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

Rocket nozzle simulation with rhoCentralFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 11, 2015, 20:50
Default Rocket nozzle simulation with rhoCentralFoam
  #1
New Member
 
Hilbert
Join Date: Aug 2015
Location: Australia
Posts: 24
Rep Power: 3
Hillie is on a distinguished road
Dear Foamers

I have experience with CFX and want to switch over to OpenFOAM for my calculations. I keep running into the same problem and I am running out of idea's to fix it. (since am quite new to openfoam please call me out on any stupid mistakes I might have made).


I am currently trying to simulate a rocket nozzle with rhocentralfoam. For the velocity I have a fixedvalue inlet condition and an inletOutlet condition on the outlet. For the pressure I have a fixed value on the inlet and outlet. I am currently just running a laminar case to get the whole thing to work. I have made my mesh with netgen.


At normally the same time the solver crashed with the following message:


--> FOAM FATAL ERROR:
Maximum number of iterations exceeded


From function thermo<Thermo, Type>::T(scalar f, scalar T0, scalar (thermo<Thermo, Type>::*F)(const scalar) const, scalar (thermo<Thermo, Type>::*dFdT)(const scalar) const, scalar (thermo<Thermo, Type>::*limit)(const scalar) const) const
in file /home/hilbert/OpenFOAM/OpenFOAM-2.4.x/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 76.


FOAM aborting


#0 Foam::error:: printStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam::species::thermo<Foam::hConstThermo<Foam:: perfectGas<Foam::specie> >, Foam::sensibleInternalEnergy>::TEs(double, double, double) const at ??:?
#3 Foam::hePsiThermo<Foam: siThermo, Foam:: pureMixture<Foam::constTransport<Foam::species::th ermo<Foam::hConstThermo<Foam:; perfectGas<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::calculate() at ??:?
#4 Foam::hePsiThermo<Foam:siThermo, Foam:: pureMixture<Foam::constTransport<Foam::species::th ermo<Foam::hConstThermo<Foam:: perfectGas<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::correct() at ??:?
#5 ? at ??:?
#6 __libc_start_main in "/lib64/libc.so.6"
#7 ? at /home/abuild/rpmbuild/BUILD/glibc-2.18/csu/../sysdeps/x86_64/start.S:125


I have already tried to put the maximum number of iterations up, but that doesn't help.
From what I have read on this forum this error comes up when there are mesh issues.


To check this I have taken one of my meshes from my CFX calculations(which runs in CFX), and loaded that one into Openfoam. (slightly different geometry, same boundary conditions).


Now I get a very similar type of error.
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal: Solving for rhoUx, Initial residual = 0, Final residual = 0, No Iterations 0
diagonal: Solving for rhoUy, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver: Solving for Ux, Initial residual = 4.90935e-10, Final residual = 4.90935e-10, No Iterations 0
smoothSolver: Solving for Uy, Initial residual = 1.10525e-10, Final residual = 1.10525e-10, No Iterations 0
diagonal: Solving for rhoE, Initial residual = 0, Final residual = 0, No Iterations 0
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 ? in "/lib64/libc.so.6"
#3 Foam::hePsiThermo<Foam:siThermo, FoamureMixture<Foam::sutherlandTransport<Foam::s pecies::thermo<Foam::hConstThermo<Foam:erfectGas <Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ??:?
#4 Foam::hePsiThermo<Foam:siThermo, Foam:ureMixture<Foam::sutherlandTransport<Foam:: species::thermo<Foam::hConstThermo<Foam:erfectGa s<Foam::specie> >, Foam::sensibleEnthalpy> > > >::correct() at ??:?
#5 ? at ??:?
#6 __libc_start_main in "/lib64/libc.so.6"
#7 ? at /home/abuild/rpmbuild/BUILD/glibc-2.18/csu/../sysdeps/x86_64/start.S:125
Floating point exception


As a final check on my mesh I ran the following command on my mesh that ran in cfx(mesh generated with ICEMCFD):
checkMesh -allGeometry -allTopology


