sampleDict and controlDict

musahossein · November 15, 2014, 11:15

Dear all:

I am using OpenFoam 2.2.1 , InterDyMFoam/SloshingTank2D as follows:

I am running a code that will modify the displacement .dat file in OpenFoam/SloshingTank2D as follows: Each time the file is overwritten with 2 lines of data with a begin time and end time and corresponding displacements as follows:
2
(
( 0.19 (( 0.0265476475 0.00 0.00) ( 0.00 0.00 0.00)))
( 0.21 (( 0.0369661065 0.00 0.00) ( 0.00 0.00 0.00)))
)

The first column is time and the next column are the displacements associated with the time. Since both the time column and the displacement column will change as the new data is created, I would like to get an output at each end time (0.21 in this case). Can anyone suggest how I can use startFrom and stopAt to do this? In the OpenFoam Manual, for controlDict under "startFrom", there are options such as firstTime, startTime and latestTime options. so for example if the file previous to the one above is as follows:
2
(
( 0.17 (( -0.0665476475 0.00 0.00) ( 0.00 0.00 0.00)))
( 0.19 (( 0.0369661065 0.00 0.00) ( 0.00 0.00 0.00)))
)

Should I use the latestTime option? What about the stopAt option? looks like I only have the writeNow option. Is that correct? Any suggestions or comments would be appreciated, Thanks.

wyldckat · November 17, 2014, 16:22

Greetings Musaddeque,

If you have a certain code that generates the file for the movement, then you can also have that code generate a file that has the times for start and stop.
For example, the new file "system/controlDict.start_stop" would have this:

Code:

newStartTime 0.17;
newStopTime 0.19;

And your file "system/controlDict" would (for example) be something like this:

Code:

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#include "controlDict.start_stop"

application     icoFoam;

startFrom       startTime;

startTime       $newStartTime;

stopAt          endTime;

endTime         $newEndTime;

//....

I didn't add more lines, as I was only trying to exemplify the main detail.

This is further explained in the release notes for one of OpenFOAM's versions... er, I have no idea in which version of OpenFOAM this was included. OK, it's explained in the User Guide: http://www.openfoam.org/docs/user/ba...8-1040004.2.10 - section 4.2.10 The #include and #inputMode directives

Best regards,
Bruno

musahossein · November 18, 2014, 22:01

Thankyou very much for your response. I am trying that approach.

musahossein · November 22, 2014, 21:51

Quote:

Originally Posted by wyldckat

Greetings Musaddeque,

If you have a certain code that generates the file for the movement, then you can also have that code generate a file that has the times for start and stop.
For example, the new file "system/controlDict.start_stop" would have this:

Code:

newStartTime 0.17;
newStopTime 0.19;

And your file "system/controlDict" would (for example) be something like this:

Code:

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#include "controlDict.start_stop"

application     icoFoam;

startFrom       startTime;

startTime       $newStartTime;

stopAt          endTime;

endTime         $newEndTime;

//....

I didn't add more lines, as I was only trying to exemplify the main detail.

This is further explained in the release notes for one of OpenFOAM's versions... er, I have no idea in which version of OpenFOAM this was included. OK, it's explained in the User Guide: http://www.openfoam.org/docs/user/ba...8-1040004.2.10 - section 4.2.10 The #include and #inputMode directives

Best regards,
Bruno

I have made the code to do what you suggested. I have verfied that at each time step the start and end times in controlDict gets updated correctly. So I am running the case with 12 pieces of data, at time intervals of 0.02 seconds. However after generating for force file with time stamp of 0.08, OpenFOAM gives the following error and shuts down:

Code:

{stuff deleted}

#19    /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xf5) [0x7f7219c39de5]
#20    interDyMFoam() [0x43c56d]
[5] 
[5] 
[5] --> FOAM FATAL ERROR: 
[5] current time (0.12) is greater than the maximum in the data table (0.12)
[5] 
[5]     From function solidBodyMotionFunctions::tabulated6DoFMotion::transformation()[2] 
[2] 
[2] --> FOAM FATAL ERROR: 
[2] current time (0.12) is greater than the maximum in the data table (0.12)
[2] 
[2]     From function solidBodyMotionFunctions::tabulated6DoFMotion::transformation()
[2] [4] 
[4] 
[4] --> FOAM FATAL ERROR: 
[4] current time (0.12) is greater than the maximum in the data table (0.12)
[4] 
[4]     From function solidBodyMotionFunctions::tabulated6DoFMotion::transformation()
[4]     in file solidBodyMotionFvMesh/solidBodyMotionFunctions/tabulated6DoFMotion/tabulated6DoFMotion.C at line [3] 
[3] 
[3] --> FOAM FATAL ERROR: 
[3] current time (0.12) is greater than the maximum in the data table (0.12)
[3] 
[3]     From function solidBodyMotionFunctions::tabulated6DoFMotion::transformation()
[3]     in file solidBodyMotionFvMesh/solidBodyMotionFunctions/tabulated6DoFMotion/tabulated6DoFMotion.C[1] 

{stuff deleted}

What does this error mean? My code that is coupling with OpenFOAM provides start and end times with 0.02 second intervals, and the final time should be 0.12. Any suggestions will be greatly appreciated.

Thankyou

wyldckat · November 23, 2014, 16:35

Hi Musaddeque,

My guess is that this message:

Quote:

Code:

current time (0.12) is greater than the maximum in the data table (0.12)

is in fact referring to two different values, such as "0.120000001" and "0.120000000", respectively. This would easily lead to "0.120000001 > 0.120000000" being true.

A possible solution is to change your file to have something like this example, for 0.17 to 0.19:

Code:

4
(
(   0.16  ((   -0.0665476475   0.00   0.00)  (   0.00   0.00   0.00)))
(   0.17  ((   -0.0665476475   0.00   0.00)  (   0.00   0.00   0.00)))
(   0.19  ((   0.0369661065   0.00   0.00)  (   0.00   0.00   0.00)))
(   0.20  ((   0.0369661065   0.00   0.00)  (   0.00   0.00   0.00)))
)

This way you enforce that the values after the limits are still the ones you want/need.

Best regards,
Bruno

musahossein · November 23, 2014, 22:59

Quote:

Originally Posted by wyldckat

Hi Musaddeque,

My guess is that this message:
is in fact referring to two different values, such as "0.120000001" and "0.120000000", respectively. This would easily lead to "0.120000001 > 0.120000000" being true.

A possible solution is to change your file to have something like this example, for 0.17 to 0.19:

Code:

4
(
(   0.16  ((   -0.0665476475   0.00   0.00)  (   0.00   0.00   0.00)))
(   0.17  ((   -0.0665476475   0.00   0.00)  (   0.00   0.00   0.00)))
(   0.19  ((   0.0369661065   0.00   0.00)  (   0.00   0.00   0.00)))
(   0.20  ((   0.0369661065   0.00   0.00)  (   0.00   0.00   0.00)))
)

This way you enforce that the values after the limits are still the ones you want/need.

Best regards,
Bruno

Bruno:
The numbers that my code sends to openfoam -- startTime, endTime, and the displacements are all followed by "0d0" after the last digit. This will ensure that there are no unintended digits. So if an updated time is 0.12, then the code will send 0.120d0, i.e. 0.1200000...to the end. Maybe that is where the conflict was. Even when I set the writeinterval in controlDict to 0.0005, the last OpenFoam time would be 0.1195 -- never quite reaching 0.1200. So what I did was subtract a small number say 0.0001 from the start time and add the same number to the end time in the displacement file, so that my displacement file would look like:

2
(0.1200001 (0, start_displacement) .... other columns deleted)
(0.1400001 (0, end_dispalcement)......other columns deleted)

However, in the controlDict file, the startTime and endTime are kept as

0.1200 and 0.1400.

Given a larger time range in the displacement file, OpenFOAM now accepts the update and does the analysis w/o problems (well until the next time). So thank you for your suggestion. But may I suggest that OpenFOAM standardize the way numbers are dealt with so it keeps track of significant digits and sets all other numbers after it to zero. I am sure this way errors such as the one I came across can be avoided. I am not sure though, however, why OpenFOAM refused to write data after 0.1195, eventhough the write interval was 0.0005, and there was a displacement associated with 0.1200000.

musahossein · November 27, 2014, 12:39

Quote:

Originally Posted by musahossein

Bruno:
The numbers that my code sends to openfoam -- startTime, endTime, and the displacements are all followed by "0d0" after the last digit. This will ensure that there are no unintended digits. So if an updated time is 0.12, then the code will send 0.120d0, i.e. 0.1200000...to the end. Maybe that is where the conflict was. Even when I set the writeinterval in controlDict to 0.0005, the last OpenFoam time would be 0.1195 -- never quite reaching 0.1200. So what I did was subtract a small number say 0.0001 from the start time and add the same number to the end time in the displacement file, so that my displacement file would look like:

2
(0.1200001 (0, start_displacement) .... other columns deleted)
(0.1400001 (0, end_dispalcement)......other columns deleted)

However, in the controlDict file, the startTime and endTime are kept as

0.1200 and 0.1400.

