[OLAFLOW] The OLAFLOW Thread

VLima · June 4, 2018, 07:13

Thank you!

Quick question:

In the breakwater case, is it ok that the file GaugesP_p.xy is not present in the folder postProcessing/sets/0/ ? A warning is issued concerning the file.

Phicau · June 4, 2018, 07:30

Yes, it is totally normal, p does not exist at t = 0 s, it is created on the first step.

VLima · June 7, 2018, 10:22

Dear Pablo,

For some reason when running runCaseKEpsilon (or SST) I am now retrieving the following errors :

Processing and plotting variables
File "postSensVOF.py", line 42
print 'Sensor ' + '%i' % int(i+1) + ' of ' + '%i' % nSens + '.'
^
SyntaxError: invalid syntax
File "postSensPres.py", line 40
print 'Sensor ' + '%i' % int(i+1) + ' of ' + '%i' % nSens + '.'
^
SyntaxError: invalid syntax
Traceback (most recent call last):
File "plotSensVOF.py", line 8, in <module>
a = os.listdir(readPath)
FileNotFoundError: [Errno 2] No such file or directory: '/home/user/OpenFOAM/user-v1606+/run/tutorials/olaFlow/tutorials/breakwater/gaugesVOF'
Traceback (most recent call last):
File "plotSensPres.py", line 8, in <module>
a = os.listdir(readPath)
FileNotFoundError: [Errno 2] No such file or directory: '/home/user/OpenFOAM/user-v1606+/run/tutorials/olaFlow/tutorials/breakwater/sensorsPres

I did not perform any changes in any files.

Any idea why this error now and how to solve this?

Thank you very much in advance.

Phicau · June 7, 2018, 20:53

Hi Vania,

I think you are using Python 3. The postprocessing files are prepared to be run with Python 2.

Please run them manually with Python 2 or change the python executable in lines 67-70 of the runCase... script.

Best,

Pablo

VLima · June 11, 2018, 07:33

Dear Pablo,

I adapted the wavemaker input, as in wavemakerFlume with Piston, for the baseWaveFlume case.

I sampled several gauges along the flume, unfortunately there is a problem in the sampling and I get an error.

The log for the sampling :

Create time

Create mesh for time = 0

Reading set description:
GaugeVOF01
GaugeVOF02
GaugeVOF03
GaugeVOF04
GaugeVOF05

Time = 0

Time = 0.05

The terminal error:

...
Simulation complete.
Sampling free surface...
#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so"
#1 Foam::sigSegv::sigHandler(int) in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so"
#2 ? in "/lib64/libc.so.6"
#3 Foam::HashTable<Foam::regIOobject*, Foam::word, Foam::string::hash>::find(Foam::word const&) const in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so"
#4 Foam::MeshObject<Foam:ointMesh, Foam::UpdateableMeshObject, Foam:ointConstraints>::New(Foam:ointMesh const&) in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so"
#5 void Foam::volPointInterpolation::interpolate<double>(F oam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam:ointPatchField, Foam:ointMesh>&) const in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so"
#6 Foam::tmp<Foam::GeometricField<double, Foam:ointPatchField, Foam:ointMesh> > Foam::volPointInterpolation::interpolate<double>(F oam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::word const&, bool) const in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so"
#7 Foam::interpolationCellPoint<double>::interpolatio nCellPoint(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so"
#8 Foam::interpolation<double>::adddictionaryConstruc torToTable<Foam::interpolationCellPoint<double> >::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so"
#9 Foam::interpolation<double>::New(Foam::word const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so"
#10 Foam::sampledSets::volFieldSampler<double>::volFie ldSampler(Foam::word const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::PtrList<Foam::sampledSet> const&) in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libsampling.so"
#11 void Foam::sampledSets::sampleAndWrite<double>(Foam::sa mpledSets::fieldGroup<double>&) in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libsampling.so"
#12 Foam::sampledSets::write() in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libsampling.so"
#13 ? in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/bin/sample"
#14 __libc_start_main in "/lib64/libc.so.6"
#15 ? in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/bin/sample"
runCase: line 63: 784 Segmentation fault (core dumped) sample -dict system/sampleDictVOF > sampleVOF.log

Any idea what might be wrong in my settings?

Thank you very much in advance for your help.

