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

Running dieselFoam error

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

Like Tree3Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   February 5, 2009, 12:56
Default Hi Hamed, in my point of vi
  #101
Member
 
Sebastian Vogl
Join Date: Mar 2009
Location: Munich, Germany
Posts: 62
Rep Power: 8
sebastian_vogl is on a distinguished road
Hi Hamed,

in my point of view dieselFoam seams to be a good choice for your problem, as far as I can understand your case.
This solver uses the Euler-Lagrange model for two phase flows, which means that the spray is represented by parcels.
If you use VTK files to to visualize your simulation, you should have a look for a folder "Lagrangian" or "defaultCloud". You need to include this in paraFoam for your visualization. It is definitely possible to see the particles in paraFoam.
You can also find the particles if you go into any time folder of your simulation and look for an folder "lagrangian" and in that there is a folder "defaultcloud". If you go into these, you will find the position, temperature, etc. of every parcel in the domain. These folders are the basis for the visualization.
If you want to understand the settings, which you have to make in a case when using dieselFoam, have a look at the following page, created by Mr Nordin:
http://openfoamwiki.net/index.php/Contrib_dieselFoam

The solver allows you to choose an evaporation model, which is appropriate for your situation, and the break up models.

I hope I could help you a little bit. If you have got further questions, feel free to ask.

Best regards,
Sebastian
sebastian_vogl is offline   Reply With Quote

Old   February 6, 2009, 09:03
Default Hi Sebastian, Thanks for your
  #102
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 8
haghajani is on a distinguished road
Hi Sebastian,
Thanks for your kind reply,
After running Aachenbomb case and using foamToVTK and opening the converted data ".../aachenbomb/VTK/lagrangian/defaultCloud" , in paraFoam3.3.0, I found a file "defaultCloud_..vtk", containing many other ".vtk" files. After clicking to open each of them, as you mentioned, some data will be added to "Data Arrays" of "Information" in "Object Inspector" bar. i.e, values for d, tTurb, m,..., n, Uturb, U. But I couldn't see any "C7H16 Liquid Jet" stream or even "C7H16 Droplet" distribution, using Filters as Glyph, Stream Tracer and Clip. (?if these or any other Filter need some settings please let me know?) Although, I could see values of C7H16 (I don't know if it is mass fraction Liquid or evaporated C7H16),Temp,...,U in ".../aachenBomb/VTK/aachenBomb_..vtk, in each desired time step.

I tried to follow >> You can also find the particles if you go ...<<, but couldn't find find the proper "reader", among ParaFoam suggested ones. :-(
I read the suggested page, thanks for that, but still, I do not understand how the "nparcel" really affects the solution? Does it have any relation with number of droplets in system?

To define a continuous mass flow rate at inlet during a period of time, should it be like;
massFlowRateProfile
(
(0 0.12)
(0.005 0.12)
);
By that, I meant, between time 0 to 0.005, a uniform mass flow rate of 0.12 Kg/s is coming to the domain from the orifice (d = 0.005 to 0.01). Am I in right way?

Thank you in advance,
Hamed
haghajani is offline   Reply With Quote

Old   February 6, 2009, 09:34
Default Dear all Can anybody explai
  #103
New Member
 
Lara Aleluia Reis
Join Date: Mar 2009
Posts: 9
Rep Power: 8
lara_areis is on a distinguished road
Dear all

Can anybody explain me what is this "Added gas mass" in the description below ? and what controls it?

Number of parcels in system | 0
Injected liquid mass....... | 0 mg
Liquid Mass in system...... | 0 mg
SMD, Dmax.................. | 0 mu, 0 mu
Added gas mass = -2.27904e+10 mg
Evaporation Continuity Error| -2.27904e+10 mg


thank you in advance

Lara Aleluia Reis
lara_areis is offline   Reply With Quote

Old   February 6, 2009, 09:52
Default Since you dont use the spray,
  #104
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 19
niklas will become famous soon enough
Since you dont use the spray, I would just ignore those numbers.

And they are only valid for closed volumes.

