[rcastilla]

Hi, Kumar,
in fact, parasitic current are important in my case. I have found a way to reduce them. As this subject is so different to "contour plottings", I have open a new thread. Please, have a look in http://www.cfd-online.com/Forums/ope...tml#post234662 and give me your opinnion.

Best regards

Robert

[yannH]

Hi everyone,

Is there an other way to get surface elevation, I mean without using a personnal script ?

My goal is to have the distance between my still water level and the interface when alpha1 is 0.5.

thanks

Yann

[kumar]

Hello yannH,
It is possible to extract the elevation of the liquid interface without using a personal script in paraview. But you still have to run the sample script, which comes with OpenFoam. You can extract the isosurface as at alpha 0.50 and then write the solution in vtk format. Then open paraview (not paraFoam) and load the .vtk file. The you can can use the slice option to get a section of your surface. Then use the (select points on) option from the edit menu. Then use the (extract selection) filter from the filters menu. Then open another window on the same screen by using split horizontal option, then use spread sheet view.

This will give you the coordinates of the interFace based on the points you selected. This is an easy way of extraction of elevation of the interface.

hope it helps

[yannH]

Hi Kumar,

Thanks for replying, I succeed with your explaination (I'm just looking after how to create a plot using the spreadsheet)

Do you think it's possible, I mean not too hard, to implement a variable for surface elevation directly in my interDyMFoam code ? because it would be quite simple for postprocess my cases !

regards,

Yann

[krishnaprasad]

i am doing a wave tank problem in fluent. i have generated waves..i got wave elevation v/s tank length plot at iso-vof=o.5.. but i have a problem in ploting wave elevation v/s time..please help me.. it is urgent,,,...thank you in advance

[lindstroem]

Hi all,

I as well used the suggested code from ozgur. But I have a Problem: The genHOF.c doesnt finish the line "scanf("%f",&swl);" (round about line 20). I placed an output in the line afterwards, which was never reached.

The file height.dat is build, but empty and times contains all my timesteps.

Does anyone has an idea what might be wrong?

-> My fault.. I just have to enter it.. maybe sth was wrong in my input before...

Thanks in advance!

[duongquaphim]

Hi Krishna,

I think you can use sampleDict to extract isosurface plane at each time step in post-processing. Or more simple, just load data to paraview and plot the isosurface alpha = 0.5 in time.

Regards,

Duong

[cheng1988sjtu]

Hi ozgur,

I'm actually not so comfortable with the integration method. We can find it OK in theoretic work, but there are many grids in which the gamma are between 0 and 1.

moreover, when there are some special situations such as overturning, then the integration method should be invalid.

In fact, if we have enough nPoints in the sampling, I believe, the criteria gamma[n]>0.5, gamma[n+1]<0.5 may be a better choice.

Any opinions are welcome. Thank you!

Zhen Cheng

Originally Posted by ozgur

Hi Niels,

Thanks for the hints.. In fact I myself was suspicious about to locate gamma=0.5 (at least by a linear interpolation).

Anyway after some dirty coding, I managed to get following results for the sloshingTank2D3DoF tutorial.



The correct location of the free surface is important for me, because I want make comparisons with experimental results.

Ozgur



Just to complete, a sampled gamma data looks like this for an individual time step:


x y z gamma
0 0 -10 1
0 0 -9.69697 1
0 0 -9.39394 1
0 0 -9.09091 1
0 0 -8.78788 1
0 0 -8.48485 1
0 0 -8.18182 1
0 0 -7.87879 1
0 0 -7.57576 1
0 0 -7.27273 1
0 0 -6.9697 1
0 0 -6.66667 1
0 0 -6.36364 1
0 0 -6.06061 1
0 0 -5.75758 1
0 0 -5.45455 1
0 0 -5.15152 1
0 0 -4.84848 1
0 0 -4.54545 1
0 0 -4.24242 1
0 0 -3.93939 0.999999
0 0 -3.63636 0.999999
0 0 -3.33333 0.999999
0 0 -3.0303 0.998297
0 0 -2.72727 0.998297
0 0 -2.42424 0.998297
0 0 -2.12121 0.875845
0 0 -1.81818 0.875845
0 0 -1.51515 0.875845
0 0 -1.21212 0.251325
0 0 -0.909091 0.251325
0 0 -0.606061 0.251325
0 0 -0.30303 0.00170957
0 0 -4.10783e-15 0.00201351
0 0 0.30303 0.00201351
0 0 0.606061 0.00201351
0 0 0.909091 2.12627e-05
0 0 1.21212 2.12627e-05
0 0 1.51515 2.12627e-05
0 0 1.81818 5.35303e-08
0 0 2.12121 5.35303e-08
0 0 2.42424 5.35303e-08
0 0 2.72727 1.30219e-11
0 0 3.0303 1.30219e-11
0 0 3.33333 1.30219e-11
0 0 3.63636 1.03978e-16
0 0 3.93939 1.03978e-16
0 0 4.24242 1.03978e-16
0 0 4.54545 4.42707e-24
0 0 4.84848 4.42707e-24
0 0 5.15152 4.42707e-24
0 0 5.45455 3.07062e-36
0 0 5.75758 3.07062e-36
0 0 6.06061 3.07062e-36
0 0 6.36364 1.69305e-52
0 0 6.66667 1.69305e-52
0 0 6.9697 1.69305e-52
0 0 7.27273 -1.2664e-58
0 0 7.57576 -1.2664e-58
0 0 7.87879 -1.2664e-58
0 0 8.18182 -1.11574e-57
0 0 8.48485 -1.11574e-57
0 0 8.78788 -1.11574e-57
0 0 9.09091 -2.91388e-57
0 0 9.39394 -2.91388e-57
0 0 9.69697 -2.91388e-57
0 0 10 -2.91388e-57
0 0 10.303 -2.28496e-57
0 0 10.6061 -2.28496e-57
0 0 10.9091 -1.05445e-57
0 0 11.2121 -1.05445e-57
0 0 11.5152 -1.05445e-57
0 0 11.8182 -3.28503e-58
0 0 12.1212 -3.28503e-58
0 0 12.4242 -3.28503e-58
0 0 12.7273 -7.07185e-59
0 0 13.0303 -7.07185e-59
0 0 13.3333 -7.07185e-59
0 0 13.6364 -1.11157e-59
0 0 13.9394 -1.11157e-59
0 0 14.2424 -1.32059e-60
0 0 14.5455 -1.32059e-60
0 0 14.8485 -1.32059e-60
0 0 15.1515 -1.17364e-61
0 0 15.4545 -1.17364e-61
0 0 15.7576 -1.17364e-61
0 0 16.0606 -7.47976e-63
0 0 16.3636 -7.47976e-63
0 0 16.6667 -7.47976e-63
0 0 16.9697 -3.43373e-64
0 0 17.2727 -3.43373e-64
0 0 17.5758 -8.76047e-66
0 0 17.8788 -1.34639e-65
0 0 18.1818 -1.34639e-65
0 0 18.4848 -1.48939e-67
0 0 18.7879 -1.48939e-67
0 0 19.0909 -1.48939e-67
0 0 19.3939 -1.95727e-70
0 0 19.697 -1.95727e-70
0 0 20 -1.95727e-70

[Eliz]

Hi everybody,

I also try to plot surface elevation vs time and I copied Ozgur's C code, compiled and execute but it gives segmentation fault for some reason. Do you have any idea why it might happen?? Thanks in advance

Regards,
Eliz

[cheng1988sjtu]

please check the file name that you need to read and also the size of the dimensions in the code ( defaultly 15000, I think , but not sure, this number should be larger than the size of the file that you need to read) cheers!

Zhen

Originally Posted by Eliz

Hi everybody,

I also try to plot surface elevation vs time and I copied Ozgur's C code, compiled and execute but it gives segmentation fault for some reason. Do you have any idea why it might happen?? Thanks in advance

Regards,
Eliz

[Eliz]

Thanks for your reply Zhen, The dimensions are 1500 and the name of the file looks fine.

I run it by using "gdb" with the help of this link, to see what the error is,

http://www.unknownroad.com/rtfm/gdbtut/gdbsegfault.html

and it said "Source file name is more recent than executable" . Do you have any idea why it says so??any suggestions??Thanks a lot!!

Regards,
Eliz

[cheng1988sjtu]

Hi,

what format is the data file?

try to use vim to open the file and see if the first few lines are data or description words.

and make sure that the executive file (e.g> a.out) is in the right folder, :-)

Zhen

Originally Posted by Eliz

Thanks for your reply Zhen, The dimensions are 1500 and the name of the file looks fine.

I run it by using "gdb" with the help of this link, to see what the error is,

http://www.unknownroad.com/rtfm/gdbtut/gdbsegfault.html

and it said "Source file name is more recent than executable" . Do you have any idea why it says so??any suggestions??Thanks a lot!!

Regards,
Eliz

[Jane L]

Hi FOAMers!

I have another question related to this topic. I'm also using the sample-utility to write the values for alpha1 (gamma) along a line into files for each time step. This can be read easily by octave.
I figured out that sample takes the data along a line in the fixed coordinate system. In my case (sloshing in a tank) I would like to sample the data along a line in the relative coordinate system of the tank which is moved by solidBodyMotionFvMesh.
Does anyone know how to do that?