Phicau · June 11, 2018, 22:14

Hi Vania,

did I understand correctly, your mesh is moving, right?

If I am not wrong the sampling utility fails because your mesh is moving and the utility does not update it. Therefore, the initial points in which you were sampling are possibly in new cells right now and this triggers an error.

You might solve this by sampling at runtime with a function object or by creating your own script in which you need to do:

Code:

sample -dict system/sampleDictVOF -time $timeFolderName

for all the times (timeFolderName) of your case.

Best,

Pablo

Phicau · June 24, 2018, 08:27

Dear all,

I have just included olaFlow in the Zenodo database to obtain a DOI. This identification system works in a similar way as the DOI of papers.

The DOI identifier for olaFlow is: https://doi.org/10.5281/zenodo.1297012

Important notice

Although no significant functionality changes have been introduced in the code during the preparation of the code for the DOI minting, the git history has been rewritten. This means that your local copy of olaFlow will not be able to obtain the latest updates in the usual manner.

Users are advised to download a fresh copy of the repository by running the following instruction in the terminal:

Code:

git clone git://github.com/phicau/olaFlow.git

Alternatively, advanced users also correct this by running:

Code:

git pull
git reset --hard origin/master
git pull origin master

After this, future updates will be available again.

Users who have made custom changes to the code and wish to continue getting updates may integrate them in the usual simple (e.g. copying and pasting their files) and advanced (e.g. git rebase) ways.

This is the official release announcement: https://sites.google.com/view/olaflo...og/olaflow-doi

VLima · July 5, 2018, 06:52

Dear Pablo,

I am trying to visualize the vertex numbers/indices of the wavemakerTank case (tried with Flume case too).

Doing paraFoam -block I get :

bash-4.1$ paraFoam -block
Created temporary 'wavemakerTank_teste.blockMesh'
fileName::stripInvalid() called for invalid fileName /home/user/Desktop/LinktoOpenFOAM/user-v1606+/run/tutorials/olaFlow/tutorials/wavemakerTank_teste/wavemakerTank_teste.blockMesh
For debug level (= 2) > 1 this is considered fatal

It is supposed to be possible to visualize with this option.

Any idea what might be causing this?

I would appreciate help or any other feasible suggestions to do this.

Many thanks in advance!

Phicau · July 5, 2018, 07:08

Hi Vania,

no idea, I have never used that option. However, this is a problem with paraFoam rather than with olaFlow, so I suggest that you open a thread here: https://www.cfd-online.com/Forums/openfoam-paraview/

Just a suggestion, try to move your case to the /home/user/ folder and try again.

Best,

Pablo

VLima · July 5, 2018, 07:14

Well that surprisingly worked!

Thank you!

dietlind · August 9, 2018, 03:42

Dear Pablo,

I am new to olaFlow and OpenFoam and just started running a few of the tutorials.
I have some issues when it comes to the wavemakerFlume tutorial (Piston wavemaker). I did not change anything in the files provided. I only added the sampling method from the breakwater tutorial to export the surface elevation.

I am able to run the simulation and there is no error occuring.

When I look at the results in Paraview and also in the surface elevation file, there is no wave generated.
The wavemakermovement.txt file is created and shows a changing in paddle position but still there is no change in surface elevation.

Do you have any idea what the problem might be?

Furthermore, when I want to adapt the data and use experimental data (wavemaker position), can I just change the data in the wavemakermovement.txt file and insert my data andthen run the case again or is there anything else that needs to be adjusted?

Kind regards,
Dietlind

Phicau · August 9, 2018, 06:11

Hi Dietlind,

which OpenFOAM version are you using? Are you sure that you are running the case with the olaDyMFlow solver?

If the case without changes works then you know that there is something wrong with the way you introduce the sampling procedure. Otherwise please come back to me with more details, there might be a bug somewhere.

Yes, you just need to edit the wavemakermovement.txt file and depending on the duration of your own signal, controlDict to set the endTime.

Best,

Pablo

dietlind · August 9, 2018, 09:23

Hi Pablo,

thanks for the quick reply. I am using Open Foam Version 2.4. I used the olaDyMFlow command to run the case.