Added gas mass is the injected mass minus the liquid mass in the domain.
Ehsan.Mn likes this.
niklas is offline   Reply With Quote

Old   February 6, 2009, 11:12
Default Hi Hamed, For making the pa
  #105
Member
 
Sebastian Vogl
Join Date: Mar 2009
Location: Munich, Germany
Posts: 62
Rep Power: 8
sebastian_vogl is on a distinguished road
Hi Hamed,

For making the parcels, which represent the spray, visible you need to apply the Glyph filter to the lagrangian_VTK file after having uploaded it in parafoam.
Do it the following way:
-Open Parafoam
-click on File->open, open the folder VTK and upload the main VTK file, which has the name of your case, and click "apply".
-click again on File->open and open the folder lagrangian, which is in the VTK folder.
-apply the Glyph filter to the lagrangian VTK file and click "apply".
-Click on the register "display" of this filter and choose as "colored by" the diameter of the droplets
-Go back to the register "Properties" and set:
scalar: d
(Vector is not importaint now)
Glyphtype: Sphere
Scale mode: scalar
Set Scale Factor: maybe 1 or 2 (is a kind of zoom factor to make the droplets appear smaller or bigger)
Maximum number of points: If your spray consists of 10000 droplets use 10000

Then you should be able to see the droplets in your domain. There is no such file like "C7H16 Liquid Jet" or "C7H16 Droplet". The droplets in the lagrangian folder are your spray.


Some comments to the massflowRate Profile:
The first entry in the round brackets is the point of time in units seconds. The second entry is indeed a mass flow in units kg/s.
For understanding this mass flow rate profile take a piece of paper and a pencil. Draw an horizontal axis for the time and a vertical axis for the mass flow with units kg/s. Now, for your example, at time 0s you mark the value 0.12kg/s in the diagram and also for the time 0.005s mark the same value. As the solver interpolates linearly between these two reference values for all time steps between 0s and 0.005s you can connect both points in your diagram with a straight line. In your case you will have a rectangle, which represents the constant mass flow rate. The area under your function, which is the area of the rectangle, is the integration of the mass flow rate over time. This is the total mass you injected between 0s and 0.005s. You must make sure that this total mass is exactly the amount of mass you specified under the item "mass" in the injectorProperties file.
Your way to build up the mass flow rate profile should be to first specify the injection time (if it is the important value) and then multiply it with the mass flow rate. In your case 0.12kg/s * (0.005s-0s) = 0.0006kg. This is the mass you should specify in the injectorProperties file. If you want to inject more liquid you ether increase the injection time or the mass flow rate. But I guess you don't want the latter thing. So if your wish is to have a constant mass flow rate of 0.12kg/s then you first make sure how long your injection time is supposed to be and by multiplying it with the flow rate, as I just showed you, you receive the mass you will inject in the system.
If your mass, which you want to inject, is the important parameter and not the injection time, divide the total mass through your mass flow rate of 0.12k/s and you can see how long your injection time is allowed to be.
This value you have write in the injectorProperties file to the item "mass".

I cannot say, whether your total mass flow rate profile is correct, as I don't know how much mass you injected. But I think you can now find out yourself, whether your file is correct. If not, write me!

@Lara: I think the added gas mass is the mass of gas which was introduced to the continuous phase by evaporation of the droplets. In my simulation it is always a very small value of the order of 1e-10mg.

Best regards,
Sebastian
Ehsan.Mn likes this.
sebastian_vogl is offline   Reply With Quote

Old   February 6, 2009, 13:10
Default Dear Sebastian, Thanks for
  #106
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 8
haghajani is on a distinguished road
Dear Sebastian,

Thanks for your kind support;

By visualizing the parcels, Thank you again, I've got some insight into dieselfoam. Now I see the parcels.
Regarding your comprehensive description on massflowrate, I have also set the mass to 6e-4kg, then I have no more anxiety on its asymptotic behaviour during spray.

Best wishes,
Hamed
haghajani is offline   Reply With Quote

Old   February 9, 2009, 08:21
Default Hi, Is it possible to, don't
  #107
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 8
haghajani is on a distinguished road
Hi,
Is it possible to, don't use spray in dieselFoam (How to set spray-off? then, How we can define that the state of entry is liquid, not gas,?)?, just to study the spill of a liquid jet and study the probable break-up/atomization effect on the liquid stream.
haghajani is offline   Reply With Quote

Old   February 11, 2009, 05:37
Default Hi everybody I want to add (L
  #108
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 8
haghajani is on a distinguished road
Hi everybody
I want to add (Liquid Hydrogen) as a new Liquid in /src/thermophysicalModels/liquids.

To follow the instruction as http://openfoamwiki.net/index.php/ContribDieselFoamThermophysicalPropertiesLiqui d Properties , I have to provide the required coefficient for calculating rho_,pv_, ..., D_ in respective NSRDS functions. I surfed the web to find "Data Compilation Tables of Properties of Pure Compounds", which may/seems contain useful data to me, but no success! :-(
Would you please let me know, what shall I do, to define this new
liquid properties?