Given a larger time range in the displacement file, OpenFOAM now accepts the update and does the analysis w/o problems (well until the next time). So thank you for your suggestion. But may I suggest that OpenFOAM standardize the way numbers are dealt with so it keeps track of significant digits and sets all other numbers after it to zero. I am sure this way errors such as the one I came across can be avoided. I am not sure though, however, why OpenFOAM refused to write data after 0.1195, eventhough the write interval was 0.0005, and there was a displacement associated with 0.1200000.

In order to "force" OpenFOAM to create files at 0.02 second intervals, I noted that if I tweaked the start time be subtracting 0.00001 seconds to it and adding the same to the end time, OpenFOAM would run without crashing and ceate time files at 0.02 second intervals. But alas I was mistaken. I put in 2000 data points (0.02 second intervals). Now OpenFOAM still does not write at 0.02 second intervals after 21 seconds into the data, which is approx half way into the run. Instead of creating files at 21.70 and 21.72 seconds, it creates a file 21.71999999 seconds. I have no idea how it comes up with this precision. It seems like no matter what time I put for the data write interval in controlDict, OpenFOAM will do what it will! Any suggestions?

musahossein · November 27, 2014, 16:33

As a follow up to the previous thread, in control dict I specify the write time as 0.02 as shown below:

Code:

 FoamFile
 {
 version     2.0;
 format      ascii;
 class       dictionary;
 location "system";
 object      controlDict;
 }
 // * * * * * * * * new file * * * * * * * * * * * * * * * * * * * * * * * * * * //
 application     interDyMFoam;
 startFrom         latestTime;
 startTime  21.70000;
 stopAt endTime;
 endTime  21.72000;
 deltaT 0.0005;
 writeControl    adjustableRunTime;
 writeInterval 0.02;
 purgeWrite 0;
 writeFormat     ascii;
 writePrecision 6;
 writeCompression compressed;
 timeFormat      general;
 timePrecision 6;
 runTimeModifiable yes;
 adjustTimeStep  yes;
 maxCo 0.5;
 maxAlphaCo 0.5;
 maxDeltaT 1;

But during OpenFoam run, I end up with the following time stamp on the oputput files:

Code:

.
.
.
21.68
21.7199999999

Looks like it not only missed writing output at 21.70, but it didnt quite get to 21.72.

Any suggestions advice would be greatly apprciated. Thanks!

wyldckat · January 25, 2015, 12:21

Hi Musaddeque,

Sorry, I wasn't able to look into this any sooner. And I know there is a bug report related to this issue, but I haven't found it yet.

OK, the latest error seems to be because the time snapshot 21.70 doesn't exist and because you have these settings:

Code:

startFrom         latestTime;
 startTime  21.70000;
 endTime  21.72000;
timePrecision 6;

But since you have only these time folders:

Code:

21.68
21.7199999999

Then it's not able to 21.70 because it doesn't exist and it's not able to find "21.7199999999" because it has a precision higher than 6... although I'm not certain about this one.

Can you please provide a test case? Because I'm not able to reproduce this error.

Best regards,
Bruno

edit: OK, found it: http://www.cfd-online.com/Forums/ope...ct-number.html

musahossein · January 25, 2015, 16:56

WyldKat:

Thanks for your response. I cant provide a test case as I have coupled at program with openfoam. The program looks for specific files with specific time stamps. As a result, if it does not find the file 27.72 for example, it will give an error. I got around this problem for the time being by:
1.Increasing the time stamp by a range. So for example, instead of supplying the start time as 2.00 seconds of simulation time, I will supply 1.999999. Similarly, I will increase the end time by a small amount say 0.0001. So the code now looks for something within that range.
2. Increasing the writPrecision in controlDict to 6.

