
[Sponsors] 
April 6, 2011, 11:27 
integrate several fields

#1 
Member
Samuel ARNAUD
Join Date: Feb 2011
Location: Grenoble, FRANCE
Posts: 39
Rep Power: 8 
Hi foamers,
I'm doing a RTD (Residence Time Distribution) of a 3D cylinder. I solved the velocity part by using simpleFoam in a steady state. Then, with this converged velocity I created a similar case (with scalarTransportFoam, transient), including a step experiment at the beginning. By measuring the Heat flux at the "outlet" patch, I would manage to study this RTD. (Hope you got everything) My case briefly presented, here's my question: in the controlDict file, I want to use a function to calculate the integral for the product (Ux*T) during the whole calculation (t= 0 > 3 with dt=2.5e3) I was trying to use "libsimpleFunctionObjects.so" with the type "patchIntegrate" as follows Code:
flux { functionObjectLibs ( "libsimpleFunctionObjects.so" ); type patchIntegrate; fields (T); patches ( "outlet" ); factor Ux; } There is no way to do what I exposed above. Note: U isn't in the integral as it's constant for the whole calculation (already established). Apparently you need a scalar and not Ux... Code:
> FOAM FATAL IO ERROR: wrong token type  expected Scalar found on line 63 the word 'Ux' 2) Does it exist another utility to multiply 2 scalarfields? Then I'll be able to use the result of this one in my integral. Thank you
__________________
Sam 

April 7, 2011, 03:15 
My bad

#2 
Member
Samuel ARNAUD
Join Date: Feb 2011
Location: Grenoble, FRANCE
Posts: 39
Rep Power: 8 
I don't know what I was thinking about...
The integral is spatial and not temporal. Therefore, Ux isn't constant (as there is a laminar profile in the tube)! I must multiply, then both Ux and T before integrating more or less as follows: Code:
flux { functionObjectLibs ( "libsimpleFunctionObjects.so" ); type patchIntegrate; fields (Ux*T); patches ( "outlet" ); }
__________________
Sam 

April 7, 2011, 07:27 

#3  
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,020
Rep Power: 43 
Quote:
As what you're trying to compute isn't THAT uncommon SFO has a functionObject patchFieldFlow to do it (for compressible flow there is also a rho there, but that's alright I guess) simpleFunctionObjects can't do arbitray calculations (Ux*T or so) on patches BUT swak4Foam can. The functionObjects there that can do that are patchExpression or swakExpression and they are based on SFO Bernhard 

April 7, 2011, 08:53 

#4  
Member
Samuel ARNAUD
Join Date: Feb 2011
Location: Grenoble, FRANCE
Posts: 39
Rep Power: 8 
Quote:
First of all: thanks for your answer ! I was doing some tries with swak4foam before I saw your reply. First of them, I tried to change (naively...) the "functionObjectsLibs" into that: Code:
flux { functionObjectLibs ( "libsimpleSwakFunctionObjects.so" ); type patchIntegrate; fields (Ux*T); patches ( "outlet" ); I was then looking at the wiki page (nice job for this contrib, btw) checking for examples. I couldn't find one that can help me. Do you have any hints considering that? Meanwhile, I'll continue to dig all of this. Best Regards,
__________________
Sam 

April 7, 2011, 10:27 

#5  
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,020
Rep Power: 43 
Quote:
I hope to find the time to update the swakWikipage when I find time (which should be hopefully before my retirement). Until then I welcome any contributions on it Bernhard 

April 7, 2011, 10:34 

#6 
Member
Samuel ARNAUD
Join Date: Feb 2011
Location: Grenoble, FRANCE
Posts: 39
Rep Power: 8 
Thank you so much. I was just about to leave a message saying I did use this example. I'm waiting for the calculation results.
I'll post what I did if effective (hopefully!)
__________________
Sam 

April 7, 2011, 10:39 

#7 
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,020
Rep Power: 43 

April 7, 2011, 11:13 

#8 
Member
Samuel ARNAUD
Join Date: Feb 2011
Location: Grenoble, FRANCE
Posts: 39
Rep Power: 8 
If you don't mind, I'd rather post it here (or send you by email) first because if it works, it's a highly not straight forward way to do it I fear... :p
Let's wait and see
__________________
Sam 