Best regards,
Hamed
haghajani is offline   Reply With Quote

Old   February 19, 2009, 10:45
Default Hi Sebastian, Finally, I fo
  #109
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 8
haghajani is on a distinguished road
Hi Sebastian,

Finally, I found the Liquid Hydrogen data and the coefficients, and added H2 Library to the existing liquid library of openFoam-1.5 . I tried to compile the new library as http://openfoamwiki.net/index.php/ContribDieselFoamThermophysicalPropertiesLiqui d, but many errors, saying,
...
/user/lib/../lib64/crt1.o: in function `_start`: (.text+0x20): undefined reference to `main'
Make/linux64GccDpOpt/H2O.o: In function `Foam::thermophysicalFunction::type() const':
H2O.C.text._ZNK4Foam22thermophysicalFunction4typeEv[Foam::thermophysicalFunction::typ e() const]+0x3) : undefined reference to `Foam::thermophysicalFunction::typeName'
Make/linux64GccDpOpt/H2O.o: In function `Foam::NSRDSfunc0::type() const':
H2O.C.text._ZNK4Foam10NSRDSFunction04typeEv[Foam::NSRDSfunc0::type() const]+0x3): undefined reference to 'Foam::NSRDSfunc0::typeName'
Make/linux64GccDpOpt/H2O.o: In function `Foam::NSRDSfunc1::type() const':
H2O.C.text._ZNK4Foam22NSRDSfunction14typeEv[Foam::NSRDSfunc1::type() const]+0x3): undefined reference to 'Foam::NSRDSfunc1::typeName'
Make/linux64GccDpOpt/H2O.o: In function `Foam::NSRDSfunc2::type() const':
H2O.C.text._ZNK4Foam22thermophysicalFunction4typeEv[Foam::NSRDSfunc2::type() const]+0x3): undefined reference to 'Foam::NSRDSfunc2::typeName'
Make/linux64GccDpOpt/H2O.o: In function `Foam::NSRDSfunc4::type() const':
H2O.C.text._ZNK4Foam22thermophysicalFunction4typeEv[Foam::NSRDSfunc4::type() const]+0x3): undefined reference to 'Foam::NSRDSfunc4::typeName'
Make/linux64GccDpOpt/H2O.o: In function `Foam::NSRDSfunc5::type() const':
H2O.C.text._ZNK4Foam22thermophysicalFunction4typeEv[Foam::NSRDSfunc5::type() const]+0x3): undefined reference to 'Foam::NSRDSfunc5::typeName'
Make/linux64GccDpOpt/H2O.o: In function `Foam::NSRDSfunc6::type() const':
H2O.C.text._ZNK4Foam22thermophysicalFunction4typeEv[Foam::NSRDSfunc6::type() const]+0x3): undefined reference to 'Foam::NSRDSfunc6::typeName'
Make/linux64GccDpOpt/H2O.o: In function `Foam::NSRDSfunc7::type() const':
H2O.C.text._ZNK4Foam22thermophysicalFunction4typeEv[Foam::NSRDSfunc7::type() const]+0x3): undefined reference to 'Foam::NSRDSfunc7::typeName'
...
Do you know what's the problem?
Best regards,
Hamed
haghajani is offline   Reply With Quote

Old   February 22, 2009, 14:51
Default Hi Foamers I have been tryi
  #110
Senior Member
 
Alexandre Pereira
Join Date: Mar 2009
Posts: 155
Rep Power: 8
alexandrepereira is on a distinguished road
Hi Foamers

I have been trying to run the aachenBomb tutorial of OpenFOAM-1.5.x with the settings of the tutorial and it crashed with the infamous janafThermo error ( too low temperature ) with ignition on and chemistry on;

So I have changed the laplacian settings from fvSchemes to Gauss linear limited 01, and the enthalpy calculation to Gauss upwind... same thing happens... :-(

janafThermo out of range....

Has anybody got any idea on what can be done to run this tutorial...?

thanks in advance

Best regards

Alex
alexandrepereira is offline   Reply With Quote

Old   February 25, 2009, 10:36
Default Hi Foamers Solved the issue
  #111
Senior Member
 
Alexandre Pereira
Join Date: Mar 2009
Posts: 155
Rep Power: 8
alexandrepereira is on a distinguished road
Hi Foamers

Solved the issue :

The default maxCo number in controlDict seems to be quite high, leading to a divergence ,janafThermo out of range with quite low temperatures.

