSimpleFoam"
#6 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#7 _start at /build/buildd/glibc-2.9/csu/../sysdeps/i386/elf/start.S:122
Floating point exception

Someone can help me?
Thanks a lot!
Nicola_Z is offline   Reply With Quote

Old   May 17, 2010, 09:36
Default
  #2
Member
 
Ngoc-Minh Truong
Join Date: Feb 2010
Location: Toulouse, France
Posts: 42
Rep Power: 7
truong_nm is on a distinguished road
Send a message via MSN to truong_nm
Please give us more details on your case: Mach Reynolds numbers, BCs, mesh properties
truong_nm is offline   Reply With Quote

Old   May 18, 2010, 15:09
Default
  #3
Member
 
Sylvain Martel
Join Date: Apr 2009
Location: University of Sherbrooke/Quebec/Canada
Posts: 51
Rep Power: 8
smart is on a distinguished road
I have the same problem with rhoSimpleFoam 1.6. In fact, I run a simple case in OF 1.5 and all is good compared to analytical value for flow in a nozzle (steam). I am trying to have the same results with OF 1.6 and I cannot obtain a converge solution. What is the main difference between these two version?

Thank you!

Sylvain
smart is offline   Reply With Quote

Old   May 19, 2010, 09:47
Default great trouble
  #4
New Member
 
Nicola Zanella
Join Date: May 2010
Location: Venice Italy
Posts: 3
Rep Power: 7
Nicola_Z is on a distinguished road
thanks for reply me,
I'm sure that my mesh was ok. I know static and total p and T at inlet and outlet: in FLUENT are called far_field and press_out. On surface of my airfoil I only know that there is slip. The Reynold's number is 3e06 and Ma = 0.5.
What are my BC in OF? I try zerogradient on airfoli, inletoutlet and outletinlet, but nothing.
I accept all suggest!
Nicola_Z is offline   Reply With Quote

Old   May 19, 2010, 09:59
Default
  #5
Member
 
Ngoc-Minh Truong
Join Date: Feb 2010
Location: Toulouse, France
Posts: 42
Rep Power: 7
truong_nm is on a distinguished road
Send a message via MSN to truong_nm
@Sylvain: Take a look at the release notes of OpenFOAM 1.6, that will certainly help you.

@Nicola_z: As your flow is subsonic, you need four characteristics at inlet and only one at outlet. I suggest you: p_s, U, T_s (two components of velocity thanks to angle of attack and slideslip angle) and p_s at outlet.
For the type of BC, I would try "freestream" for U/T and "freestreamPressure" for p at inlet and freestream for p at outlet and zerogradient for the others.
It seems strange that there is a slip condition on the airfoil as you use viscous computations. What about no-slip condition ? In this last case, I would try fixedValue to 0,0,0 for U and zeroGradient for p/T.

Don't forget to post your results
truong_nm is offline   Reply With Quote

Old   May 19, 2010, 11:12
Default
  #6
New Member
 
Nicola Zanella
Join Date: May 2010
Location: Venice Italy
Posts: 3
Rep Power: 7
Nicola_Z is on a distinguished road
Tahnks truong_nm!
now i try your suggest and you say the true, the condition on airfoil is no slip... I was sleeping, sorry
And what you can say me about mut e nutilda? I have calculated the value, but what BC can I use for this, especially on surface of airfoil? I've used mutSpalartAllmarasFunction or zeroGradient.
Nicola_Z is offline   Reply With Quote

Old   May 19, 2010, 11:22
Default
  #7
Member
 
Ngoc-Minh Truong
Join Date: Feb 2010
Location: Toulouse, France
Posts: 42
Rep Power: 7
truong_nm is on a distinguished road
Send a message via MSN to truong_nm
For the freestream conditions, take a look at this page on the CFDOnline wiki: http://www.cfd-online.com/Wiki/Turbu...ary_conditions
I think that it'll help you to determine the farfield conditions.
Concerning the airfoil nuTilda value, if your mesh is good enough, you can try zeroGradient. Otherwise, use SA wall function

Wait for your feedback
truong_nm is offline   Reply With Quote

Old   April 23, 2013, 04:12
Unhappy
  #8
Member
 
Join Date: Oct 2012
Posts: 47
Rep Power: 4
sh.d is on a distinguished road
hi truong
i want to simulate super critical airfoil by rhosimplecfoam but there is this error:Floating point exception
mach:0.5
please help me
Attached Files
File Type: zip 0.zip (6.0 KB, 20 views)
File Type: zip system.zip (4.8 KB, 14 views)
sh.d is offline   Reply With Quote

Old   April 23, 2013, 10:13
Default
  #9
Senior Member
 
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 236
Rep Power: 8
fredo490 is on a distinguished road
Usually, I use this technic (be careful, I use rhoSimplecFoam not rhoSimpleFoam ) :

1) I run my case with rhoSimplecFoam with very small relaxation number if needed (can go down to 0.1 or even 0.01). This is just to get a first field. You have to know that those low relaxation numbers will lead to unphysical results because it doesn't satisfy continuity and other. I usually run for few hundred or thousand of iterations.
http://www.fredo490.fr/public/rhoSim...aca12-AOA4.zip