Both these appear to help and I have running simulations w/o problems on this issue. I will try OpenFOAM version 2.3 soon.

Thanks

rocap · June 4, 2015, 16:00

Dear all.

I have the same type of problem as musahossein. I’am working on foam-extend 3.1 on a turbine simulation. I am using pimpleDyMFoam to solve the simulation.

What I need to do now, is to set probes on one face of the blades. But probes can’t be fixed. I need them to follow the blades to always get the pressure at the good point.

I read all your previous post but I could not fix my problem.

Do you have an idea about the way I can do this? It also need to be run in parallel. I don’t know if it’s possible with this “moving” probes.

Best Regards
Romain

wyldckat · June 12, 2015, 19:38

Greetings Romain and welcome to the forum!

AFAIK, "moving probes" is only somewhat implemented in OpenFOAM 2.2.x and newer: http://www.openfoam.org/mantisbt/view.php?id=1090
It's in this commit: https://github.com/OpenFOAM/OpenFOAM...f27b5d573c2a9b

I don't know if this feature has been back-ported to foam-extend already or not.

Best regards,
Bruno

okcfdlab · June 16, 2015, 20:44

Sample can be run in parallel on a decomposed case in exactly the same manner as the case itself is run in parallel.

For instance, if you have a case decomposed into four processor directories, you can run sample in parallel on four processors by

mpirun -np 4 sample -parallel

This is much faster than running reconstructPar and then sample.

rocap · June 18, 2015, 12:36

Dear Bruno

Thanks for your reply and your help. I will try it and I will let you know

regards

gautami · August 14, 2015, 07:27

Dear All,

I am working on the interDyMFoam/floatingObject tutorial. I need guidance with post processing. I am trying to get fluid velocities and acceleration values at specific points in the computational domain.

1.In the "sampleDict/controlDict" file can I use the option "type cloud" and read the points from a file.
2.Is it possible to get the acceleration data for these specific points by using "fields" (as U for velocity).

Thank you.

gautami · August 17, 2015, 13:39

Dear Mr Bruno,

I am trying to use sampleDict utility with cloud of points option. Kindly can you please guide me as to how I could read the coordinates of the cloud points form a data file (as I need to track up to 150 points). Your help is highly appreciated.Thank you.

Regards,
Gautami.

wyldckat · August 18, 2015, 15:08

Quick answers:

Quote:

Originally Posted by gautami

1.In the "sampleDict/controlDict" file can I use the option "type cloud" and read the points from a file.

...and...

Quote:

Originally Posted by gautami

how I could read the coordinates of the cloud points form a data file (as I need to track up to 150 points).

You can't. There is no CSV option for loading points for sampling: https://github.com/OpenFOAM/OpenFOAM...ple/sampleDict
The best you can do is use "#include" to include the file that has the data, but the data must be formatted in OpenFOAM's own interpretation of the data, e.g.:

Code:

    somePoints
    {
        type    cloud;
        axis    xyz;
        points  (
#include "$FOAM_CASE/the_data.txt"
);
    }

There the file "the_data.txt" would be located in the case main folder and the content would have to be something like this:

Code:

(0.049 0.049 0.00501)
(0.051 0.049 0.00501)

Warning: I have not tested if this works as intended.

Quote:

Originally Posted by gautami

2.Is it possible to get the acceleration data for these specific points by using "fields" (as U for velocity).

...not very easily. The acceleration field isn't used in most solvers. Nonetheless, instructions on how to perhaps do this are provided here: http://www.cfd-online.com/Forums/ope...tml#post196210 - post #3

gautami · August 19, 2015, 14:34

Dear Mr Bruno,

Thank you very much for your reply.

As per your suggestion I have used "#include option" in the "sampleDict" utility, to read the coordinate of the points from file "mordata" as:

Code:

 sets
(
    somePoints
    {
        type    cloud;
        axis    xyz;
        #include "mordata"
        points;
    }
);

(The mordata file is located in the system folder and the content, as an example for 6 points is: as described in
http://cfd.direct/openfoam/user-guid...c-file-format/)

Code:

points
(
(0 0 0)
(1 0 1.1)
(2 0 1.2)
(3 0 1.3)
(4 0 1.4)
(5 0 1.5)
);

I was able to run sample without any error and could see sub folders postProcesisng/sets/(time folders) were created with the required field data at the points.