In all the runs that i have tried, basic kinetics to full kinetics with combustion on, the maxCo=0.1 led to divergence;

I tried setting the enthalpy calculation in fvSchemes to Gauss upwind, the laplacianSchemes to Gauss limited Linear 01, and the pressure corectors in fvSolution to 4... no avail...

what I did was lowering the maxCo to 0.05... seem that this leeds to a stable calculation...

Now for one last question ( if anyone can answer it ... :-) )

I will try to simulate the spray combustion of a fuel blend of dymethylether and isooctane with dieselEngineFoam with a moving mesh, I will set the inert species to {}, and change the chem.inp to simulate the Zeldovich Kinetics of NO2 formation, as well as the kinetics of soot formation.

This is quite a heavy duty calculation, so I ask you more experienced Foam users of combustion codes, what should be my tentative maxCo for this calculation ( moving mesh, tumble and swirl motions ... ) one order of magnitude lower? about the same value ( 0.05) ?

What would you advise me to use ?

Is there any kind of "rule of thumb" for the selection of maximum Courant number in a simulation like this...?


"Current CFD wisdom" says that one should always avoid Courant numbers of 1 in a simulation, well , 0.1 was not enough for dieselFoam to converge... :-(

Any hints here... ?


Thanks in advance

Alex
alexandrepereira is offline   Reply With Quote

Old   February 25, 2009, 11:12
Default You should be able to run with
  #112
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 19
niklas will become famous soon enough
You should be able to run with a Co number of 0.1 without any problem.
Im using 0.3 most of the times and it works fine.

The problem...or difficulty with sprays is the timestep used at time of injection.
The timestep is based on the Courant number at previous timestep, so when the injection starts you will have a big biig change in the flow conditions.

If you have a big time step at the start of calculation, you will inject alot of high velocity high density mass that will transfer alot of momentum to the gas. If you also have evaporation, you can cool the gas too much, which will extract too much energy from the gas and lead to negative temperatures.

It is therefore good practise to reduce the timestep just before the injection to give the code a chance to adjust to the high speed liquid jet that is about to enter the domain.
niklas is offline   Reply With Quote

Old   February 25, 2009, 12:42
Default Hi Niklas Thanks for the hi
  #113
Senior Member
 
Alexandre Pereira
Join Date: Mar 2009
Posts: 155
Rep Power: 8
alexandrepereira is on a distinguished road
Hi Niklas

Thanks for the hint :-)

BRGDS

Alex
alexandrepereira is offline   Reply With Quote

Old   February 28, 2009, 13:40
Default Hi Foamers When i run diese
  #114
Senior Member
 
Alexandre Pereira
Join Date: Mar 2009
Posts: 155
Rep Power: 8
alexandrepereira is on a distinguished road
Hi Foamers

When i run dieselFoam or engineFoam, in thermophysicalProperties dictionary the inertSpecie is set to N2, meaning that N2 wont be allowed to react ( am i right here... ?) ;

I am currently using the 15 reaction model chem.inp_15.

What keyword must i set in the entry inertSpecie to study Zeldovich kinetics in the combustion process of a Diesel simulation...?

It is possible to do this... is it not... ?

Thanks in advance

Alex
alexandrepereira is offline   Reply With Quote

Old   February 28, 2009, 16:14
Default No, of course all species part
  #115
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 19
niklas will become famous soon enough
No, of course all species participate in the reactions.

Inert only means that the transport equation wont be solved.

Check YEqn.H
niklas is offline   Reply With Quote

Old   February 28, 2009, 17:05
Default Thanx a lot Niklas BRGDS
  #116
Senior Member
 
Alexandre Pereira
Join Date: Mar 2009
Posts: 155
Rep Power: 8
alexandrepereira is on a distinguished road
Thanx a lot Niklas

BRGDS

Alex
alexandrepereira is offline   Reply With Quote

Old   March 1, 2009, 12:49
Default Hi Niklas Sorry to bother y
  #117
Senior Member
 
Alexandre Pereira
Join Date: Mar 2009
Posts: 155
Rep Power: 8
alexandrepereira is on a distinguished road
Hi Niklas

Sorry to bother you again...

This is not about dieselFoam... so far so good, I have managed to run the case with all the options available, selection of droplet break up model, type of injector, chemistry kinetics... so far so good.