April 8, 2011, 08:43 

#9 
Member
Samuel ARNAUD
Join Date: Feb 2011
Location: Grenoble, FRANCE
Posts: 39
Rep Power: 8 
I finally manage to realize my RTD!
The problem I had about integrating Ux and T together is solved. Here's what I used (it's definitely not the best way to do so, but that's a start): First thing, in my case I admitted that Ux=magU (as the flow is almost perfectly unidirectional). In controlDict, I input: Code:
functions { dflux { type expressionField; outputControl timeStep; outputInterval 1; fieldName dflux; expression "(T*mag(U))"; patches ( "outlet" ); autowrite true; } flux { functionObjectLibs ( "libsimpleFunctionObjects.so" ); type patchIntegrate; fields (dflux); patches ( "outlet" ); } } libs ( "libOpenFOAM.so" "libgroovyBC.so" "libsimpleSwakFunctionObjects.so" "libswakFunctionObjects.so" "libswakTopoSources.so" ) ; 2) I'm not sure if the dflux "patches" is correct or if the calculation is made everywhere... As I said, it's highly inefficient compare to what's possible to do, but that's a start. I wait for your comments before putting my example in the swak4foam wiki (if it's not too crappy) Have a nice weekend
__________________
Sam 

April 9, 2011, 08:40 

#10  
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,020
Rep Power: 43 
Quote:
You don't have to go through the expressionField. libsimpleSwakFunctionObjects.so already has what you need: Code:
temperatureSum { type patchExpression; accumulations ( sum ); patches ( outlet ); expression "mag(U)*T*area()"; verbose true; } Code:
temperatureSum { type patchExpression; accumulations ( sum ); patches ( outlet ); expression "phi*T"; verbose true; } Bernhard 

April 11, 2011, 03:56 

#11  
Member
Samuel ARNAUD
Join Date: Feb 2011
Location: Grenoble, FRANCE
Posts: 39
Rep Power: 8 
thanks for your answer.
I didn't want to use the patchExpression with "sum" because I thought it was only for an addition. I didn't push it further... Quote:
[EDIT]: I tried to use your expression (to compare results) but I'm having some trouble with. It can't find the "linsimpleSwakFunctionObjects.so" apparently. Don't know what's wrong, I did "wclean" and "wmake" again, but it seems there's a problem with it. With OF1.7, I guess that's normal (as you put in your README) but with OF1.6dev, it should work...
__________________
Sam Last edited by sixwp; April 11, 2011 at 04:02. Reason: test done 

December 1, 2011, 10:27 

#12 
Member
Tibor Nyers
Join Date: Jul 2010
Location: Hungary
Posts: 91
Rep Power: 10 
Hi,
To get to grips with the simpleFunctionObjects and swak4Foam I created a modified PD case to pisoFoam and injected scalarTransport into it  scalar T. I want to track the very uninteresting change of T in the domain and on the boundary. In the blockMeshDict I named all my blocks "domain". I failed to create an expression for the difference of patchFieldFlow @ the inlet and outlet  main aim is to replicate the sumT expression with only boundary information only. Later I realized that I cannot reproduce the patchFieldFlow simpleFuncuntionObject with swak ... At first I tried to somehow name (save) the two patchFieldFlow and make a subtraction. Is it possible to name / save it or to combine this with swak4Foam? My pure swak was crap as well ... For the new sumT expression the timeStep information is necessary, how can one obtain the timeStep within swak? There's some very similar stuff in the Examples / groovyBC / pulsedPitzDaily but I couldn't put it into practise. Code:
functions { massFlowAverageT { type patchMassFlowAverage; functionObjectLibs ( "libsimpleFunctionObjects.so" ); fields ( T ); patches ( inlet outlet ); factor 1.0; verbose true; } patchFieldFlowT { type patchFieldFlow; functionObjectLibs ( "libsimpleFunctionObjects.so" ); fields ( T ); patches ( inlet outlet ); verbose true ; } patchFieldFlowT_S4F { type patchExpression; expression "mag(Sf())*phi*T" ; patches ( inlet outlet ); accumulations ( sum ); verbose true ; } patchFieldFlowNettoT_S4F { type swakExpression; valueType internalField; variables ( "inFlowT{inlet}=mag(Sf())*phi*T;" "outFlowT{outlet}=mag(Sf())*phi*T;" ); expression "outFlowTinFlowT"; accumulations ( sum ); verbose true; } // total T in simulation domain sumT { type swakExpression; valueType cellSet; setName domain; expression "( T * vol() ) / sum( vol() )"; accumulations ( sum ); verbose true ; } } 

December 2, 2011, 07:17 

#13  
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,020
Rep Power: 43 
Quote:
http://openfoamwiki.net/index.php/Ma...ver_is_writing That means multiplying the surface is not necessary (actually it is wrong). Also remote variables only work correctly if they are uniform. So for your difference you'll have to do the sums on the patches (inFlowT{inlet}=sum(phi*T)) and on the internalField accumulate the difference with min, max or average (they all should give the same result). Whether checking for the "conservation of temperature" makes physical sense of course depends on your solver 