However when I try to implement the same in "controlDict" utility to obtain the data runtime I end up getting the following error:

Code:

 /opt/OpenFOAM-2.2.0/bin/tools/RunFunctions: line 42:  8205 Segmentation fault      $APP_RUN "$@" > log.$APP_NAME 2>&1

This is how I implement the above in controlDict

Code:

functions
{
   points
     {
    type            sets;
        functionObjectLibs ("libsampling.so");
        outputControl   outputTime;
        interpolationScheme cellPoint;
        setFormat       raw;
        sets
        (
           somePoints
            {
              type cloud;
              axis xyz;
              #include "mordata" 
              points;
            }
        );
        fields
        (
            U
        );
    }
}

Kindly can you please help me with this issue.Thank you.

(I would like to mention here that, the option probes and wallPressure/surfaces in controlDict works fine, but the line option and points option in controlDict gaves me this error similar to the above error.

Code:

 : /opt/OpenFOAM-2.2.0/bin/tools/RunFunctions: line 42: 18418 Segmentation fault $APP_RUN "$@" > log.$APP_NAME 2>&1.

I have posted this issue in the thread: http://www.cfd-online.com/Forums/ope...s-runtime.html)

Your guidance will be invaluable.

Regards,
Gautami.

R.Mah · July 7, 2016, 06:31

Hello Mr Bruno,
I was looking how to extraxt points from my configuration for the postprocessing till I found these posts above, I kindly would like to know how can I extract points from differents lines from my geometry and save it with a format that OpenFOAM would read it, (I´m using type cloud for sampling)
The point is to sample the concentration in these differents cells on each time step

moh-farmani · July 17, 2016, 11:00

Hi Bruno
first thanks for your kindness and time. I want to take the velocity profile at every time steps over some surfaces located in computational doamin during running, and as my case is big so i can't save all fields every time steps and i couldn't use sampleDict.
could you please let me know the way?

November 15, 2014, 11:15	How to use endTime in ControlDict	#21
musahossein Senior Member musaddeque hossein Join Date: Mar 2009 Posts: 309 Rep Power: 18	Dear all: I am using OpenFoam 2.2.1 , InterDyMFoam/SloshingTank2D as follows: I am running a code that will modify the displacement .dat file in OpenFoam/SloshingTank2D as follows: Each time the file is overwritten with 2 lines of data with a begin time and end time and corresponding displacements as follows: 2 ( ( 0.19 (( 0.0265476475 0.00 0.00) ( 0.00 0.00 0.00))) ( 0.21 (( 0.0369661065 0.00 0.00) ( 0.00 0.00 0.00))) ) The first column is time and the next column are the displacements associated with the time. Since both the time column and the displacement column will change as the new data is created, I would like to get an output at each end time (0.21 in this case). Can anyone suggest how I can use startFrom and stopAt to do this? In the OpenFoam Manual, for controlDict under "startFrom", there are options such as firstTime, startTime and latestTime options. so for example if the file previous to the one above is as follows: 2 ( ( 0.17 (( -0.0665476475 0.00 0.00) ( 0.00 0.00 0.00))) ( 0.19 (( 0.0369661065 0.00 0.00) ( 0.00 0.00 0.00))) ) Should I use the latestTime option? What about the stopAt option? looks like I only have the writeNow option. Is that correct? Any suggestions or comments would be appreciated, Thanks.

November 17, 2014, 16:22		#22
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,981 Blog Entries: 45 Rep Power: 128	Greetings Musaddeque, If you have a certain code that generates the file for the movement, then you can also have that code generate a file that has the times for start and stop. For example, the new file "system/controlDict.start_stop" would have this: Code: newStartTime 0.17; newStopTime 0.19; And your file "system/controlDict" would (for example) be something like this: Code: FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // #include "controlDict.start_stop" application icoFoam; startFrom startTime; startTime $newStartTime; stopAt endTime; endTime $newEndTime; //.... I didn't add more lines, as I was only trying to exemplify the main detail. This is further explained in the release notes for one of OpenFOAM's versions... er, I have no idea in which version of OpenFOAM this was included. OK, it's explained in the User Guide: http://www.openfoam.org/docs/user/ba...8-1040004.2.10 - section 4.2.10 The #include and #inputMode directives Best regards, Bruno vsammartano likes this. __________________ OpenFOAM: FAQ \| Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM

November 27, 2014, 16:33	OpenFOAM write interval doesnt always work	#28
musahossein Senior Member musaddeque hossein Join Date: Mar 2009 Posts: 309 Rep Power: 18	As a follow up to the previous thread, in control dict I specify the write time as 0.02 as shown below: Code: FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * new file * * * * * * * * * * * * * * * * * * * * * * * * * * // application interDyMFoam; startFrom latestTime; startTime 21.70000; stopAt endTime; endTime 21.72000; deltaT 0.0005; writeControl adjustableRunTime; writeInterval 0.02; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression compressed; timeFormat general; timePrecision 6; runTimeModifiable yes; adjustTimeStep yes; maxCo 0.5; maxAlphaCo 0.5; maxDeltaT 1; But during OpenFoam run, I end up with the following time stamp on the oputput files: Code: . . . 21.68 21.7199999999 Looks like it not only missed writing output at 21.70, but it didnt quite get to 21.72. Any suggestions advice would be greatly apprciated. Thanks! Last edited by wyldckat; January 25, 2015 at 12:09. Reason: Added [CODE][/CODE]

January 25, 2015, 12:21		#29
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,981 Blog Entries: 45 Rep Power: 128	Hi Musaddeque, Sorry, I wasn't able to look into this any sooner. And I know there is a bug report related to this issue, but I haven't found it yet. OK, the latest error seems to be because the time snapshot 21.70 doesn't exist and because you have these settings: Code: startFrom latestTime; startTime 21.70000; endTime 21.72000; timePrecision 6; But since you have only these time folders: Code: 21.68 21.7199999999 Then it's not able to 21.70 because it doesn't exist and it's not able to find "21.7199999999" because it has a precision higher than 6... although I'm not certain about this one. Can you please provide a test case? Because I'm not able to reproduce this error. Best regards, Bruno edit: OK, found it: http://www.cfd-online.com/Forums/ope...ct-number.html Last edited by wyldckat; January 25, 2015 at 12:24. Reason: see "edit:"

January 25, 2015, 16:56	OpenFOAM write interval doesnt always work	#30
musahossein Senior Member musaddeque hossein Join Date: Mar 2009 Posts: 309 Rep Power: 18	WyldKat: Thanks for your response. I cant provide a test case as I have coupled at program with openfoam. The program looks for specific files with specific time stamps. As a result, if it does not find the file 27.72 for example, it will give an error. I got around this problem for the time being by: 1.Increasing the time stamp by a range. So for example, instead of supplying the start time as 2.00 seconds of simulation time, I will supply 1.999999. Similarly, I will increase the end time by a small amount say 0.0001. So the code now looks for something within that range. 2. Increasing the writPrecision in controlDict to 6. Both these appear to help and I have running simulations w/o problems on this issue. I will try OpenFOAM version 2.3 soon. Thanks

November 18, 2014, 22:01		#23
musahossein Senior Member musaddeque hossein Join Date: Mar 2009 Posts: 309 Rep Power: 18	Thankyou very much for your response. I am trying that approach.

June 4, 2015, 16:00		#31
rocap New Member romain Join Date: Jun 2015 Posts: 2 Rep Power: 0	Dear all. I have the same type of problem as musahossein. I’am working on foam-extend 3.1 on a turbine simulation. I am using pimpleDyMFoam to solve the simulation. What I need to do now, is to set probes on one face of the blades. But probes can’t be fixed. I need them to follow the blades to always get the pressure at the good point. I read all your previous post but I could not fix my problem. Do you have an idea about the way I can do this? It also need to be run in parallel. I don’t know if it’s possible with this “moving” probes. Best Regards Romain

June 12, 2015, 19:38		#32
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,981 Blog Entries: 45 Rep Power: 128	Greetings Romain and welcome to the forum! AFAIK, "moving probes" is only somewhat implemented in OpenFOAM 2.2.x and newer: http://www.openfoam.org/mantisbt/view.php?id=1090 It's in this commit: https://github.com/OpenFOAM/OpenFOAM...f27b5d573c2a9b I don't know if this feature has been back-ported to foam-extend already or not. Best regards, Bruno __________________ OpenFOAM: FAQ \| Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM

June 16, 2015, 20:44		#33
okcfdlab New Member Joshua Brinkerhoff Join Date: Nov 2014 Location: Kelowna, BC Canada Posts: 3 Rep Power: 12	Sample can be run in parallel on a decomposed case in exactly the same manner as the case itself is run in parallel. For instance, if you have a case decomposed into four processor directories, you can run sample in parallel on four processors by mpirun -np 4 sample -parallel This is much faster than running reconstructPar and then sample.