This is about the simpleEngine tutorial of http://powerlab.fsb.hr/ped/kturbo/Op...neTutorial.tgz

I untared the case and blockmeshed it and ran into the

keyword engineMesh is undefined in dictionary "/home/alex/Desktop/Simul/simpleEngine2/constant/engineGeometry" error, so i changed engineGeometry and added the engineMesh layered; entry

Ran engineFoam again and there was a core dump :

root@iskandhar:/home/alex/Desktop/simpleEngine# engineFoam
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.5 |
| \ / A nd | Web: http://www.OpenFOAM.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/
Exec : engineFoam
Date : Mar 01 2009
Time : 16:32:56
Host : iskandhar
PID : 7376
Case : /home/alex/Desktop/simpleEngine
nProcs : 1

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

Create mesh for time = -225

Selecting engineMesh layered
*** glibc detected *** engineFoam: munmap_chunk(): invalid pointer: 0x08176a98 ***
======= Backtrace: =========
/lib/tls/i686/cmov/libc.so.6(cfree+0x1bb)[0xb6b5092b]
/root/OpenFOAM/ThirdParty/gcc-4.3.1/platforms/linux/lib/libstdc++.so.6(_ZdlPv+0x 21)[0xb6d2a051]
/root/OpenFOAM/ThirdParty/gcc-4.3.1/platforms/linux/lib/libstdc++.so.6(_ZdaPv+0x 1d)[0xb6d2a0ad]
/root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so(_ZNK4Foam13primitiv eMesh22makeCellCentresAndVolsERKNS_5FieldINS_6Vect orIdEEEES6_RS4_RNS1_IdEE+0x4af )[0xb6fa876f]
/root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so(_ZNK4Foam13primitiv eMesh22calcCellCentresAndVolsEv+0x132)[0xb6fa88f2]
/root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so(_ZNK4Foam13primitiv eMesh11cellVolumesEv+0x38)[0xb6fa8a78]
/root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libfiniteVolume.so(_ZNK4Foam6fvMes h1VEv+0xc3)[0xb771fee3]
/root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libfiniteVolume.so(_ZN4Foam6fvMesh C2ERKNS_8IOobjectE+0x7f1)[0xb77426f1]
/root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libengine.so(_ZN4Foam10engineMeshC 2ERKNS_8IOobjectE+0x29)[0xb7f3a319]
/root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libengine.so(_ZN4Foam17layeredEngi neMeshC1ERKNS_8IOobjectE+0x29)[0xb7f418b9]
/root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libengine.so(_ZN4Foam10engineMesh2 9addIOobjectConstructorToTableINS_17layeredEngineM eshEE3NewERKNS_8IOobjectE+0x3a )[0xb7f49c0a]
/root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libengine.so(_ZN4Foam10engineMesh3 NewERKNS_8IOobjectE+0x6a6)[0xb7f3f8c6]
engineFoam[0x805e382]
/lib/tls/i686/cmov/libc.so.6(__libc_start_main+0xe0)[0xb6af9050]
engineFoam(_ZNK4Foam11regIOobject11writeObjectENS_ 8IOstream12streamFormatENS1_13 versionNumberENS1_15compressionTypeE+0xc9)[0x805d9e1]
======= Memory map: ========
08048000-080d8000 r-xp 00000000 08:01 1136587 /root/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/engineFoam
080d8000-080d9000 r--p 00090000 08:01 1136587 /root/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/engineFoam
080d9000-080da000 rw-p 00091000 08:01 1136587 /root/OpenFOAM/OpenFOAM-1.5/applications/bin/linuxGccDPOpt/engineFoam
080da000-081c2000 rw-p 080da000 00:00 0 [heap]
b61f1000-b61fa000 r-xp 00000000 08:01 12009769 /lib/tls/i686/cmov/libnss_files-2.6.1.so
b61fa000-b61fc000 rw-p 00008000 08:01 12009769 /lib/tls/i686/cmov/libnss_files-2.6.1.so
b6217000-b6219000 rw-p b6217000 00:00 0
b6219000-b621b000 r-xp 00000000 08:01 12009905 /lib/tls/i686/cmov/libutil-2.6.1.so
b621b000-b621d000 rw-p 00001000 08:01 12009905 /lib/tls/i686/cmov/libutil-2.6.1.so
b621d000-b6231000 r-xp 00000000 08:01 12009766 /lib/tls/i686/cmov/libnsl-2.6.1.so
b6231000-b6233000 rw-p 00013000 08:01 12009766 /lib/tls/i686/cmov/libnsl-2.6.1.so
b6233000-b6235000 rw-p b6233000 00:00 0
b6235000-b626a000 r-xp 00000000 08:01 4849994 /root/OpenFOAM/ThirdParty/openmpi-1.2.6/platforms/linuxGccDPOpt/lib/libopen-pal. so.0.0.0
b626a000-b626b000 r--p 00034000 08:01 4849994 /root/OpenFOAM/ThirdParty/openmpi-1.2.6/platforms/linuxGccDPOpt/lib/libopen-pal. so.0.0.0
b626b000-b626c000 rw-p 00035000 08:01 4849994 /root/OpenFOAM/ThirdParty/openmpi-1.2.6/platforms/linuxGccDPOpt/lib/libopen-pal. so.0.0.0
b626c000-b628f000 rw-p b626c000 00:00 0
b628f000-b62df000 r-xp 00000000 08:01 4850000 /root/OpenFOAM/ThirdParty/openmpi-1.2.6/platforms/linuxGccDPOpt/lib/libopen-rte. so.0.0.0
