integrate several fields
 

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:D)

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
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...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 :)

My bad
 

I don't know what I was thinking about...:o

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:(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

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: 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

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

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

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:
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:D)

Have a nice weekend :)

Hi.

You don't have to go through the expressionField. libsimpleSwakFunctionObjects.so already has what you need:
If you want the actual amount of T (which still is not the energy) flowing out this is better
But if you had wanted that you would have used the patchFieldFlow from the simpleFunctionObjects

Bernhard

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...:o

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...

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.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

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

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.

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:

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

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?

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...

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!

Of course. By using the fractionExpression to switch between gradientExpression and valueExpression you can emulate something like the freestream BC

Thank you bernhard, but would you mind to explain further about this BC?? I have looked for this everywhere without success!!

Best,

I only help with technical aspects of swak/groovyBC. The physics you've got to work out yourself.

Usually the best way is to sit down with a piece of paper "If the flow goes the BC is a Dirichlet condition with this expression else a Neuman with this gradient expression". Implementing this in groovyBC is then pretty straightforward (if you understand the meaning of the phi-field - but this has been explained numerous times here on the MessageBoard and on the Wiki)

Hello everyone
I'm facing similar problem, I want to calculate surface integral of velocity multiplied by temperature in order to compute bulk temperature at each longitudinal position of a heated pipe and therefore Nusselt number in flow direction.
Do you have any idea how to implement it by swak4foam?
Thanks in advance

Dear Bernhard,

I am troubling you again...

I want to create a new/derived field and write it at the output time.

lets visualize a new volScalarField of mag(U).

I found out there three ways to do it---

1. edit the application/code (I want to omit this option)

2. using Swak4foam with expressionField. I tried the following in controlDict,

Quote:
velocityMagSquared
{
type expressionField;
//outputControl outputTime;
//outputInterval 1;
fieldName UMag2;
expression "U&U";
autowrite true;
}
I also get the output file written in the corresponding output/time directory.

But problem is paraview do not import thes new field, it do not have this information.

(also how do swak4Foam decide weather to create a volScalarfield or volVectorfield )

the last way is using coded function/dynamic code,

I tried this, by adding the following lines in controlDict

Quote:
compute_ptot
{
functionObjectLibs ( "libutilityFunctionObjects.so" );
type coded;
enabled true;
redirectType ptot;
// outputControl outputTime;
// outputInterval 1;
code
#{

const volVectorField& U = mesh().lookupObject<volVectorField>("U");
volScalarField ptot
(
IOobject
(
"ptot",
mesh().time().timeName(),
U.mesh(),
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
mag(U)
);


#};
}
I neither get any new file in the corresponding output/time directory nor any visualization..:confused::confused::confused:

Please give me some suggesions with option 2 or 3.

I am trying this in OF 3.x and using following libraries,
Quote:
libs (
"libOpenFOAM.so"
"libsimpleSwakFunctionObjects.so"
"libswakFunctionObjects.so"
"libgroovyBC.so"
"mylibfvOptions.so"

);
Thanks,

It seems I'm currently on a crusade about this: PLEASE people. Use the Code-environment (the #-icon in the message-edit-toolbar) when adding code (and OpenFOAM-dictionaries count as code) to your messages. It makes reading so much easier
Which flavour of paraview: the built-in reader or paraFoam? Are any messages printed to the console about problems with the files or are they just silently ignored?
By looking at the valid result of a computation: in your case: inner product of two vectors is scalar. Therefor a volScalarField

Hi again Bernhard,

I'd like to integrate a velocity component across an interpolated plane in a 2D, O-grid. I usually dealt with swakExpressions and patch or volumes integrations. In this case, I have to fix the plane where integrating across. Can you tell me how to proceed with your tool?

Thanks in advance!
Best