2) I run the previous case with higher relaxation number. So I use the final results from the previous solver as initialization of this solver. I usually increase all the relaxation numbers over 0.5. This should immediately converge your case and remove all unphysical behavior.
http://www.fredo490.fr/public/rhoSim...a12-AOA4_2.zip

3) Finally, I use the second solver data to initialize the unsteady solver. I have found that rhoLTSPimpleFoam is more stable that rhoPimpleFoam. If you run OpenFoam 2.2, rhoLTSPimpleFoam is now a solver. If you run OpenFoam 2.1, you can use rhoPorousMRFLTSPimpleFoam where you remove all Porous zones.
http://www.fredo490.fr/public/rhoLTS...aca12-AOA4.zip

I have another case with a cylinder which is already in an unsteady solver:
http://www.fredo490.fr/public/rhoLTS...m-Cylinder.zip

I have found that for "coarse" mesh, this strategy is quite robust. However, for fine mesh you might have to play with the different relaxation number to get the data you want. Also, don't be afraid to use paraview to choose the best (the most realistic I would say) timeStep between the 1 and 2 solver.
fredo490 is offline   Reply With Quote

Old   April 23, 2013, 10:18
Default
  #10
Senior Member
 
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 236
Rep Power: 8
fredo490 is on a distinguished road
If you have a very fine mesh, you can also use rhoLTSPimpleFoam to initialize your case. I had a case with y+ = 0.1 that needed rhoLTSPimpleFoam ti be initialized. Just run few seconds of simulation and then use the solution (even not converged) as initialization of rhoSimplecFoam.
fredo490 is offline   Reply With Quote

Old   April 24, 2013, 02:14
Default
  #11
Member
 
Join Date: Oct 2012
Posts: 47
Rep Power: 4
sh.d is on a distinguished road
Quote:
Originally Posted by fredo490 View Post
If you have a very fine mesh, you can also use rhoLTSPimpleFoam to initialize your case. I had a case with y+ = 0.1 that needed rhoLTSPimpleFoam ti be initialized. Just run few seconds of simulation and then use the solution (even not converged) as initialization of rhoSimplecFoam.
hi fredo
thanks for your answer
i run my case with your boundary condition and relaxation factor and other but i can't run it.
there is this error:
-> FOAM FATAL IO ERROR:
Attempt to return dictionary entry as a primitive

file: /home/admin/OpenFOAM/admin-2.1.x/run/tutorials/compressible/rhoSimplecFoam/2test/constant/thermophysicalProperties::thermoType from line 20 to line 26.

From function ITstream& primitiveEntry::stream() const
in file db/dictionary/dictionaryEntry/dictionaryEntry.C at line 82.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::IOerror::abort() in "/opt/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 Foam::dictionaryEntry::stream() const in "/opt/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#3 Foam::basicPsiThermo::New(Foam::fvMesh const&) in "/opt/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#4
in "/opt/OpenFOAM/OpenFOAM-2.1.x/platforms/linux64GccDPOpt/bin/rhoSimplecFoam"
#5 __libc_start_main in "/lib64/libc.so.6"
#6
at /home/abuild/rpmbuild/BUILD/glibc-2.15/csu/../sysdeps/x86_64/elf/start.S:116
Aborted
?
Attached Files
File Type: zip 0.zip (6.5 KB, 10 views)
File Type: zip constant.zip (2.9 KB, 11 views)
File Type: zip system.zip (2.7 KB, 9 views)
sh.d is offline   Reply With Quote

Old   April 24, 2013, 08:12
Default
  #12
Senior Member
 
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 236
Rep Power: 8
fredo490 is on a distinguished road
After a quick look,
- your pRefCell 0; pRefPoint 0; pRefValue 0; while it should be your domain pressure (pressure 110000; ?).
- why did you remove the rho limiter ? rhoMin, rhoMax ...
- are you sure your mesh doesn't need any nNonOrthogonalCorrectors ?
- your nuTilda is initialized with "value uniform $turbulentK;" but there is no "turbulentK" variable in your initialConditions file.
- ...

many many mistakes.
fredo490 is offline   Reply With Quote

Old   April 24, 2013, 08:14
Default
  #13
Senior Member
 
HECKMANN Frédéric
Join Date: Jul 2010
Posts: 236
Rep Power: 8
fredo490 is on a distinguished road
plus, you try to use a OpenFoam 2.2 thermoType in a OpenFoam 2.1 solver... It cannot work because all the thermo model has been deeply changed.
fredo490 is offline   Reply With Quote

Reply

Tags
rhosimplefoam, spalartallmaras

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
Question about rhoSimpleFoam "if (transonic)" universez OpenFOAM 4 April 17, 2010 10:21
Problem with rhoSimpleFoam mecbe2002 OpenFOAM 3 April 11, 2010 00:54
TRANSONIC FLOW in RHOSIMPLEFOAM dinonettis OpenFOAM Running, Solving & CFD 9 October 21, 2009 12:02
RhoSimpleFoam FoamX spv24 OpenFOAM Running, Solving & CFD 1 July 21, 2008 10:29
Stability startup problems with rhoSimpleFoam olesen OpenFOAM Running, Solving & CFD 1 July 18, 2006 08:09


All times are GMT -4. The time now is 23:14.