Checking geometry...
Overall domain bounding box (-11.505 -15 0) (11.505 36.6 1)
Mesh (non-empty, non-wedge) directions (1 1 0)
Mesh (non-empty) directions (1 1 0)
All edges aligned with or perpendicular to non-empty directions.
Boundary openness (-3.33549e-17 -4.40429e-17 1.23435e-14) OK.
Max cell openness = 2.63552e-14 OK.
Max aspect ratio = 368.724 OK.
Minimum face area = 3.82905e-09. Maximum face area = 0.125174. Face area magnitudes OK.
Min volume = 3.82905e-09. Max volume = 0.00618363. Total volume = 638.575. Cell volumes OK.
Mesh non-orthogonality Max: 19.9021 average: 8.25572
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.90249 OK.
Coupled point location match (average 0) OK.
Face tets OK.
*Edges too small, min/max edge length = 4.1539e-05 1, number too small: 2040
<<Writing 2040 points on short edges to set shortEdges
All angles in faces OK.
Face flatness (1 = flat, 0 = butterfly) : min = 1 average = 1
All face flatness OK.
Cell determinant (wellposedness) : minimum: 1.4384e-05 average: 2.44698
***Cells with small determinant (< 0.001) found, number of cells: 3546
<<Writing 3546 under-determined cells to set underdeterminedCells
Concave cell check OK.
Face interpolation weight : minimum: 0.0947609 average: 0.491795
Face interpolation weight check OK.
Face volume ratio : minimum: 0.104671 average: 0.971557
Face volume ratio check OK.


Failed 1 mesh checks.

Checkmesh seems to suggest a mesh issue, but if I look at my mesh statistics in icem is says that all element have a determinant between 0.95 and 1. Which would lead to the conclusion that there is an issue in the conversion script. (From icem I saved my mesh as a fluent file and used the fluentMeshToFoam utility to get my mesh)


This seems a bit unrealistic to me but I am a bit out of idea's. So if anybody have an other idea, that would be greatly appreciated.
Hillie is offline   Reply With Quote

Old   August 12, 2015, 06:24
Default
  #2
Member
 
Join Date: Jun 2012
Posts: 73
Rep Power: 6
maHein is on a distinguished road
This could be related to mesh issues, but does not have to (other examples: time stepping, wrong boundary conditions, ...). How does the solution look like just before the crash? Often, this helps in finding out where the error comes from.

Regards,

Martin
maHein is offline   Reply With Quote

Old   August 12, 2015, 21:12
Default
  #3
New Member
 
Hilbert
Join Date: Aug 2015
Location: Australia
Posts: 24
Rep Power: 3
Hillie is on a distinguished road
Hi Martin,

Thanks for your reply. That is were I am a bit puzzled, I can't find anything weird in the pressure, temp or velocity.

Checked time stepping, but I also get the same error with small time steps (1e-8).

Looking at the solution there is the most change at my inlet. At the my inlet I have a fixed value b.c for my velocity pressure and temperature, which looks oke to me.

Do you know of any other root causes for that error?

regards,
Hilbert
Hillie is offline   Reply With Quote

Old   August 13, 2015, 03:41
Default
  #4
Senior Member
 
anonymous
Join Date: Aug 2014
Posts: 198
Rep Power: 4
ssss is on a distinguished road
Well indeed if checkMesh fails then it means that there is a problem with the exporting process of your mesh. The error doesnt sound good.

Moreover, I would use a zeroGradient for your inlet p BC if you are planning to prescribe the inlet velocity

Is your case wedge?

You are using a compressible solver I suppose, so is the temperature 0 in somewhere of your domain?
ssss is offline   Reply With Quote

Old   August 14, 2015, 03:56
Default
  #5
New Member
 
Hilbert
Join Date: Aug 2015
Location: Australia
Posts: 24
Rep Power: 3
Hillie is on a distinguished road
Temperature looks fine. Also tried to put a total pressure bc on the inlet, but that was also to no avail. After some more experimentation on my mesh from icem I found the issue. The flow is accelerating in the first part of my domain. (first couple of mm) to very high speeds (were physically the flow shouldn't) and then the solver fails. I am still not really sure on what the root cause is though.
Hillie is offline   Reply With Quote

