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

Error with rhoCentralFoam in Shock tube

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

Like Tree1Likes
  • 1 Post By dhuckaby

Reply
 
LinkBack Thread Tools Display Modes
Old   January 1, 2013, 09:45
Exclamation Error with rhoCentralFoam in Shock tube
  #1
Member
 
Himanshu Sharma
Join Date: Jul 2012
Posts: 81
Rep Power: 4
himanshu28 is on a distinguished road
hi,

i have been working with the tutorial file of compressible flow in the open foam of Shock tube During the process the Mesh of the geometry is happening quiet easily but when i am running the solver it is giving me the error message as follows:
************************************************** *************
vaio@ubuntu:~/OpenFOAM/vaio-2.1.1/run/shockTube$ rhoCentralFoam
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.1.1-221db2718bbb
Exec : rhoCentralFoam
Date : Jan 01 2013
Time : 19:08:08
Host : "ubuntu"
PID : 5824
Case : /home/vaio/OpenFOAM/vaio-2.1.1/run/shockTube
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Reading thermophysical properties

Selecting thermodynamics package ePsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
Reading field U

Creating turbulence model

Selecting turbulence model type laminar
Reading thermophysicalProperties

fluxScheme: Kurganov

Starting time loop

#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 void Foam::divide<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh>(Foam::GeometricField<Foam::Vect or<double>, Foam::fvsPatchField, Foam::surfaceMesh>&, Foam::GeometricField<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/rhoCentralFoam"
#4 Foam::tmp<Foam::GeometricField<Foam::Vector<double >, Foam::fvsPatchField, Foam::surfaceMesh> > Foam:perator/<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh>(Foam::GeometricField<Foam::Vect or<double>, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/rhoCentralFoam"
#5
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/rhoCentralFoam"
#6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7
in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/rhoCentralFoam"
Floating point exception (core dumped)
vaio@ubuntu:~/OpenFOAM/vaio-2.1.1/run/shockTube$ ^C
vaio@ubuntu:~/OpenFOAM/vaio-2.1.1/run/shockTube$


I am new to the open foam and not able to find the solution of the problem if anybody has encountred the same problem please help in resolving the issue.:con fused:

Thanks
Himanshu..
himanshu28 is offline   Reply With Quote

Old   January 2, 2013, 06:11
Post
  #2
Senior Member
 
Tushar Chourushi
Join Date: Jul 2009
Location: IIT-Indore, India
Posts: 318
Blog Entries: 1
Rep Power: 8
Tushar@cfd is on a distinguished road
Hello,

Check the following thread, it will be helpful to you.

RhoCentralFoam detail

Best regards,
Tushar
Tushar@cfd is offline   Reply With Quote

Old   January 6, 2013, 04:10
Default
  #3
Super Moderator
 
praveen's Avatar
 
Praveen. C
Join Date: Mar 2009
Location: Bangalore
Posts: 244
Blog Entries: 6
Rep Power: 9
praveen is on a distinguished road
You are getting floating point exception due to negative pressure or density. Try changing the limiter or reducing time step or cfl number.
__________________
http://twitter.com/cfdlab
praveen is offline   Reply With Quote

Old   January 7, 2013, 16:41
Default
  #4
New Member
 
Join Date: Dec 2012
Posts: 3
Rep Power: 4
Lantiantiger is on a distinguished road
I've been having the exact same error as himanshu28. (Bear in mind, I'm running the tutorial file with NO modifications...)

Quote:
You are getting floating point exception due to negative pressure or density. Try changing the limiter or reducing time step or cfl number.
I tried reducing the timestep from 1e-6 to 1e-9, same error. Reducing maxCo from 0.2 to 0.02 also did not change the error.

Forgive me, I'm new to OpenFoam, but I can't figure out what you mean by limiter.
Lantiantiger is offline   Reply With Quote

Old   January 8, 2013, 06:40
Default
  #5
Member
 
Himanshu Sharma
Join Date: Jul 2012
Posts: 81
Rep Power: 4
himanshu28 is on a distinguished road
Quote:
Originally Posted by Lantiantiger View Post
I've been having the exact same error as himanshu28. (Bear in mind, I'm running the tutorial file with NO modifications...)