Actually there was one minor change that I did to the transportProperties file because I always got an error saying "wrong token, expected word, found '['" in the line where sigma is specified. So I changed this line to

sigma sigma [1 0 -2 0 0 0 0] 0.07;

Then it worked. It was the same for the other tutorials I conducted. I run the baseWaveFlume and breakwater tutorial and there I also had to make this change in sigma but these two tutorials worked.

Furthermore, for the sampling I implemented the breakwater sampling to the baseWaveFlume tutorial to check if I had done it correctly and it worked.

In paraview also waves appeared for the baseWaveFlume and breakwater tutorial but not for the piston wave maker. The sampling was just to check if it was more an illustrative problem with paraview but that seems not to be the case.

I am not sure which information you need exactly to find out what the solution to that problem might be.

I attached the wavemakermovement.txt file which was created during the run aswell as the sampleDictVOF file I used. As an example of what I got from the sampling I added the file for gauge04.

I hope you can help me to solve this.
Thanks in advance!

wavemakerMovement.txt

sampleDictVOF.txt

GaugeVOF04.txt

Quote:

Originally Posted by Phicau

Hi Dietlind,

which OpenFOAM version are you using? Are you sure that you are running the case with the olaDyMFlow solver?

If the case without changes works then you know that there is something wrong with the way you introduce the sampling procedure. Otherwise please come back to me with more details, there might be a bug somewhere.

Yes, you just need to edit the wavemakermovement.txt file and depending on the duration of your own signal, controlDict to set the endTime.

Best,

Pablo

Phicau · August 9, 2018, 20:17

Hi Dietlind,

the olaFlow tutorials for version 2.4 and any older versions are in another repository, try those:

https://github.com/phicau/olaFlow_oldVersionTutorials

Pablo

arashghgood · August 24, 2018, 06:22

Dear Pablo

is it possible to plot the following in paraveiw after running olaflow examples?

the position of the crest of the wave
the position of the crest of the interacted waves
the changes of the width and so on

Phicau · August 24, 2018, 22:14

Hi Arash,

although I have never done that there is probably a way to do it, preview can do pretty complex analysis with the elevation, threshold and python programming filters.

I would suggest, however, that you export free surface elevation and perform such analysis in python/matlab, because it might be easier and more universal to apply to other of your cases.

Best,

Pablo

arashghgood · September 2, 2018, 16:53

Dear Pablo
How can I make two solitary waves with the same direction but with different properties such as amplitude and velocity so that they can interact with each other?

arashghgood · September 2, 2018, 16:57

Dear Pablo
is it possible to write my own solver based on my 1D or 2D equations in OpenFOAM or olaFlow to study a given problem?
In fact, I have an equation which is KdV type in 1D. I would like to solve and study my problem based on this equation.

Phicau · September 3, 2018, 01:28

Hi Arash,

there is a way to simulate this using olaFlow, solving the RANS equations. The process is as follows:
- Simulate the first solitary wave.
- See the log and stop the simulation at time equal to the reported equivalent wave period of the solitary wave.
- Duplicate the original simulation, remove all the time steps except the last one and rename it to be time 0.
- Change the solitary wave parameters and set rereadAlpha and rereadU to true in waveDict

Regarding solving KdV equation, yes, it can be implemented in a custom solver. You will also need to modify the olaFlow wave generation BCs to work with the new solver.

Good luck

Pablo

arashghgood · September 3, 2018, 09:56

Dear Pablo
Regarding solving KdV equation, which files and which parts of the files should be modified or changed?

June 4, 2018, 07:30		#42
Phicau Senior Member Pablo Higuera Join Date: Jan 2011 Location: Auckland Posts: 627 Rep Power: 19	Yes, it is totally normal, p does not exist at t = 0 s, it is created on the first step. __________________ Check out my new project: olaFlow --> The olaFlow Support Thread

June 7, 2018, 20:53		#44
Phicau Senior Member Pablo Higuera Join Date: Jan 2011 Location: Auckland Posts: 627 Rep Power: 19	Hi Vania, I think you are using Python 3. The postprocessing files are prepared to be run with Python 2. Please run them manually with Python 2 or change the python executable in lines 67-70 of the runCase... script. Best, Pablo __________________ Check out my new project: olaFlow --> The olaFlow Support Thread