Thanks a lot!

[luchen2408]

hello,jane, I have the same problem with you ,I also need to make the plot of the liquid level with time, and I want to make the relative coordiate system moving with the model. Have you solved the problem?

[Jane L]

Hi luchen2408!

I hope my reply still helps a few days later. Go to the folder for the sample utility (OpenFOAM-2.1.1/applications/utilities/postProcessing/sampling/sample), make your own copy of that folder (for example relatveSample) and outcomment following lines in the *.C file:

// Handle geometry/topology changes
// polyMesh::readUpdateState state = mesh.readUpdate();

// sSets.readUpdate(state);
// sSurfs.readUpdate(state);

Make all necessary changes in the other files in that folder and compile with wmake. If everything worked fine, you can run your of relatveSample right after the calculation like the normal sample utility. You may have a look in the attached example which I called dynamicSample for some reasons

kind regards

[luchen2408]

hello,jane, I copy your attached file into my case, I look through the file, but I can't catch them very much. I input " wmake", but failed, I got following result,
Making dependency list for source file dynamicSample.C
SOURCE=dynamicSample.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-40 -I/opt/openfoam171/src/finiteVolume/lnInclude -I/opt/openfoam171/src/meshTools/lnInclude -I/opt/openfoam171/src/sampling/lnInclude -I/opt/openfoam171/src/surfMesh/lnInclude -I/opt/openfoam171/src/lagrangian/basic/lnInclude -IlnInclude -I. -I/opt/openfoam171/src/OpenFOAM/lnInclude -I/opt/openfoam171/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/dynamicSample.o
dynamicSample.C: In function ‘int main(int, char**)’:
dynamicSample.C:100:5: error: ‘addOption’ is not a member of ‘Foam::argList’
dynamicSample.C:112:26: error: ‘class Foam::argList’ has no member named ‘optionLookupOrDefault’
dynamicSample.C:112:52: error: expected primary-expression before ‘>’ token
dynamicSample.C:112:62: warning: left operand of comma operator has no effect [-Wunused-value]
dynamicSample.C:119:9: error: ‘MUST_READ_IF_MODIFIED’ is not a member of ‘Foam::IOobject’
dynamicSample.C:128:9: error: ‘MUST_READ_IF_MODIFIED’ is not a member of ‘Foam::IOobject’
make: *** [Make/linux64GccDPOpt/dynamicSample.o] Error 1
luch@ctcnwk843-ubuntu:~/Desktop/test/testheight/00/system/dynamicSample$

can you explain it more about it and how can I get the final result? Thanks very much

[luchen2408]

hello ,Dear Jane, I have tried the method you referred, I can wmake and generate a file--dynamicsample, when I run the file, I also got an error as following.
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time



--> FOAM FATAL IO ERROR:
cannot open file

file: /home/luch/Desktop/test/testheight/00/system/newdynamicSample/system/controlDict at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 61.

FOAM exiting

luch@ctcnwk843-ubuntu:~/Desktop/test/testheight/00/system/newdynamicSample$


after I copy the controlDict into the folder and run the file, I also got error:

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



--> FOAM FATAL ERROR:
No times selected

From function dynamicsample
in file db/Time/timeSelector.C at line 240.

FOAM exiting

luch@ctcnwk843-ubuntu:~/Desktop/test/testheight/00/system/newdynamicSample$


can you give me more hint ?how can I make it ? thanks

[Jane L]

Hi luchen!

Did does the ordinary "sample" utilty which comes with OpenFOAM give results? This was described in the previous posts.

Kind regards

[luchen2408]

Dear Jane,I have tried "sample" utility, it can give a height with the original coordinate system, however, my simulation object is moving, I have to make a local coordinate system with my object and give the sample with the local coordinate system,but I don't konw how to make it. do you have any suggestion?

[Jane L]

Hi Luchen,

so we're talking about the same problem
I faced the same problem as you do and I found that the "sample" utility gives the coordinates in the global inertial coordinate system. Therefore it needs to updade the geometry changes (movement). I disabled this updating progress so in the sample routine the movement of the geometry is not known and it writes the coordinates in the local system.
If the original sample works on vour machine you could try the following:
Outcomment the lines

// Handle geometry/topology changes
// polyMesh::readUpdateState state = mesh.readUpdate();

// sSets.readUpdate(state);
// sSurfs.readUpdate(state);

directly in the sample.C file without any renaming or copying. You have to run wmake in that folder to compilethe change in sample. If that works you may run sample after your simulation and check if the results are in a local coordinate system.

Which version of OF do you use by the way?

kind regards