December 5, 2011, 12:09 

#14 
Member
Tibor Nyers
Join Date: Jul 2010
Location: Hungary
Posts: 91
Rep Power: 10 
Thank for the assistance!
With your advices I managed to pull it through, big thank you! The only thing that still puzzles me is the slight difference in the the values  volume integration of the scalar and the calculated value based on the boundary flows. The latter gets accumulated in a variable, so there will be some error as the simulation progresses. But what causes the relatively big difference at the start, and the error wouldn't grow afterward, albeit it is not constant  quite strange! Attached the plots. I attach the case since I usually find them quite useful if there's an attached project on the threads. So, the attachment contains a very simple extended pisoFoam solver with a scalar transport equation in it. The case is the pitzDaily with a scalar injected on the inlet. I used groovyBC to partition just the middle section of the inlet. I use simpleFunctionObjects and swakExpressions to track the evolution of the T scalar in the domain. I tried to replicate some functionalities with swak just to get some things sorted and learn a bit. At the end of the simulation pyFoam generates the plots. 

December 5, 2011, 20:14 

#15  
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,020
Rep Power: 43 
Quote:
Anyway: I don't think that the initial error is something to worry about. The relative error at the first timestep is (judging from your diagram) approx 10% and rapidly becoming smaller. Possible explanations are: the solution is not "totally correct" (try changing the tolerances of the linear solver and see if that error changes), error in the interpolation to the patches, time discretization: the summation at the patches is a pure explicit Euler while the other stuff depends on whatever scheme you chose for ddt 

January 7, 2014, 07:27 

#16  
Member
Join Date: Jun 2011
Posts: 79
Rep Power: 8 
Quote:
I am wondering how swak4foam and the libsimpleSwakFunctionObjects.so library compute exactly the integrals, I mean accuracy and method. Thanks! Best! 

January 7, 2014, 19:36 

#17 
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,020
Rep Power: 43 
What do you mean? Usually integrals are implemented in the user expressions: size of the discretization elements (=cell volume or face area) times the (cell or face value). Sum.
__________________
Note: I don't use "Friend"feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request 

January 30, 2014, 07:46 

#18  
Member
Join Date: Jun 2011
Posts: 79
Rep Power: 8 
Quote:
Now I'm trying to integrate an expression on a patch via swak4foam. To do it I'd need the value of a field on another patch... I wonder if you could tell me how to do it with swakExpression. Also, I'd need the time derivative of the velocity as I set an uniform velocity ramp at the inlet but I got the next message when I use the "ddt" function: Code:
> FOAM FATAL ERROR: LHS and RHS of  have different dimensions dimensions : [0 1 2 0 0 0 0]  [0 0 1 0 0 0 0] Code:
dUdt { type expressionField; outputControl timeStep; fieldName ddtU; // expression "(UoldTime(U))/deltaT()"; expression "ddt(U)"; verbose true; autowrite true; Thanks for your attention!! Best! 

January 30, 2014, 13:04 

#19  
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,020
Rep Power: 43 
Quote:
 which OFversion  which swakversion  the fatalerror is without any context (so I could only guess what is going on). Try the following: "export FOAM_ABORT=1" and rerun. This should yield a stacktrace which would be helpful to see WHERE this is happening  what is "expected results" and what are the results you get?
__________________
Note: I don't use "Friend"feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request 

January 31, 2014, 06:49 

#20  
Member
Join Date: Jun 2011
Posts: 79
Rep Power: 8 
Quote:
Code:
{ type swakExpression; valueType patch; variables ( "ddtUin{INLET}=(UoldTime(U))/deltaT();" "ddtV{BODY}=(UoldTime(U))/deltaT();" ); patchName CYLINDER; accumulations ( sum ); expression "(ddtVddtUin)&normal()*area()"; verbose true; } Thank you so much, Bernhard!! Best! 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
The mysterious _0 fields  stevenvanharen  OpenFOAM Running, Solving & CFD  2  January 4, 2011 08:24 
Missing fields in reconstructPar  flowris  OpenFOAM  1  July 9, 2010 02:48 
domainIntegrate, dieselFoam and Lagrangian Fields  mturcios777  OpenFOAM  0  May 14, 2010 15:16 
PostChannel  maka  OpenFOAM PostProcessing  5  July 22, 2009 09:15 
Integrate Variables using PAraFoam  nandiganavishal  OpenFOAM PostProcessing  2  April 17, 2009 12:38 