# How to update a volScalarField's values

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 October 23, 2013, 04:09 How to update a volScalarField's values #1 Member   Thomas Vossel Join Date: Aug 2013 Location: Germany Posts: 45 Rep Power: 5 Hi! I have a question concerning how to update a volScalarField. Imagine the following problem: You have a volScalarField T for the temperature (with values applied to it). You now have another volScalarField X which is meant to consist of values depending on the respective temperatures. How do I implement an update for X which looks up the temperature of each element and then updates the value in terms of special conditions. With that I mean a procedure of this sort: Code: ```if (T<100) { X = 1; } if (T=100) { X = 2; } if (T>100) { X = 3; }```

 October 23, 2013, 04:26 #2 Senior Member   Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,437 Rep Power: 25 There are several ways to do it. One of them: Code: ```forAll(X, cellI) { if (T[cellI] < 100) X[cellI] = 1; else if (T[cellI] > 100) X[cellI] = 3; else X[cellI] = 2; }``` ThomasV likes this.

 October 23, 2013, 04:44 #3 Senior Member     Armin Join Date: Feb 2011 Location: Helsinki, Finland Posts: 156 Rep Power: 11 There are many examples in the source code, see e.g.: https://github.com/OpenFOAM/OpenFOAM.../hePsiThermo.C Here a simplified example: Say you get your temperature field like this: Code: ` const volScalarField& T = thermo.T();` Then you can update your field X like this: Code: ``` scalarField& TCells = T.internalField(); forAll(TCells, celli) { if (T[celli] < 100.0) X[celli] = 1; else if (T[celli] > 100.0) X[celli] = 3; else X[celli] = 2; }``` The boundary field you can update in a similar manner, I suggest you have a look at the code I linked above if you need to do this. ThomasV likes this.

 October 23, 2013, 05:13 #4 Member   Thomas Vossel Join Date: Aug 2013 Location: Germany Posts: 45 Rep Power: 5 Thanks! EDIT: Btw - is there a difference between writing "celli" and "cellI" (i.e. upper- / lowercase letter)?

October 23, 2013, 08:15
#5
Senior Member

Armin
Join Date: Feb 2011
Location: Helsinki, Finland
Posts: 156
Rep Power: 11
Quote:
 Originally Posted by ThomasV Btw - is there a difference between writing "celli" and "cellI" (i.e. upper- / lowercase letter)?
No, there is no difference.
The variable celli is a 'label' (i.e. a integer) defined in forAll, which is a macro that sets up the for loop. So, you can call the variable whatever you want, you just need to be consistent.

Last edited by dkxls; October 23, 2013 at 09:45.

 October 28, 2013, 11:06 #6 Member   Thomas Vossel Join Date: Aug 2013 Location: Germany Posts: 45 Rep Power: 5 Allright thanks... I'd like to add another more "practical" question here. Things now work fine and I define a temperature field which then is analyzed to determine the solid fraction in the respective cells. What I'd like to know is how to write the new volScalarField for the fraction solid into the "0 folder". I create the fraction solid field like this: Code: ``` volScalarField fracSol ( IOobject ( "fracSol", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::AUTO_WRITE ), mesh, scalar(0) );``` Afterwards it becomes filled with the actual data determined by the respective temperatures of the cells. This way I get my fracSol file written in every timestep. Every timestep except for the initial one that is... I now would like to know how I also can write the calculated fracSol into the 0 folder i.e. the fraction solid field for the initial temperatures. This also would come in handy when postprocessing the project in ParaFoam as there now is no fracSol field in time step 0 and it is a bit tedious to go to timestep 1 and activate the field plus once again any time you accidentally rewind to timestep 0 as it then gets unloaded (because there's no data for it in step 0)... I already tried to simply put a runtime.write() command before progressing time in the time loop but this didn't do the trick. I guess one usually would approach this problem with the setfields utility but as far as I know one here is limited to the premade functions like defining a block in which the variable get set to a certain value...

 October 28, 2013, 11:31 #7 Senior Member     Armin Join Date: Feb 2011 Location: Helsinki, Finland Posts: 156 Rep Power: 11 you can force the writing of a field at any time with Code: `fracSol.write();` You just should take care that you don't do it in the time-loop, as the field would then be written every time-step. ThomasV likes this.

 October 28, 2013, 12:07 #8 Member   Thomas Vossel Join Date: Aug 2013 Location: Germany Posts: 45 Rep Power: 5 Thanks - if I can come up with enough self-motivation after having finished my master thesis I might write a beginners tutorial so people won't have such a hard time figuring out such "mundane" things like this...

 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 brooksmoses OpenFOAM Post-Processing 2 December 8, 2008 11:00 JB FLUENT 2 November 1, 2008 13:04 Wilesco CD-adapco 0 January 5, 2006 06:34 Cb CD-adapco 1 January 22, 2005 10:21 acboge FLUENT 0 February 6, 2004 07:41

All times are GMT -4. The time now is 09:09.

 Contact Us - CFD Online - Top