# integrate several fields

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

 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=2.5e-3) 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; }``` but: 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'``` 1) Anyone has an idea how to do it? 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" ); }``` (Ux*T) doesn't work but that's the idea of what I wanna solve __________________ Sam

April 7, 2011, 07:27
#3
Assistant Moderator

Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,036
Rep Power: 43
Quote:
 Originally Posted by sixwp 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" ); }``` (Ux*T) doesn't work but that's the idea of what I wanna solve
@your recent posting: the factor always has to be a number that's why Ux didn't work. If you know the velocity you'd have to hardcode it here.

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:
 Originally Posted by gschaider @your recent posting: the factor always has to be a number that's why Ux didn't work. If you know the velocity you'd have to hardcode it here. 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
Hi Bernhard,

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" );```
but without success...

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: 4,036
Rep Power: 43
Quote:
 Originally Posted by sixwp Hi Bernhard, 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" );``` but without success... 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,
Have a look at the Examples that come with swak. Especially other/angledDuctImplicit is bloated with functionObjects.

I hope to find the time to update the swak-Wiki-page 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: 4,036
Rep Power: 43
Quote:
 Originally Posted by sixwp 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!)
Or (even better) you can add it as an example to the Wiki-page

 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" ) ;``` Remarque: 1) The huge amount of libraries at the end isn't required (only some would be necessary). I just have them from a previous case and didn't optimize it. 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: 4,036
Rep Power: 43
Quote:
 Originally Posted by sixwp 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" ) ;``` Remarque: 1) The huge amount of libraries at the end isn't required (only some would be necessary). I just have them from a previous case and didn't optimize it. 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
Hi.

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;
}```
If you want the actual amount of T (which still is not the energy) flowing out this is better
Code:
``` temperatureSum
{
type patchExpression;
accumulations (
sum
);
patches (
outlet
);
expression "phi*T";
verbose true;
}```
But if you had wanted that you would have used the patchFieldFlow from the simpleFunctionObjects

Bernhard

April 11, 2011, 03:56
#11
Member

Samuel ARNAUD
Join Date: Feb 2011
Location: Grenoble, FRANCE
Posts: 39
Rep Power: 8

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:
 If you want the actual amount of T (which still is not the energy) flowing out this is better Code: temperatureSum { type patchExpression; accumulations ( sum ); patches ( outlet ); expression "phi*T"; verbose true; } But if you had wanted that you would have used the patchFieldFlow from the simpleFunctionObjects
Exactly

[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 "outFlowT-inFlowT"; 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 ; } }``` Thank you!

December 2, 2011, 07:17
#13
Assistant Moderator

Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,036
Rep Power: 43
Quote:
 Originally Posted by Toorop 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 "outFlowT-inFlowT"; 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 ; } }``` Thank you!
Sorry for not answering to your post in more detail, but at a first glance I'd say that there is a slight misunderstanding on the definition of phi:
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.
Attached Files
 pisoScalarFoam.tar.gz (2.3 KB, 24 views) pitzDailyPisoScalar.tar.gz (4.4 KB, 26 views) volInt_vs_phi - all.pdf (13.6 KB, 70 views) volInt_vs_phi - start.pdf (9.4 KB, 48 views)

December 5, 2011, 20:14
#15
Assistant Moderator

Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,036
Rep Power: 43
Quote:
 Originally Posted by Toorop 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.
Sorry. I currently don't have the time to have a look at the case.

Anyway: I don't think that the initial error is something to worry about. The relative error at the first time-step 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:
 You don't have to go through the expressionField. libsimpleSwakFunctionObjects.so already has what you need:
Hi Bernhard!!

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: 4,036
Rep Power: 43
Quote:
 Originally Posted by maalan Hi Bernhard!! I am wondering how swak4foam and the libsimpleSwakFunctionObjects.so library compute exactly the integrals, I mean accuracy and method. Thanks! Best!
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:
 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.

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]```
I have used both the OF BC's and groovyBC to implement the velocity ramp. Also, I have calculated the time derivative like that:

Code:
```    dUdt
{
type expressionField;
outputControl timeStep;
fieldName ddtU;
//        expression "(U-oldTime(U))/deltaT()";
expression "ddt(U)";
verbose true;
autowrite true;```
But I don't get the expected results.

Best!

January 30, 2014, 13:04
#19
Assistant Moderator

Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,036
Rep Power: 43
Quote:
 Originally Posted by maalan Hi again and thanks for your reply! 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]``` I have used both the OF BC's and groovyBC to implement the velocity ramp. Also, I have calculated the time derivative like that: Code: ``` dUdt { type expressionField; outputControl timeStep; fieldName ddtU; // expression "(U-oldTime(U))/deltaT()"; expression "ddt(U)"; verbose true; autowrite true;``` But I don't get the expected results. Thanks for your attention!! Best!
A numer of questions:
- which OF-version
- which swak-version
- the fatal-error 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:
 - what is "expected results" and what are the results you get?
At last I got it!! This is an example of the correct expression... I just wanted to call the value of the field on another patch...

Code:
```    {
type swakExpression;
valueType patch;
variables (
"ddtUin{INLET}=(U-oldTime(U))/deltaT();"
"ddtV{BODY}=(U-oldTime(U))/deltaT();"
);
patchName CYLINDER;
accumulations (
sum
);
expression "(ddtV-ddtUin)&normal()*area()";
verbose true;
}```
Now I have another problem... I know that to set a velocity ramp at the inlet one can do it by using both the uniformFixedValue function in OF and groovyBC. Well, I would like to set a ramp with the freestream BC and it's not possible to do it with 'uniformFixedValue', so is there any way to do it with groovyBC??

Thank you so much, Bernhard!!
Best!

 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 stevenvanharen OpenFOAM Running, Solving & CFD 2 January 4, 2011 08:24 flowris OpenFOAM 1 July 9, 2010 02:48 mturcios777 OpenFOAM 0 May 14, 2010 15:16 maka OpenFOAM Post-Processing 5 July 22, 2009 09:15 nandiganavishal OpenFOAM Post-Processing 2 April 17, 2009 12:38

All times are GMT -4. The time now is 22:22.