# Probe for X or Y velocity

 Register Blogs Members List Search Today's Posts Mark Forums Read

 May 10, 2006, 04:30 Can someone please share with #1 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 703 Rep Power: 14 Can someone please share with me the code to monitor velocity (either U or V) as the solution progresses. I know this is done using the probe utility. However, I would prefer if someone can show me the code. I'm using the incompressible icoFoam solver. Thanks a lot!

 May 10, 2006, 06:02 That depends on whether you wa #2 Senior Member   Eugene de Villiers Join Date: Mar 2009 Posts: 725 Rep Power: 14 That depends on whether you want the data to be written to screen or to a file. If you want it written to file, check the implementation in oodles. If you want it written to the standard out, see below. Put this before your time loop: /******************************************/ IOdictionary pLocs ( IOobject ( "probeLocations", runTime.constant(), mesh, IOobject::MUST_READ, IOobject::NO_WRITE ) ); const pointField& probeLocations(pLocs.lookup("probeLocations")); labelList probeCells(probeLocations.size(), -1); forAll(probeLocations, pI) { probeCells[pI] = mesh.findCell(probeLocations[pI]); } /******************************************/ And then put the following at the end inside your time loop: /*******************************************/ forAll(probeCells, pI) { if(probeCells[pI] != -1) { label cellNo = probeCells[pI]; Pout << pI << ". Location: " << probeLocations[pI] << ", cell no.: " << cellNo << ", U: " << U[cellNo] << ", p: " << p[cellNo] //add any other fields here << endl; } } /*******************************************/ Put the probe locations in the constant/probeLocations dictionary as per usual. Note the code hasn't been tested so there might be bugs.

 May 10, 2006, 06:09 Thanks very much Eugene. I fee #3 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 703 Rep Power: 14 Thanks very much Eugene. I feel ashamed. I just went and included Probe.H and createProbes.H in my icoFoam.C followed by a reference to writeprobes.H after the runTime.write(); (i.e. # include "writeProbes.H"). Then I created a probeLocations inside the constant sub-directory. That was all. Follow that with a wclean && wmake to rebuild icoFoam and when I run my case, it neatly creates a probes subdirectory with velocity and pressure data at my selected point. I thank you guys a lot for being so patient with n00bs. Thanks and keep up the good work!

 August 2, 2007, 23:05 Eugene, Many thanks for your #4 Member   Quinn Tian Join Date: Mar 2009 Posts: 62 Rep Power: 10 Eugene, Many thanks for your code. I have successfully compiled my code. For some reason, I got this error while I tried to run the application. --> FOAM FATAL IO ERROR : problem while reading header for object probeLocations file: /home/qtian/OpenFOAM/qtian-1.4/run/tutorials/simpleFoam/bumpkom2/constant/probeL ocations at line 1. From function regIOobject::readStream(const word&) in file db/regIOobject/regIOobjectRead.C at line 75. FOAM exiting I know it must be something wrong with the probeLocations file format. Here is probeLocations file format. ( 0.01 0.10 0.000 0.01 0.15 0.000 0.01 0.2 0.000 ) Is there any other way to read the probe points location? Thanks for your help. Best QT

 August 3, 2007, 11:53 OpenFOAM 1.4 has probe functio #5 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 703 Rep Power: 14 OpenFOAM 1.4 has probe functionality inbuilt. Define your probe points in controlDict. james.conger likes this.

 August 6, 2007, 11:05 Dear Srinath, Could you tel #6 Member   Flavio Galeazzo Join Date: Mar 2009 Location: Karlsruhe, Germany Posts: 32 Rep Power: 10 Dear Srinath, Could you tell what are the keywords one have to write to the controlDict to activate the inbuilt probe functionality? Thanks

 August 6, 2007, 11:19 Please use the 'Search' option #7 Senior Member   Srinath Madhavan (a.k.a pUl|) Join Date: Mar 2009 Location: Edmonton, AB, Canada Posts: 703 Rep Power: 14 Please use the 'Search' option in future. Thanks! Quoting Eugene from an eariler post: Activate probes by adding the following to the end of your controlDict: functions ( probes1 { type probes; functionObjectLibs ("libsampling.so"); //dictionary probesDict; region region0; probeLocations ( (0.710 -0.730 0.829) (0.710 -0.757 0.763) (0.855 -0.714 0.881) (0.855 -0.748 0.805) (0.855 -0.774 0.735) (1.000 -0.695 0.932) (1.000 -0.754 0.805) (1.000 -0.779 0.735) (1.350 -0.651 1.030) (1.350 -0.740 0.862) ); fields ( p U ); } ) Reference: http://www.cfd-online.com/OpenFOAM_D...es/1/4350.html amir.mofakham likes this.

 August 7, 2007, 11:45 Dear Srinath, Thank you for #8 Member   Flavio Galeazzo Join Date: Mar 2009 Location: Karlsruhe, Germany Posts: 32 Rep Power: 10 Dear Srinath, Thank you for the prompt reply. Just a correction. The last parenthesis have to be followed by a ";", or the function doesn't work. flga amir.mofakham likes this.

 May 22, 2009, 00:51 surface patch instead of probelocations #9 Member   santhosh Join Date: Apr 2009 Location: India Posts: 70 Rep Power: 10 Hi, Can we use any surface patch instead of writing probeLocation explicitly. I need this to calculate surface averaged quantity(vertex averaged) at the outlet patch in case of RTD calculations. The following is not working. functions ( RTD { type probes; functionObjectLibs ("libsampling.so"); setFormat gnuplot; surfaceFormat raw; probeLocations ( patches (outflow) ); fields (T); } ); Thanks Santhosh..

