[titio]

Hi Foamers,

I am having problems working with the sample utility in OpenFoam 1.6. I have downloaded the current version from the site, and installed following the instructions. I tested the installation doing a simulation, and everything went fine. However, when I tested the sample utility, using the example given in the UserGuide manual, it seems it did not worked.
I ran the case, and after that I typed sample in the main case directory. It ran without problems, at least no error message. However, it created no sets directory. I tried with sample -time xx, and no result again.
After this, I tried after recompiling the sample utility, that compiled with no problems, and the same problem occorred.
I am runing OpenFoam 1.6 in Ubuntu 8.1, and I have already done some development work, with a solver to model the flow of fluids with electroforetic effects. The results were good, but the sampling of results is hard, and with this difficulties with the sampling utility, even worse.

Can anyone help me out?

Regards,

Antonio Martins

[wyldckat]

Greetings Antonio,

Why don't you try using Mads cookbook (this thread)? I suggest trying the script version for Ubuntu 9.04, although I'm not 100% sure it will work with Ubuntu 8.10, although it should.
With that script, you can get the latest OpenFOAM 1.6.x that has multiple bug fixes since last July's 1.6 release and then you can make sure if the problems are related to an old bug or a pending bug in OpenFOAM!

As for your other thread about Paraview, it seems a bit strange... have you checked the md5 checksum of the downloaded packages? There have been issues with either downloading as well as unpacking files! And even disappearing files!
Try also getting the official Paraview binaries from www.paraview.org, and using foamToVTK to export the OpenFOAM case files to VTK format, and then opening with the official Paraview. It's not the perfect solution, but at least will get you going for a while!

edit: Try looking for solutions in this thread for your Paraview issues!

Best regards,
Bruno Santos

[titio]

Hi wyldckat,

Concerning the sample problem in OpenFoam 1.6, the same thing goes to OpenFoam 1.5. I followed the script you recomended, with no sucess. The same problem occurrs in version 1.5 of OpenFoam, the official one. The sample utility runs, the problem is that it does not generate a sets directory. I even tried with a sampleDict file with incorrect values, and it works without even giving a error of scales... without creating ounce again a sets directory. I am lost with this things, OpenFoam works, pos-processing is hell...

Regards,

António Martins

[examosty]

Hi António Martins,
I think it's very important to set the position of the line or point correct. It happened to me because of that.
Regards,
June

[heavy_user]

HI There,

the sampling utility also does NOT create an "sets" directory, when you request a parameter to be evaluated which is not present or which sample just cant process...or a location outside the domain....

If you try sampling components of U (like U.component(0) ) sample does not like it.
In this case you have to sample the U-vector and extract the desired component yourself.
( like this
sed 's/\t/ /g' z\=0_U.xy >new | cut new -d ' ' -f1,4 >U_z
)

regards

[catapult]

Hi,

I experience similar problems with U.components(n) or R.components(n) ....

a perhaps more elegant way to extract columns of a field (velocity component or Reynols stress component) :

awk '{print $1, $3}' input.agr > output.agr

extract the first column (coordinate for exemple) and third column (Uy for exemple) of the file. then :

xmgrace output.agr

Though you may need to edit the headers of the file.

Hope it helps

[martad]

You can also run

foamCalc <calcType> <fieldName1 ... fieldNameN>

so eg. for the velocity components

foamCalc components U

first, and then sample picks those up using sampleDict if written correctly.