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

sonicFoam not matching shock theory

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

Like Tree2Likes
  • 1 Post By Alan
  • 1 Post By alberto

Reply
 
LinkBack Thread Tools Display Modes
Old   April 19, 2010, 05:36
Default sonicFoam not matching shock theory
  #1
New Member
 
Alan Harrland
Join Date: Mar 2009
Posts: 21
Rep Power: 8
Alan is on a distinguished road
Hi all,

I am trying to use sonicFoam for some inviscid simulations, and my test case (supersonic flow over a wedge) does not seem to be following the analytical solution.

I am simulating a 14.03 deg wedge at Mach 7, sea level atmospheric conditions. If you look at the image below, it shows that the shock sits lower than the analytical solution (the line source).



I can adjust the thermophysical properties get the shock to sit in the right position, but this does not give me much faith in other solutions! My thermophysical properties are:

Code:
thermoType      ePsiThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>>;

mixture         air 1 28.96 1005 0 0 0.715;
If I adjust my cp I can get the shock to sit in the right position. I have also tried a finer mesh, but there is not change in shock position, so I do not believe it is a meshing issue.

Does anyone have any ideas as to what could be causing this? I have simulated the same wedge in other solvers (rhoCentralFoam and rhopSonicFoam) and the results match the analytical theory.

Thanks in advance for any help,
Alan
Alan is offline   Reply With Quote

Old   April 20, 2010, 02:25
Default
  #2
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Hello, I'm sorry to answer with a question: what does rhoSonicFoam does?

The major difference I can see between the solvers you used is that rhopSonicFoam and rhoCentralFoam solve for conserved variables, while sonicFoam does not.

I hope this additional test can help to clarify.

Best,
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   April 20, 2010, 04:57
Default
  #3
New Member
 
Alan Harrland
Join Date: Mar 2009
Posts: 21
Rep Power: 8
Alan is on a distinguished road
No problems at all Alberto, your help is much appreciated. Here is an image of the wedge simulated in rhoSonicFoam, as you can see shock lies in the correct position.



Thanks again,
Alan
Alan is offline   Reply With Quote

Old   April 22, 2010, 00:44
Default
  #4
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Interesting.

To exclude a possibility: in your run in rhoCentralFoam, did you set thermoPhysical properties to the same data you report for air (some tutorials use the normalised gas)?

Best,
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   April 24, 2010, 05:52
Default
  #5
New Member
 
Alan Harrland
Join Date: Mar 2009
Posts: 21
Rep Power: 8
Alan is on a distinguished road
Hi Alberto,

If I run the wedge in rhoCentralFoam with the same thermophysical properties as my sinicFoam case (i.e. not normalised) then the shock matches the theory. It appears to be a problem with the sonicFoam solver, as it gives the same (incorrect) shock position in both normalised and regular thermophysical properties.

Thanks again for your help, it is much appreciated.
immortality likes this.
Alan is offline   Reply With Quote

Old   April 24, 2010, 08:36
Default
  #6
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
If there is no bug, it might be related to how the equations are discretized, as I said before, but it's just a guess.

I'd suggest to use codes with the conservative form of the equations for shock capturing.

Best,
immortality likes this.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   April 26, 2010, 04:12
Default Try tutorial
  #7
Member
 
Join Date: May 2009
Posts: 31
Rep Power: 8
KrisT is on a distinguished road
I tried sonicFoam on OF-1.3, shock tube case in tutorial. It gives the wrong result (as said before, probably due to the fact that scheme is not conservative).

I checked against exact solution, obtained from C-code in the link below

http://num.math.uni-goettingen.de/kn...ro_ss2006.html

Haven't checked later versions (but that would be easy to do).
KrisT is offline   Reply With Quote

Old   April 26, 2010, 07:27
Default
  #8
New Member
 
Alan Harrland
Join Date: Mar 2009
Posts: 21
Rep Power: 8
Alan is on a distinguished road
So is there a way to fix this? sonicFoam seems to be the obly stable solver for my problem, the others seem to get anomalies in the solution that diverge
Alan is offline   Reply With Quote

Old   April 26, 2010, 09:11
Default
  #9
Member
 
Join Date: May 2009
Posts: 31
Rep Power: 8
KrisT is on a distinguished road
Quote:
Originally Posted by Alan View Post
So is there a way to fix this? sonicFoam seems to be the obly stable solver for my problem, the others seem to get anomalies in the solution that diverge
What kind of problems do you get with rhoCentralFoam? Have you tried varying CFL on that solver?
KrisT is offline   Reply With Quote

Old   April 26, 2010, 17:31
Default
  #10
New Member
 
Alan Harrland
Join Date: Mar 2009
Posts: 21
Rep Power: 8
Alan is on a distinguished road
Well, in rhoCentralFoam I am unable to progress the solution without it crashing within a few iterations (getting a maximum number of iterations exceeded error). This is the error I get:

Code:
Create time

Create mesh for time = 0.00264945

Reading thermophysical properties

Selecting thermodynamics package ePsiThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>>


Maximum number of iterations exceeded#0  Foam::error::printStack(Foam::Ostream&) in "/home/aharrland/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#1  Foam::error::abort() in "/home/aharrland/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so"
#2  Foam::ePsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::calculate() in "/home/aharrland/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libbasicThermophysicalModels.so"
#3  Foam::ePsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::ePsiThermo(Foam::fvMesh const&) in "/home/aharrland/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libbasicThermophysicalModels.so"
#4  Foam::basicPsiThermo::addfvMeshConstructorToTable<Foam::ePsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > > >::New(Foam::fvMesh const&) in "/home/aharrland/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libbasicThermophysicalModels.so"
#5  Foam::basicPsiThermo::New(Foam::fvMesh const&) in "/home/aharrland/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libbasicThermophysicalModels.so"
#6  main in "/home/aharrland/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/rhoCentralFoam"
#7  __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#8  _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/i386/elf/start.S:122


    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/dm2/henry/OpenFOAM/OpenFOAM-1.6/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 68.