 August 17, 2009, 05:40 patchAverage #10 Member   santhosh Join Date: Apr 2009 Location: India Posts: 70 Rep Power: 10 I started again looking at the answer for the above problem. Finally I could find that patchAverage utility can do the required operation. Now the problem is patchAverage cannot be used for runTime calucation, i.e., patchAverage cannot write the output at each time step similar to probes utility. I am trying to modify it so that it will output average of a patch at each time step. If anybody already done that please reply. Regards santhosh

August 17, 2009, 11:22
#11
Assistant Moderator

Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,020
Rep Power: 43
Quote:
 Originally Posted by santoo_cfd I started again looking at the answer for the above problem. Finally I could find that patchAverage utility can do the required operation. Now the problem is patchAverage cannot be used for runTime calucation, i.e., patchAverage cannot write the output at each time step similar to probes utility. I am trying to modify it so that it will output average of a patch at each time step. If anybody already done that please reply.
Yes. It has been done. Have a look at http://openfoamwiki.net/index.php/Co...unctionObjects and the (note the original name) patchAverage-functionObject

Bernhard

 August 18, 2009, 01:17 #12 Member   santhosh Join Date: Apr 2009 Location: India Posts: 70 Rep Power: 10 Thanks Bernhard, That is exactly what I want. Actually I was able to change the solver to do the required operation. But this utility is much more robust and generic. Thanks a lot --santoo..

 August 18, 2009, 01:52 #13 Member   santhosh Join Date: Apr 2009 Location: India Posts: 70 Rep Power: 10 Bernhard Little help, May be I am doing simple mistake. I successfully compiled simpleFunctionObject and could able to see it in USER_LIBBIN. But, when I included function object in system dictionary as following, functions ( RTD { type patchAverage ; functionObjectsLibs ("libsimpleFunctionObjects.so"); verbose true; patches ( outflow ); factor 1; } ); I got following error, Unknown function type patchAverage Table of functionObjects is empty From function functionObject::New(const word& name, const Time&, const dictionary&) in file db/functionObjects/functionObject/functionObject.C at line 74. FOAM exiting --santosh

 August 18, 2009, 02:12 #14 Member   santhosh Join Date: Apr 2009 Location: India Posts: 70 Rep Power: 10 It is working now, I added following in controlDict (change is addition of fields to it) functions ( RTD { type patchAverage; functionObjectLibs ("libsimpleFunctionObjects.so"); fields ( T ); patches ( outflow ); verbose true; factor 1; } ); -santhosh

August 18, 2009, 03:59
#15
Assistant Moderator

Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,020
Rep Power: 43
Quote:
 Originally Posted by santoo_cfd It is working now, I added following in controlDict (change is addition of fields to it)
Strange. Your previous example should have failed with an error about that missing (not with an empty table)

 August 18, 2009, 06:21 #16 Member   santhosh Join Date: Apr 2009 Location: India Posts: 70 Rep Power: 10 I too felt the same. I came to know about adding field after running in openFOAM 1.5 version. I feel the problem is with 1.6 version. It may be printing wrong error messages/Error messages are misplaced in code. -santhosh

 August 18, 2009, 08:46 Confused... #17 Senior Member   Sandy Lee Join Date: Mar 2009 Posts: 213 Rep Power: 11 There is always different response ... Last edited by sandy; August 18, 2009 at 19:33.

August 18, 2009, 08:47
#18
Assistant Moderator

Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,020
Rep Power: 43
Quote:
 Originally Posted by santoo_cfd I too felt the same. I came to know about adding field after running in openFOAM 1.5 version. I feel the problem is with 1.6 version. It may be printing wrong error messages/Error messages are misplaced in code.
Question: You used different sources for 1.5 and 1.6 (the 1.5 version of the simpleFunctionObjects will not compile on 1.6 so this leads me to the suspicion that they were not there at all)

Bernhard

 August 18, 2009, 09:50 #19 Member   santhosh Join Date: Apr 2009 Location: India Posts: 70 Rep Power: 10 I have two machines one with 1.5 version and another 1.6 version.. I have compiled respective simpleObjects on different machines as given at http://openfoamwiki.net/index.php/Co...unctionObjects. (there both simpleObject utility for 1.5 and 1.6 versions are available) The error I got in 1.6 machine is regarding "Table Empty" The error I got in 1.5 machine is regarding "missing field" hope I am clean now. --santoo..

August 19, 2009, 04:04
#20
Assistant Moderator

Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,020
Rep Power: 43
Quote:
 Originally Posted by santoo_cfd I have two machines one with 1.5 version and another 1.6 version.. I have compiled respective simpleObjects on different machines as given at http://openfoamwiki.net/index.php/Co...unctionObjects. (there both simpleObject utility for 1.5 and 1.6 versions are available) The error I got in 1.6 machine is regarding "Table Empty" The error I got in 1.5 machine is regarding "missing field" hope I am clean now. --santoo..
If it is not in the table, then the problem is that OpenFOAM can't find it. So do a wclean on the 1.6-version of the sources (I can't stress enough that the 1.5-version won't compile on 1.6) and make a "wmake libso" on them again. Lookout for an error. If there is
- no error
- it still doesn't work
- the library is found in \$FOAM_USER_LIBBIN
try using another functionObject (probe for instance) with that case (because I only take responsibility after the simpleFunctionObjects are loaded into the runtime-selection-table )

Bernhard

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post nzy102 OpenFOAM Running, Solving & CFD 1 April 14, 2008 01:16 hoerl OpenFOAM Running, Solving & CFD 2 January 15, 2007 07:04 ztdep OpenFOAM Running, Solving & CFD 6 November 30, 2006 04:22 hydrogen CFX 2 May 22, 2006 11:59 Yolanda CFX 0 May 17, 2006 06:27

All times are GMT -4. The time now is 05:17.