June 11, 2018, 22:14		#46
Phicau Senior Member Pablo Higuera Join Date: Jan 2011 Location: Auckland Posts: 627 Rep Power: 19	Hi Vania, did I understand correctly, your mesh is moving, right? If I am not wrong the sampling utility fails because your mesh is moving and the utility does not update it. Therefore, the initial points in which you were sampling are possibly in new cells right now and this triggers an error. You might solve this by sampling at runtime with a function object or by creating your own script in which you need to do: Code: sample -dict system/sampleDictVOF -time $timeFolderName for all the times (timeFolderName) of your case. Best, Pablo __________________ Check out my new project: olaFlow --> The olaFlow Support Thread

June 24, 2018, 08:27		#47
Phicau Senior Member Pablo Higuera Join Date: Jan 2011 Location: Auckland Posts: 627 Rep Power: 19	Dear all, I have just included olaFlow in the Zenodo database to obtain a DOI. This identification system works in a similar way as the DOI of papers. The DOI identifier for olaFlow is: https://doi.org/10.5281/zenodo.1297012 Important notice Although no significant functionality changes have been introduced in the code during the preparation of the code for the DOI minting, the git history has been rewritten. This means that your local copy of olaFlow will not be able to obtain the latest updates in the usual manner. Users are advised to download a fresh copy of the repository by running the following instruction in the terminal: Code: git clone git://github.com/phicau/olaFlow.git Alternatively, advanced users also correct this by running: Code: git pull git reset --hard origin/master git pull origin master After this, future updates will be available again. Users who have made custom changes to the code and wish to continue getting updates may integrate them in the usual simple (e.g. copying and pasting their files) and advanced (e.g. git rebase) ways. This is the official release announcement: https://sites.google.com/view/olaflo...og/olaflow-doi __________________ Check out my new project: olaFlow --> The olaFlow Support Thread Last edited by Phicau; June 25, 2018 at 03:26.

July 5, 2018, 07:08		#49
Phicau Senior Member Pablo Higuera Join Date: Jan 2011 Location: Auckland Posts: 627 Rep Power: 19	Hi Vania, no idea, I have never used that option. However, this is a problem with paraFoam rather than with olaFlow, so I suggest that you open a thread here: https://www.cfd-online.com/Forums/openfoam-paraview/ Just a suggestion, try to move your case to the /home/user/ folder and try again. Best, Pablo __________________ Check out my new project: olaFlow --> The olaFlow Support Thread

June 4, 2018, 07:13		#41
VLima New Member Vania Join Date: Dec 2016 Posts: 13 Rep Power: 9	Thank you! Quick question: In the breakwater case, is it ok that the file GaugesP_p.xy is not present in the folder postProcessing/sets/0/ ? A warning is issued concerning the file.

June 7, 2018, 10:22		#43
VLima New Member Vania Join Date: Dec 2016 Posts: 13 Rep Power: 9	Dear Pablo, For some reason when running runCaseKEpsilon (or SST) I am now retrieving the following errors : Processing and plotting variables File "postSensVOF.py", line 42 print 'Sensor ' + '%i' % int(i+1) + ' of ' + '%i' % nSens + '.' ^ SyntaxError: invalid syntax File "postSensPres.py", line 40 print 'Sensor ' + '%i' % int(i+1) + ' of ' + '%i' % nSens + '.' ^ SyntaxError: invalid syntax Traceback (most recent call last): File "plotSensVOF.py", line 8, in <module> a = os.listdir(readPath) FileNotFoundError: [Errno 2] No such file or directory: '/home/user/OpenFOAM/user-v1606+/run/tutorials/olaFlow/tutorials/breakwater/gaugesVOF' Traceback (most recent call last): File "plotSensPres.py", line 8, in <module> a = os.listdir(readPath) FileNotFoundError: [Errno 2] No such file or directory: '/home/user/OpenFOAM/user-v1606+/run/tutorials/olaFlow/tutorials/breakwater/sensorsPres I did not perform any changes in any files. Any idea why this error now and how to solve this? Thank you very much in advance.

