Description: I am trying to r
 

Description:
I am trying to run samplDict in the dambreak tutorial and capture the pressure values on the leftwall using the surface option in sampleDict.

Solver/Application:
interFoam

Source file:
sampleDict

Testcase:
Dambreak

Platform:
Opensuse 11.0

Version:
OpenFoam version 1.5

Notes:
No output is generated. Problem could lie in the fact that there is insufficient documentation in section 6.3 as to how the wall patches are to be called hence the user maybe unclear as to how to correctly call the patches. For example, in blockmeshDict in the patch section, the walls are called as wall left wall etc. But that is conjecture only.

Additional comment by fellow Openfoam user:

------------------------------------------------------------
OpenFOAM Message Board: OpenFOAM: Running / Solving / CFD: About interFoam solver
------------------------------------------------------------

Posted by Michael Jaworski on Monday, February 23, 2009 - 09:46 pm:

Musa,
I am unable to get the "surface" portion of sample to work as well
(no files created). Perhaps someone out there has an example
dictionary. Otherwise, you'll have to dig into the source code to
determine the error.

There used to be a surfaceSample utility in 1.4.1. It's been removed
from 1.5, apparently. Looking for it in the old release might give you
a temporary fix.

Regards,
Mike J.

In 1.5.x I put in my surfaces
 

In 1.5.x I put in my surfaces section of system/sampleDict:

surfaces
(
leftWall
{
type patch;
patchName leftWall;
interpolate true;
triangulate true;
}
);

and that gives me surfaces/ddd/p_leftWall.vtk where ddd is the time.

Matt: Thanks for your respons
 

Matt:
Thanks for your response! if I understand it correctly the values are obtained by interpolation and triangulation. Is the triangulation / interpolation being done between the cell centers?

Musa

triangulation: per face. Does
 

triangulation: per face. Does not introduce any new vertices.
interpolation: from cell (or boundary face) to point (using distance weighted averaging).

Mattijs: I revised the samp
 

Mattijs:

I revised the sampleDict file as you suggested in your post
http://www.cfd-online.com/cgi-bin/OpenFOAM_Discus/show.cgi?tpc=126&post=32641#POST326 41

However, still no output for pressure p. In your post you refered to OpenFoam 1.5.x. Is there an updated version of OpenFoam available in which the sampleDict works? I am running OpenFoam 1.5 on openSUSE 11.0.

Also, is there a limit to the mesh size for which the sampleDict will work?
Looking forward to your response.

I found my problem earlier tod
 

I found my problem earlier today when I looked at the dictionary again: a typo. Make sure you specify a sampleFormat as raw or vtk or what-not. You can see this in the user guide online or in the source code for the sample utility.

Hi, i agree with Michael,
 

Hi,

i agree with Michael, even i am alos unig the same procedure for my case. with OF- 1.5,

Regards,

Vishal

Hello Musahossein, The 1.5.
 

Hello Musahossein,

The 1.5.x version is a source-only version downloadable using Git. See www.openfoam.org/download.html.

There is no limit on the mesh size apart from your computer's memory.

Hi Musaddeque, Here's a lin
 

Hi Musaddeque,

Here's a link to the file:
https://netfiles.uiuc.edu:443/mjawor...OAM/sampleDict

Good luck!

Mike J.

Michael: Thanks for your resp
 

Michael:
Thanks for your response. If you compare the command sturcture of the file you referred me to with the one in OpenFOAM 1.5, you will see that they are different. Either way, neither one works it does not generate any output. I will keep trying though.

Musa

Musa, Try changing the in
 

Musa,
Try changing the interpolation scheme to cellPointFace instead of just "cell". That might be the cause of your woes.

Also, I'd suggest putting a "setFormat raw;" line in there just in case it needs it.

Good Luck,
Mike J.

Mattijs After running OpenF
 

Mattijs

After running OpenFoam 1.5 interFoam solver for the dambreak problem, I used l -ual to check to see whether the sampleDict file had been accessed. l -ual sampleDict showed that the file had not been accessed during program run.

Any suggestions as to how to fix this will be appreciated.

Thanks
Musa

Musa, you're running the
 

Musa,
you're running the sample utility by typing "sample" in the case home directory, right?

-Mike

Mike: No. I have assumed th
 

Mike:

No. I have assumed that the interFoam solver will process the sampleDict file and generate output at each time step. Is that an incorrect assumption?.

Mike: THANKS!!! You were ri
 

Mike:

THANKS!!! You were right - didnt realize sampleDict acts as a post processor than something that runs at interFoam runtime. I typed in sample and a subdirectory called "surfaces" was created storing images of pressure and velocity at each time step. But i need to get numbers. How can I do that?

Musa, OpenFOAM is pretty m
 

Musa,
OpenFOAM is pretty modular. "blockMesh" is a pre-processing utility that reads a "blockMeshDict" file to build a mesh. "sample" is a post-processing tool to pull out numerical data from the mesh. Both of these are separate from any solver you might be using. You have to run them separately for them to do anything. Now, one *could* write a solver that automatically does something like what "sample" does, but I don't know that any of the solvers distributed with OF actually do this.

Try running the utility and that may solve all of your problems.

-Mike

Musa, With the "raw" data
 

Musa,
With the "raw" data format, there are some tab delimited data files created within the subdirectory for each time step. It's your choice what plotting program to use or other data analysis tools to analyze the data. I personally make use of gnuplot for pretty much everything I do.

There is an example of gnuplot usage here. It's your choice how to post-process the data, though.

Good luck,
Mike J.

Mike: I didnt realize that
 

Mike:

I didnt realize that .raw file as output by sampleDict is an text file with x, y,z and p (pressure values) in my case. However, in the dambreak case, if i want to look at the left wall, there should be only p values associated with y and no x or z. However, I see only x ordinates and y and z are zero. Also, my mesh is 100 (vertical) x 166 (horizontal) so there should be at the most 100 p values on the leftwall but the file header says:

"p" POINT_DATA 334, indicating 334 points.

Is there somthing wrong or am I not looking at the data correctly?

I look forward to your response.

Mike: Ignore the previous p
 

Mike:

Ignore the previous post. Silly mistake on my part.

Musa

It runs as a post processor. I checked to see if it runs during the solver runtime, and it shows that the file is not accessed during runtime. The only time it runs is after the processing is complete and the word sampleDict is typed at the prompt.