I tried reducing the timestep from 1e-6 to 1e-9, same error. Reducing maxCo from 0.2 to 0.02 also did not change the error.

Forgive me, I'm new to OpenFoam, but I can't figure out what you mean by limiter.
The limiter are termed as interpolation scheme while solving the hyperbolic PDEs to calculate from cell center to the face. for more details you ca refer to OPENFOAM user guide section 4.4.1. My problem is still not solved yet. If you get some result please share

Thanks
Himanshu
himanshu28 is offline   Reply With Quote

Old   January 8, 2013, 09:21
Question Error Persist..!!!
  #6
Member
 
Himanshu Sharma
Join Date: Jul 2012
Posts: 81
Rep Power: 4
himanshu28 is on a distinguished road
Quote:
Originally Posted by praveen View Post
You are getting floating point exception due to negative pressure or density. Try changing the limiter or reducing time step or cfl number.
hello,
thanks for reply

I have tryed your suggestions but the the error is still persist i am attaching the executable of shocktube if you can check it would be a great help.0.zip

system.zip
thank you
himanshu28 is offline   Reply With Quote

Old   January 8, 2013, 12:09
Default
  #7
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,186
Rep Power: 16
immortality is on a distinguished road
I have same this error with rhoCentralFoam for a long time.is rhoPimpleFoam more stable?
immortality is offline   Reply With Quote

Old   January 8, 2013, 14:06
Default
  #8
New Member
 
Join Date: Dec 2012
Posts: 3
Rep Power: 4
Lantiantiger is on a distinguished road
Alright, I've tried 10 different limiters, and I'm still getting the same error. The original limiter was linear, with reconstructs for rho, U, and T using vanLeer, vanLeerV, and vanLeer respectively. I commented out the reconstructs and tried different limiters for the default and still get the same error message.

I've also tried using the shockTube example in sonicFoam, same error message.
Lantiantiger is offline   Reply With Quote

Old   January 11, 2013, 15:49
Default
  #9
New Member
 
David Huckaby
Join Date: Jul 2009
Posts: 21
Rep Power: 7
dhuckaby is on a distinguished road
Hello Himanshu,

I think the problem is the initial conditions. According to your ./0 directory, your pressure is initialized to 0 (Pa) and the temperature 1 (K). It appears that you did not run "setFields" before running "rhoCentralFoam".

Dave
dhuckaby is offline   Reply With Quote

Old   January 12, 2013, 04:49
Default
  #10
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,186
Rep Power: 16
immortality is on a distinguished road
i dont want to use non homogenious initial condition so deleted setFieldsDict.is it ok?
immortality is offline   Reply With Quote

Old   January 14, 2013, 09:27
Default
  #11
New Member
 
David Huckaby
Join Date: Jul 2009
Posts: 21
Rep Power: 7
dhuckaby is on a distinguished road
You can use a homogeneous initial condition, but for the simulation to run, the initial pressure should be a positive number (1e5 Pa). The temperature might also need to be increased ( > 200K) due to the thermodynamic parameterization.
immortality likes this.
dhuckaby is offline   Reply With Quote

Old   January 16, 2013, 00:54
Default
  #12
Member
 
Himanshu Sharma
Join Date: Jul 2012
Posts: 81
Rep Power: 4
himanshu28 is on a distinguished road
Quote:
Originally Posted by immortality View Post
i dont want to use non homogenious initial condition so deleted setFieldsDict.is it ok?
Can you please tell me how to run a setfieldDict file the procedure i adopt s
is
$ blockMesh
$ <solver> /in this case rhoCentralFoam

what alterations i need to perform to run this case.Since i am new to open foam your guidance will help.