June 11, 2018, 07:33		#45
VLima New Member Vania Join Date: Dec 2016 Posts: 13 Rep Power: 9	Dear Pablo, I adapted the wavemaker input, as in wavemakerFlume with Piston, for the baseWaveFlume case. I sampled several gauges along the flume, unfortunately there is a problem in the sampling and I get an error. The log for the sampling : Create time Create mesh for time = 0 Reading set description: GaugeVOF01 GaugeVOF02 GaugeVOF03 GaugeVOF04 GaugeVOF05 Time = 0 Time = 0.05 The terminal error: ... Simulation complete. Sampling free surface... #0 Foam::error:rintStack(Foam::Ostream&) in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so" #1 Foam::sigSegv::sigHandler(int) in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so" #2 ? in "/lib64/libc.so.6" #3 Foam::HashTable<Foam::regIOobject*, Foam::word, Foam::string::hash>::find(Foam::word const&) const in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so" #4 Foam::MeshObject<Foam:ointMesh, Foam::UpdateableMeshObject, Foam:ointConstraints>::New(Foam:ointMesh const&) in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so" #5 void Foam::volPointInterpolation::interpolate<double>(F oam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam:ointPatchField, Foam:ointMesh>&) const in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so" #6 Foam::tmp<Foam::GeometricField<double, Foam:ointPatchField, Foam:ointMesh> > Foam::volPointInterpolation::interpolate<double>(F oam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::word const&, bool) const in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so" #7 Foam::interpolationCellPoint<double>::interpolatio nCellPoint(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so" #8 Foam::interpolation<double>::adddictionaryConstruc torToTable<Foam::interpolationCellPoint<double> >::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so" #9 Foam::interpolation<double>::New(Foam::word const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so" #10 Foam::sampledSets::volFieldSampler<double>::volFie ldSampler(Foam::word const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::PtrList<Foam::sampledSet> const&) in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libsampling.so" #11 void Foam::sampledSets::sampleAndWrite<double>(Foam::sa mpledSets::fieldGroup<double>&) in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libsampling.so" #12 Foam::sampledSets::write() in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/lib/libsampling.so" #13 ? in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/bin/sample" #14 __libc_start_main in "/lib64/libc.so.6" #15 ? in "/opt/OpenFOAM/OpenFOAM-v1606+/platforms/linux64GccDPInt32Opt/bin/sample" runCase: line 63: 784 Segmentation fault (core dumped) sample -dict system/sampleDictVOF > sampleVOF.log Any idea what might be wrong in my settings? Thank you very much in advance for your help.

July 5, 2018, 06:52		#48
VLima New Member Vania Join Date: Dec 2016 Posts: 13 Rep Power: 9	Dear Pablo, I am trying to visualize the vertex numbers/indices of the wavemakerTank case (tried with Flume case too). Doing paraFoam -block I get : bash-4.1$ paraFoam -block Created temporary 'wavemakerTank_teste.blockMesh' fileName::stripInvalid() called for invalid fileName /home/user/Desktop/LinktoOpenFOAM/user-v1606+/run/tutorials/olaFlow/tutorials/wavemakerTank_teste/wavemakerTank_teste.blockMesh For debug level (= 2) > 1 this is considered fatal It is supposed to be possible to visualize with this option. Any idea what might be causing this? I would appreciate help or any other feasible suggestions to do this. Many thanks in advance!

July 5, 2018, 07:14		#50
VLima New Member Vania Join Date: Dec 2016 Posts: 13 Rep Power: 9	Well that surprisingly worked! Thank you!

August 9, 2018, 03:42	WaveMakerFlume Tutorial	#51
dietlind New Member dietlind Join Date: Aug 2018 Posts: 4 Rep Power: 7	Dear Pablo, I am new to olaFlow and OpenFoam and just started running a few of the tutorials. I have some issues when it comes to the wavemakerFlume tutorial (Piston wavemaker). I did not change anything in the files provided. I only added the sampling method from the breakwater tutorial to export the surface elevation. I am able to run the simulation and there is no error occuring. When I look at the results in Paraview and also in the surface elevation file, there is no wave generated. The wavemakermovement.txt file is created and shows a changing in paddle position but still there is no change in surface elevation. Do you have any idea what the problem might be? Furthermore, when I want to adapt the data and use experimental data (wavemaker position), can I just change the data in the wavemakermovement.txt file and insert my data andthen run the case again or is there anything else that needs to be adjusted? Kind regards, Dietlind