FOAM aborting
Here is an image I get of the solution at the point of it crashing:



This is what the simulation looks like in rhopSonicFoam:



Note the 'stagnation' points at the top of the compression wedge. These slowly over the time of the solution go to zero, causing the time step (with adjust time step on) to go to a very large number.

Here is the simulation in sonicFoam:



This gives a nice stable solution, although with the incorrect shock angle.

I have a well refined, structured mesh, so I do not believe this to be the problem. This is also only a simple case which I need to expand to much more complex geometries, so the apparent stability of sonicFoam is quite appealing to me.

Thanks for your help KrisT.
Alan is offline   Reply With Quote

Old   April 26, 2010, 17:32
Default
  #11
New Member
 
Alan Harrland
Join Date: Mar 2009
Posts: 21
Rep Power: 8
Alan is on a distinguished road
Quote:
Originally Posted by KrisT View Post
What kind of problems do you get with rhoCentralFoam? Have you tried varying CFL on that solver?
No matter how small I make the CFL it still crashes.
Alan is offline   Reply With Quote

Old   April 26, 2010, 21:48
Default
  #12
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by Alan View Post
No matter how small I make the CFL it still crashes.
In rhoCentralFoam, what is giving troubles to you seems to be the energy equation, given the error message you obtain. Is it converging before the crash?

Are you performing inviscid runs in rhoCentralFoam? It seems to me the behaviour at the walls is different.

Additionally, could you show a zoom of the mesh with the solution under it (Surface with edges in paraview) around the tip of the triangle at the exit (where rhoCentralFoam has a sort of blue circle in the solution).

Best,
Alberto
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   April 26, 2010, 22:47
Default
  #13
New Member
 
Alan Harrland
Join Date: Mar 2009
Posts: 21
Rep Power: 8
Alan is on a distinguished road
Hi Alberto,

Im not sure what you mean by 'is it converging before the crash?'. Do you mean is the energy equation converging, or is the entire solution converging? I am solving this case as inviscid, as far as I am aware rhoCentralFoam is only an inviscid solver? My wall BC's are slip for the velocity file, and zeroGradient for p and T.

Here is the image that you asked for (note the flow is from left to right, so this is at the inlet, not the outlet):



I have also attached a similar picture around the entry to the isolator, which is the area of flow I believe is giving the solvers all the trouble.



Thanks again for your help Alberto, it is very much appreciated.

Alan
Alan is offline   Reply With Quote

Old   April 26, 2010, 23:04
Default
  #14
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by Alan View Post
Hi Alberto,

Im not sure what you mean by 'is it converging before the crash?'. Do you mean is the energy equation converging, or is the entire solution converging?
Yes, I'm asking if the energy equation is converging.

Quote:
I am solving this case as inviscid, as far as I am aware rhoCentralFoam is only an inviscid solver? My wall BC's are slip for the velocity file, and zeroGradient for p and T.
No, rhoCentralFoam can solve for both the inviscid and the viscous flow. Check the code (see flag "inviscid").

Quote:
Here is the image that you asked for (note the flow is from left to right, so this is at the inlet, not the outlet):
The grid seems good. Maybe it won't make any difference, but could you avoid having that tip touching the inlet conditions?

Best,
Alberto
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   April 27, 2010, 02:03
Default Ramp up Mach number?
  #15
Member
 
Join Date: May 2009
Posts: 31
Rep Power: 8
KrisT is on a distinguished road
Maybe I'm stupid here, but what happens if you ramp up the Mach number?

Would you get a stable solution for a lower Mach number? Is it possible to specify varying (increasing) inlet Mach number?

/j
KrisT is offline   Reply With Quote

Old   June 27, 2013, 07:10
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
Hi Alan
although a somewhat old thread.but I saw the same problem when a moving shock goes near the wall.residuals of U.x and h increases,although crashing doesn't occur.I use maxCo too.
has had anyone this problem too to share?
well,then sonicFoam solves only non-conservative form of equations.that was a very good information you gave to me!
__________________
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
HLL Riemann Shock Tube Matlab Problem Luke F Main CFD Forum 1 July 7, 2009 13:44
energy in sonicFoam joern OpenFOAM Running, Solving & CFD 0 June 16, 2009 15:53
Shock Fitting Craig FLUENT 1 April 24, 2008 17:06
Will compression waves overtake a moving shock? GRA Main CFD Forum 2 October 19, 2006 00:24
Shock capturing Dr B.M. Smith (Smith) OpenFOAM Running, Solving & CFD 1 December 10, 2004 06:40


All times are GMT -4. The time now is 05:24.