June 18, 2015, 12:36		#34
rocap New Member romain Join Date: Jun 2015 Posts: 2 Rep Power: 0	Dear Bruno Thanks for your reply and your help. I will try it and I will let you know regards

August 14, 2015, 07:27		#35
gautami Member Gautami Erukulla Join Date: Mar 2009 Posts: 71 Rep Power: 17	Dear All, I am working on the interDyMFoam/floatingObject tutorial. I need guidance with post processing. I am trying to get fluid velocities and acceleration values at specific points in the computational domain. 1.In the "sampleDict/controlDict" file can I use the option "type cloud" and read the points from a file. 2.Is it possible to get the acceleration data for these specific points by using "fields" (as U for velocity). Thank you.

August 17, 2015, 13:39		#36
gautami Member Gautami Erukulla Join Date: Mar 2009 Posts: 71 Rep Power: 17	Dear Mr Bruno, I am trying to use sampleDict utility with cloud of points option. Kindly can you please guide me as to how I could read the coordinates of the cloud points form a data file (as I need to track up to 150 points). Your help is highly appreciated.Thank you. Regards, Gautami.

August 19, 2015, 14:34		#38
gautami Member Gautami Erukulla Join Date: Mar 2009 Posts: 71 Rep Power: 17	Dear Mr Bruno, Thank you very much for your reply. As per your suggestion I have used "#include option" in the "sampleDict" utility, to read the coordinate of the points from file "mordata" as: Code: sets ( somePoints { type cloud; axis xyz; #include "mordata" points; } ); (The mordata file is located in the system folder and the content, as an example for 6 points is: as described in http://cfd.direct/openfoam/user-guid...c-file-format/) Code: points ( (0 0 0) (1 0 1.1) (2 0 1.2) (3 0 1.3) (4 0 1.4) (5 0 1.5) ); I was able to run sample without any error and could see sub folders postProcesisng/sets/(time folders) were created with the required field data at the points. However when I try to implement the same in "controlDict" utility to obtain the data runtime I end up getting the following error: Code: /opt/OpenFOAM-2.2.0/bin/tools/RunFunctions: line 42: 8205 Segmentation fault $APP_RUN "$@" > log.$APP_NAME 2>&1 This is how I implement the above in controlDict Code: functions { points { type sets; functionObjectLibs ("libsampling.so"); outputControl outputTime; interpolationScheme cellPoint; setFormat raw; sets ( somePoints { type cloud; axis xyz; #include "mordata" points; } ); fields ( U ); } } Kindly can you please help me with this issue.Thank you. (I would like to mention here that, the option probes and wallPressure/surfaces in controlDict works fine, but the line option and points option in controlDict gaves me this error similar to the above error. Code: : /opt/OpenFOAM-2.2.0/bin/tools/RunFunctions: line 42: 18418 Segmentation fault $APP_RUN "$@" > log.$APP_NAME 2>&1. I have posted this issue in the thread: http://www.cfd-online.com/Forums/ope...s-runtime.html) Your guidance will be invaluable. Regards, Gautami. Last edited by wyldckat; August 19, 2015 at 17:11. Reason: Added [CODE][/CODE] markers

July 7, 2016, 06:31		#39
R.Mah New Member Bah.Mah Join Date: Jun 2016 Posts: 18 Rep Power: 10	Hello Mr Bruno, I was looking how to extraxt points from my configuration for the postprocessing till I found these posts above, I kindly would like to know how can I extract points from differents lines from my geometry and save it with a format that OpenFOAM would read it, (I´m using type cloud for sampling) The point is to sample the concentration in these differents cells on each time step

July 17, 2016, 11:00		#40
moh-farmani New Member mohafarmani Join Date: Aug 2015 Location: shiraz Posts: 14 Rep Power: 11	Hi Bruno first thanks for your kindness and time. I want to take the velocity profile at every time steps over some surfaces located in computational doamin during running, and as my case is big so i can't save all fields every time steps and i couldn't use sampleDict. could you please let me know the way?