August 9, 2018, 06:11		#52
Phicau Senior Member Pablo Higuera Join Date: Jan 2011 Location: Auckland Posts: 627 Rep Power: 19	Hi Dietlind, which OpenFOAM version are you using? Are you sure that you are running the case with the olaDyMFlow solver? If the case without changes works then you know that there is something wrong with the way you introduce the sampling procedure. Otherwise please come back to me with more details, there might be a bug somewhere. Yes, you just need to edit the wavemakermovement.txt file and depending on the duration of your own signal, controlDict to set the endTime. Best, Pablo __________________ Check out my new project: olaFlow --> The olaFlow Support Thread

August 9, 2018, 20:17		#54
Phicau Senior Member Pablo Higuera Join Date: Jan 2011 Location: Auckland Posts: 627 Rep Power: 19	Hi Dietlind, the olaFlow tutorials for version 2.4 and any older versions are in another repository, try those: https://github.com/phicau/olaFlow_oldVersionTutorials Pablo __________________ Check out my new project: olaFlow --> The olaFlow Support Thread

August 24, 2018, 06:22	How to plot the crest of the wave	#55
arashghgood Member Arash Join Date: Aug 2018 Posts: 31 Rep Power: 7	Dear Pablo is it possible to plot the following in paraveiw after running olaflow examples? the position of the crest of the wave the position of the crest of the interacted waves the changes of the width and so on

August 24, 2018, 22:14		#56
Phicau Senior Member Pablo Higuera Join Date: Jan 2011 Location: Auckland Posts: 627 Rep Power: 19	Hi Arash, although I have never done that there is probably a way to do it, preview can do pretty complex analysis with the elevation, threshold and python programming filters. I would suggest, however, that you export free surface elevation and perform such analysis in python/matlab, because it might be easier and more universal to apply to other of your cases. Best, Pablo __________________ Check out my new project: olaFlow --> The olaFlow Support Thread

Thread Tools	Search this Thread
Show Printable Version Email this Page	Search this Thread: Advanced Search
Display Modes
Linear Mode Switch to Hybrid Mode Switch to Threaded Mode

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Divergence detected in AMG solver: k when udf loaded	google9002	Fluent UDF and Scheme Programming	3	November 7, 2019 23:34
udf problem	jane	Fluent UDF and Scheme Programming	37	February 20, 2018 04:17
UDF velocity profile	willroca	Fluent UDF and Scheme Programming	2	January 10, 2016 03:13
Error messages	atg	enGrid	7	August 30, 2013 11:16
Phase locked average in run time	panara	OpenFOAM	2	February 20, 2008 14:37

September 2, 2018, 16:53	Solitary wave	#57
arashghgood Member Arash Join Date: Aug 2018 Posts: 31 Rep Power: 7	Dear Pablo How can I make two solitary waves with the same direction but with different properties such as amplitude and velocity so that they can interact with each other?

September 2, 2018, 16:57	Make Solver	#58
arashghgood Member Arash Join Date: Aug 2018 Posts: 31 Rep Power: 7	Dear Pablo is it possible to write my own solver based on my 1D or 2D equations in OpenFOAM or olaFlow to study a given problem? In fact, I have an equation which is KdV type in 1D. I would like to solve and study my problem based on this equation.

September 3, 2018, 01:28		#59
Phicau Senior Member Pablo Higuera Join Date: Jan 2011 Location: Auckland Posts: 627 Rep Power: 19	Hi Arash, there is a way to simulate this using olaFlow, solving the RANS equations. The process is as follows: - Simulate the first solitary wave. - See the log and stop the simulation at time equal to the reported equivalent wave period of the solitary wave. - Duplicate the original simulation, remove all the time steps except the last one and rename it to be time 0. - Change the solitary wave parameters and set rereadAlpha and rereadU to true in waveDict Regarding solving KdV equation, yes, it can be implemented in a custom solver. You will also need to modify the olaFlow wave generation BCs to work with the new solver. Good luck Pablo __________________ Check out my new project: olaFlow --> The olaFlow Support Thread

September 3, 2018, 09:56	kdv equ	#60
arashghgood Member Arash Join Date: Aug 2018 Posts: 31 Rep Power: 7	Dear Pablo Regarding solving KdV equation, which files and which parts of the files should be modified or changed?