b62df000-b62e0000 r--p 00050000 08:01 4850000 /root/OpenFOAM/ThirdParty/openmpi-1.2.6/platforms/linuxGccDPOpt/lib/libopen-rte. so.0.0.0
b62e0000-b62e2000 rw-p 00051000 08:01 4850000 /root/OpenFOAM/ThirdParty/openmpi-1.2.6/platforms/linuxGccDPOpt/lib/libopen-rte. so.0.0.0
b62e2000-b62e8000 r-xp 00000000 08:01 1077921 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/liblagrangian.so
b62e8000-b62e9000 r--p 00005000 08:01 1077921 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/liblagrangian.so
b62e9000-b62ea000 rw-p 00006000 08:01 1077921 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/liblagrangian.so
b62ea000-b6359000 r-xp 00000000 08:01 4849986 /root/OpenFOAM/ThirdParty/openmpi-1.2.6/platforms/linuxGccDPOpt/lib/libmpi.so.0. 0.0
b6359000-b635a000 r--p 0006e000 08:01 4849986 /root/OpenFOAM/ThirdParty/openmpi-1.2.6/platforms/linuxGccDPOpt/lib/libmpi.so.0. 0.0
b635a000-b6361000 rw-p 0006f000 08:01 4849986 /root/OpenFOAM/ThirdParty/openmpi-1.2.6/platforms/linuxGccDPOpt/lib/libmpi.so.0. 0.0
b6361000-b6367000 rw-p b6361000 00:00 0
b6367000-b637b000 r-xp 00000000 08:01 1077937 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libz.so
b637b000-b637c000 r--p 00013000 08:01 1077937 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libz.so
b637c000-b637d000 rw-p 00014000 08:01 1077937 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libz.so
b637d000-b637e000 rw-p b637d000 00:00 0
b637e000-b63ed000 r-xp 00000000 08:01 1077954 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libtriSurface.so
b63ed000-b63ee000 r--p 0006e000 08:01 1077954 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libtriSurface.so
b63ee000-b63ef000 rw-p 0006f000 08:01 1077954 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libtriSurface.so
b63ef000-b650d000 r-xp 00000000 08:01 1077989 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libsampling.so
b650d000-b6510000 r--p 0011e000 08:01 1077989 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libsampling.so
b6510000-b6512000 rw-p 00121000 08:01 1077989 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libsampling.so
b6512000-b665f000 r-xp 00000000 08:01 1077946 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libfvMotionSolvers.so
b665f000-b6663000 r--p 0014d000 08:01 1077946 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libfvMotionSolvers.so
b6663000-b6665000 rw-p 00151000 08:01 1077946 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libfvMotionSolvers.so
b6665000-b6937000 r-xp 00000000 08:01 1077945 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libdynamicMesh.so
b6937000-b693a000 r--p 002d2000 08:01 1077945 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libdynamicMesh.so
b693a000-b693d000 rw-p 002d5000 08:01 1077945 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libdynamicMesh.so
b693d000-b693e000 rw-p b693d000 00:00 0
b693e000-b6ad4000 r-xp 00000000 08:01 1077935 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libmeshTools.so
b6ad4000-b6ad6000 r--p 00196000 08:01 1077935 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libmeshTools.so
b6ad6000-b6ad8000 rw-p 00198000 08:01 1077935 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libmeshTools.so
b6ad8000-b6ad9000 rw-p b6ad8000 00:00 0
b6ad9000-b6ae2000 r-xp 00000000 08:01 1622066 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/openmpi-1.2.6/libPstream.so
b6ae2000-b6ae3000 rw-p 00008000 08:01 1622066 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/openmpi-1.2.6/libPstream.so
b6ae3000-b6c27000 r-xp 00000000 08:01 12009567 /lib/tls/i686/cmov/libc-2.6.1.so
b6c27000-b6c28000 r--p 00143000 08:01 12009567 /lib/tls/i686/cmov/libc-2.6.1.so
b6c28000-b6c2a000 rw-p 00144000 08:01 12009567 /lib/tls/i686/cmov/libc-2.6.1.so
b6c2a000-b6c2d000 rw-p b6c2a000 00:00 0
b6c2d000-b6c41000 r-xp 00000000 08:01 12009774 /lib/tls/i686/cmov/libpthread-2.6.1.so
b6c41000-b6c43000 rw-p 00013000 08:01 12009774 /lib/tls/i686/cmov/libpthread-2.6.1.so
b6c43000-b6c45000 rw-p b6c43000 00:00 0
b6c45000-b6c51000 r-xp 00000000 08:01 1917202 /root/OpenFOAM/ThirdParty/gcc-4.3.1/platforms/linux/lib/libgcc_s.so.1
b6c51000-b6c52000 rw-p 0000b000 08:01 1917202 /root/OpenFOAM/ThirdParty/gcc-4.3.1/platforms/linux/lib/libgcc_s.so.1
b6c52000-b6c53000 rw-p b6c52000 00:00 0
b6c53000-b6c76000 r-xp 00000000 08:01 12009764 /lib/tls/i686/cmov/libm-2.6.1.so