Thank You

Himanshu
himanshu28 is offline   Reply With Quote

Old   January 16, 2013, 05:37
Default
  #13
Senior Member
 
Bernhard Linseisen
Join Date: May 2010
Location: Magdeburg/Geneva
Posts: 176
Blog Entries: 1
Rep Power: 7
Linse is on a distinguished road
@immortality: If you have no gradients at any place, what flow would you have? So keeping a completely homogeneous case without any gradients or differing values in my opinion contradicts the principle of flow. But that is your decision to make.
The important thing indeed is that you need to have a case which has conditions acceptable to the solver.
If you really do not want to change anything via the setFieldsDict, please change 0/p and 0/T to reasonable values! Temperatures below 200 K are difficult to some of the thermodynamic libraries. And pressures below 1000 Pa most probably are below limits for using a control-volume approach as the FVM is one. (More info on that: Look for Knudsen-number and direct simulation monte carlo DSMC)

@himanshu28:
- The alteration you need to make should be simply running the command "setFields" just after blockMesh. Then your case should be set up correctly and you should have a nice shocktube simulation. The different pressure zones you can define within system/setFieldsDict.
- In general for working with the tutorials, it is advantageous to have a look into the "Allrun" file. Usually all the steps are conducted in the right order in there.
The basic approach actually would be to first conduct simply "./Allrun", then do the single steps from the Allrun-file by hand.
Linse is offline   Reply With Quote

Old   January 17, 2013, 08:25
Default Thanks alot !!!
  #14
Member
 
Himanshu Sharma
Join Date: Jul 2012
Posts: 81
Rep Power: 4
himanshu28 is on a distinguished road
Quote:
Originally Posted by Linse View Post
@immortality: If you have no gradients at any place, what flow would you have? So keeping a completely homogeneous case without any gradients or differing values in my opinion contradicts the principle of flow. But that is your decision to make.
The important thing indeed is that you need to have a case which has conditions acceptable to the solver.
If you really do not want to change anything via the setFieldsDict, please change 0/p and 0/T to reasonable values! Temperatures below 200 K are difficult to some of the thermodynamic libraries. And pressures below 1000 Pa most probably are below limits for using a control-volume approach as the FVM is one. (More info on that: Look for Knudsen-number and direct simulation monte carlo DSMC)

@himanshu28:
- The alteration you need to make should be simply running the command "setFields" just after blockMesh. Then your case should be set up correctly and you should have a nice shocktube simulation. The different pressure zones you can define within system/setFieldsDict.
- In general for working with the tutorials, it is advantageous to have a look into the "Allrun" file. Usually all the steps are conducted in the right order in there.
The basic approach actually would be to first conduct simply "./Allrun", then do the single steps from the Allrun-file by hand.
Hi linse,
Thank a lot for your guidance.

Regards
Himanshu..
himanshu28 is offline   Reply With Quote

Old   January 17, 2013, 14:15
Default
  #15
Senior Member
 
Mahdi Hosseinali
Join Date: Apr 2009
Posts: 124
Rep Power: 8
anishtain4 is on a distinguished road
Quote:
Originally Posted by Linse View Post
@immortality: If you have no gradients at any place, what flow would you have? So keeping a completely homogeneous case without any gradients or differing values in my opinion contradicts the principle of flow.
Actually that is one perfect way every developer uses when they are just crazy about a difficult bug, having no gradient does not contradict anything to prevent the simulation and produce error, if you don't have gradient but flow that is what you should call contradict.
anishtain4 is offline   Reply With Quote

Old   December 4, 2013, 14:06
Default
  #16
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,186
Rep Power: 16
immortality is on a distinguished road
I had an entry in the tube with higher pressure,then a gradient there was and movement occurred due to incoming fluid.
__________________
Injustice Anywhere is a Threat for Justice Everywhere.Martin Luther King.
To Be or Not To Be,Thats the Question!
The Only Stupid Question Is the One that Goes Unasked.
immortality 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
Shock tube simulation harish FLUENT 5 January 25, 2014 03:20
Modelling Shock Tube with Venting RCBlast Main CFD Forum 1 December 17, 2012 10:40
rhoCentralFoam not reflecting shock in Shock Tube? Astaria OpenFOAM Running, Solving & CFD 5 March 4, 2012 04:07
HLL Riemann Shock Tube Matlab Problem Luke F Main CFD Forum 1 July 7, 2009 13:44
shock tube validation AB Main CFD Forum 3 December 10, 2004 08:31


All times are GMT -4. The time now is 14:36.