Old   August 14, 2015, 04:38
Default
  #6
Member
 
Join Date: Jun 2012
Posts: 73
Rep Power: 6
maHein is on a distinguished road
Is the flow subsonic at the inlet? In that case, I would set pressure and velocity at the same patch. I think this could be the source of error.
maHein is offline   Reply With Quote

Old   August 14, 2015, 05:02
Default
  #7
New Member
 
Hilbert
Join Date: Aug 2015
Location: Australia
Posts: 24
Rep Power: 3
Hillie is on a distinguished road
yes the flow is subsonic there. (I am initializing the flow subsonic through the entire domain).

Thanks for your tip, but i don't follow completely what you mean.

In my 2D domain my inlet and outlet are patches, my symmetry walls are empty, and the rest of my walls or of wall type.

On my Inlet I set both a fixedValue B.C on the pressure and velocity. Is this what you mean?
Hillie is offline   Reply With Quote

Old   August 14, 2015, 09:54
Default
  #8
Senior Member
 
mkraposhin's Avatar
 
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 11
mkraposhin is on a distinguished road
Hi, in my experience, rhoCentralFoam is not suitable for subsonic flows.

To overcome this limitation, i wrote hybrid solver, which you can download here

http://www.cfd-online.com/Forums/ope...ntralfoam.html

I'm interested in real life tests
mkraposhin is offline   Reply With Quote

Old   August 26, 2015, 21:00
Default
  #9
New Member
 
Hilbert
Join Date: Aug 2015
Location: Australia
Posts: 24
Rep Power: 3
Hillie is on a distinguished road
mkraposhin, thanks for your reply, I will look into it. The problem turned out to be the mesh in the end and not the solver. I though I would post how I worked through my issues for anybody else who has the same issue.

The first point was the boundary conditions. I supplied a fixed value boundary condition on the inlet for the pressure velocity and temperature. This overspecifies the problem, and therefore one should only specify a fixed value B.C for 2 of the 3 and the 3the one should be a zeroGradient.

The problem that I was left with was that all the inlet moment was not convected downsteam. Therefore very high velocities were obtained directly at the inlet. The same problem has also been posted on this forum elsewhere: http://www.cfd-online.com/Forums/ope...outlet-bc.html (no solution here though) . I have now rebuild most of my mesh with blockmesh and now the solver runs like a charm. So somehow my mesh make with icem, that runs well in CFX does not run with openfoam. I have to note here that I did switch to sonicfoam in the process of problem solving.

I havn't figured out yet what the underlying issue is, but it is a mesh issue.
Hillie is offline   Reply With Quote

Old   August 27, 2015, 05:54
Default
  #10
Member
 
Join Date: Sep 2014
Location: Germany
Posts: 74
Rep Power: 4
TobM is on a distinguished road
You have several cells with a determinant smaller than 0.001 in your mesh and you get a floating point error when using your cfx mesh.
I had a similar problem, although a different solver. Getting rid of the small determinants helped.
TobM is online now   Reply With Quote

Old   August 30, 2015, 19:34
Default
  #11
New Member
 
Hilbert
Join Date: Aug 2015
Location: Australia
Posts: 24
Rep Power: 3
Hillie is on a distinguished road
Hi TobM,

I gathered that from the checkmesh output. But I still find it a bit weird since I checked the determinanats in icem and icem told me that all determinants where greater that 0.9. Which in my view then means that the fluentMeshToFoam utility screws up the mesh.
Hillie 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
Simulation of a De Laval Nozzle RR16988 CFX 1 June 3, 2015 06:20
Problems with an overexpanded nozzle simulation nmtr FLUENT 0 April 11, 2015 07:01
2D Nozzle vapor simulation xof5006 FLUENT 0 December 18, 2012 22:51
Nozzle - Simulation converges, but data incorrect fade CFX 0 July 20, 2009 04:13
Need assistance in BC's for simulation of Vacuum cleaning nozzle bruce OpenFOAM Running, Solving & CFD 0 May 22, 2009 13:56


All times are GMT -4. The time now is 08:11.