b6c76000-b6c78000 rw-p 00023000 08:01 12009764 /lib/tls/i686/cmov/libm-2.6.1.so
b6c78000-b6d56000 r-xp 00000000 08:01 1917222 /root/OpenFOAM/ThirdParty/gcc-4.3.1/platforms/linux/lib/libstdc++.so.6.0.10
b6d56000-b6d5a000 r--p 000dd000 08:01 1917222 /root/OpenFOAM/ThirdParty/gcc-4.3.1/platforms/linux/lib/libstdc++.so.6.0.10
b6d5a000-b6d5b000 rw-p 000e1000 08:01 1917222 /root/OpenFOAM/ThirdParty/gcc-4.3.1/platforms/linux/lib/libstdc++.so.6.0.10
b6d5b000-b6d61000 rw-p b6d5b000 00:00 0
b6d61000-b6d63000 r-xp 00000000 08:01 12009763 /lib/tls/i686/cmov/libdl-2.6.1.so
b6d63000-b6d65000 rw-p 00001000 08:01 12009763 /lib/tls/i686/cmov/libdl-2.6.1.so
b6d6c000-b6d74000 r-xp 00000000 08:01 12009771 /lib/tls/i686/cmov/libnss_nis-2.6.1.so
b6d74000-b6d76000 rw-p 00007000 08:01 12009771 /lib/tls/i686/cmov/libnss_nis-2.6.1.so
b6d76000-b6d7d000 r-xp 00000000 08:01 12009767 /lib/tls/i686/cmov/libnss_compat-2.6.1.so
b6d7d000-b6d7f000 rw-p 00006000 08:01 12009767 /lib/tls/i686/cmov/libnss_compat-2.6.1.so
b6d7f000-b6d80000 rw-p b6d7f000 00:00 0
b6d80000-b7121000 r-xp 00000000 08:01 1077976 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so
b7121000-b712b000 r--p 003a0000 08:01 1077976 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so
b712b000-b712e000 rw-p 003aa000 08:01 1077976 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libOpenFOAM.so
b712e000-b7132000 rw-p b712e000 00:00 0
b7132000-b7159000 r-xp 00000000 08:01 1077969 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/liblaminarFlameSpeedModels.so
b7159000-b715a000 r--p 00026000 08:01 1077969 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/liblaminarFlameSpeedModels.so
b715a000-b715b000 rw-p 00027000 08:01 1077969 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/liblaminarFlameSpeedModels.so
b715b000-b715c000 rw-p b715b000 00:00 0
b715c000-b719c000 r-xp 00000000 08:01 1077929 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libspecie.so
b719c000-b719d000 r--p 00040000 08:01 1077929 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libspecie.so
b719d000-b719e000 rw-p 00041000 08:01 1077929 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libspecie.so
b719e000-b7319000 r-xp 00000000 08:01 1077930 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libcombustionThermophysicalModels. so
b7319000-b731c000 r--p 0017a000 08:01 1077930 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libcombustionThermophysicalModels. so
b731c000-b731d000 rw-p 0017d000 08:01 1077930 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libcombustionThermophysicalModels. so
b731d000-b7363000 r-xp 00000000 08:01 1077939 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libbasicThermophysicalModels.so
b7363000-b7364000 r--p 00046000 08:01 1077939 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libbasicThermophysicalModels.so
b7364000-b7365000 rw-p 00047000 08:01 1077939 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libbasicThermophysicalModels.so
b7365000-b74e3000 r-xp 00000000 08:01 1077931 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libcompressibleRASModels.so
b74e3000-b74e5000 r--p 0017e000 08:01 1077931 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libcompressibleRASModels.so
b74e5000-b74e7000 rw-p 00180000 08:01 1077931 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libcompressibleRASModels.so
b74e7000-b7ef3000 r-xp 00000000 08:01 1077926 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libfiniteVolume.so
b7ef3000-b7f0f000 r--p 00a0b000 08:01 1077926 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libfiniteVolume.so
b7f0f000-b7f13000 rw-p 00a27000 08:01 1077926 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libfiniteVolume.so
b7f13000-b7f18000 rw-p b7f13000 00:00 0
b7f18000-b7f5a000 r-xp 00000000 08:01 1077934 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libengine.so
b7f5a000-b7f5b000 r--p 00042000 08:01 1077934 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libengine.so
b7f5b000-b7f5c000 rw-p 00043000 08:01 1077934 /root/OpenFOAM/OpenFOAM-1.5/lib/linuxGccDPOpt/libengine.so
b7f5c000-b7f5e000 rw-p b7f5c000 00:00 0
b7f5e000-b7f78000 r-xp 00000000 08:01 12009494 /lib/ld-2.6.1.so
b7f78000-b7f7a000 rw-p 00019000 08:01 12009494 /lib/ld-2.6.1.so
bf937000-bf94c000 rw-p bf937000 00:00 0 [stack]
ffffe000-fffff000 r-xp 00000000 00:00 0 [vdso]
Aborted (core dumped)

I am using OpenFOAM-1.5

What do you suggest me to change in the case setup before trying to run this...?

You see, I am trying to set up a simulation of a free piston HCCI working on Dymethyl Ether in OpenFOAM...

I must first understand how do the mesh modifiers in engineFoam work before trying to set up an anarmonic periodic motion of the piston ( as it happens in a free piston engine ) in my case...

Could you help me setup the simpleEngineTutorial... ?

Thanks in advance

Alex
alexandrepereira is offline   Reply With Quote

Old   March 12, 2009, 15:23
Default hi all, when I reduce the int
  #118
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 8
haghajani is on a distinguished road
hi all,
when I reduce the internal pressure of domain to 1e+5 in liquid hydrogen spray into aachenbomb case, it gives a message of Maximum number of iterations exceeded#0; I reduced pressure from 5e+6 step by step, this error appeared from the pressure 1e+6.

What would be your suggestion, to this error,
Thanks in advance,
Hamed
haghajani is offline   Reply With Quote

Old   March 12, 2009, 15:37
Default I also, changed a lot with max
  #119
Member
 
Hamed Aghajani
Join Date: Mar 2009
Location: London, UK
Posts: 77
Rep Power: 8
haghajani is on a distinguished road
I also, changed a lot with maxIter_, and the tolerance in system/fvSolution;
haghajani 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
DieselFoam Spray Evaporation Continuity Error spv24 OpenFOAM Running, Solving & CFD 14 December 30, 2010 11:50
ERROR IN RUNNING THE FIRST EXAMPLE marhamat OpenFOAM Installation 8 August 27, 2006 04:13
FIDAP RUNNING ERROR "ERROR-DIR-NOT-EMPTY=145" BAOYU FLUENT 0 January 26, 2006 19:32
DieselFoam error turbulent dispersion adorean OpenFOAM Running, Solving & CFD 6 April 22, 2005 06:55
error while running UDF murthy FLUENT 1 October 22, 2001 05:02


All times are GMT -4. The time now is 06:27.