how to calculate mass flow rate on patches and summation of that during the run?
 

I know I have to use such code.but I don't know where should i put this in the OF files.in solver code(where of it?)or controlDict?

I think there shouldn't be a problem if you add the code just before

Best regards,
Fumiya

thanks Fumiya
and in this thread http://www.cfd-online.com/Forums/ope...ry-values.html
two files are introduced for calculating flow rate during the run.
where have to add the include files and the headers themselves in the solver code?

Although hard-coding this into the solver might give you the data you need, I suppose that it is way much easier to use some of OpenFOAM's run-time postprocessing tools, witch will give you what you need without the need to compile a single line of code.

To calculate the mass flow rates out of a patch/domain you should try something similar to this: https://www.hpc.ntnu.no/display/hpc/...Postprocessing

In addition you might want to look at swak4Foam, witch you can use to create complex expressions (used in the note linked to above).

If you need to integrate the mass flow over time (to find the total volume of discharged mass) you can do that as a post-processing step (for example in Octave/Matlab or similar tools). Integrating by the trapezoid rule should be straight-forward and probably accurate enough.

in this link there is the same as above.but where should i add the header files?
http://www.openfoamwiki.net/index.ph...ting_mass_flow

I really think you should pay more attention to my answers. I certainly expect people to read and find out stuff on their own. That means that I still think you should have a look at this tutorial: https://www.hpc.ntnu.no/display/hpc/...Postprocessing

The reason for me to stress this is that I suspect that your suggested solution, that is creating and compiling a custom-made solver, is way too complicated. The thread you found is from 2005, and the wiki article you link to is not updated since 2006. That is really a long time ago in the OpenFOAM world, and a lot of new features are added since then. Another aspect is that OpenFOAM 1.3 was the newest version in 2006, and you have no guarantees that the code will compile against the 2.x.x-versions of OpenFOAM (without looking at the code at all I would guess that so many things have happened since version 1.3 that it will not compile).

My suggested solution is simple, and a more or less verbatim copy of my recommended tutorial:

1. Install swak4Foam. This is an extremely useful toolbox, and you will probably find the time well invested. You should find the installation instructions on your own (Google, forum search).
2. Add the following to the bottom of your system/controlDict file:
   Code:

   ---

   libs (
        "libOpenFOAM.so"
        "libsimpleSwakFunctionObjects.so"
        "libswakFunctionObjects.so"
    );

functions
{
    volFlow
    {
        type                swakExpression;
        valueType          patch;
        patchName          outletPatchName;
       
        verbose            true;
        expression          "U&Sf()";
        accumulations      ( sum );
    }
}

   ---

The great with this is that you are able to use it with any solver, across different versions and cases without the need to recompile and rewrite a lot of source code each time. If you need more advanced expressions that is certainly possible too, there are a lot of examples out on the internet (search!).

Good luck.

thank you very much.the thread seemed somewhat confusing but now your summary is so useful.but
1)I have one inlet and one outlet.how to introduce both patches?
2)since the boundaries are changing during the run I want to calculate mass flow rates between two times.is it possible to calculating of phi like other parameters as: patchAverage -time '.001:.002' variable patchName ?
3)how to calculate total mass balance at the end of run.does the code
do such thing?
thanks.

and also i have a compressible fluid.isn't it better to use phi instead of U?
Please Give me a link for other expressions if there is.i haven't found anything.

If you need the flow at the inlet and outlet separately, you can add two copies of the volFlow function, like this:
If you need to calculate the net difference in flow, then you can do this by summing the two flows. I guess it is easiest to do this in Excel, Octave, Matlab or similar. If you really need it i also guess it is also possible to do this at run-time, but I can't give you an example right now. Check the examples that is distributed with swak4Foam, they are really good. You should pay special attention to the angledDuctImplicit example, as it is packed with swak4Foam examples.

I guess it is easiest to do this based on the results from the individual mass flows as well. Load the data into Matlab, calculate the difference at each time and integrate. A trapezoidal integration is probably fine.

Have you considered doing a volume integration to get the total mass in the domain at each time? The accumulated/lost mass between the two times will then be just the difference in total mass. Isn't that the easiest way to do it?


This piece of code sum over the patch, i.e. integrates. I guess, again, that the mass balance over time is easiest to find by postprocessing your numbers. Or perhaps doing a volume integration?

And yes, you can use phi instead of U&Sf(). I have never done any compressible analyses, so all my examples assume constant density (hence volume and mass flow is the same thing). You should watch out for this on your own.

thanks a lot.since i hadn't added the functions you mentioned since first how can I obtain mass flow rate now(in the middle of run.I've stopped the run and now need to know the mass flow rates)

What do you mean? I don't think i understand. It should be perfectly possible to stop a run (assuming you have some saved fields), add the swak4Foam probes in controlDict and start the run again (remember to set startFrom latestTime in controlDict).

the run is reached to a stage that i should check for equality of inflow and outflow to be exactly the same(althogh problem is unsteady compressible since inflow and outflow are in fact connected to combustion chamber that i don't need to simulate but mass since flow rate into and out from combustion chamber should be the same I have to set outflow patch to be closed when the total mass out of it be equal to inflow.it means mass flow rates should be the same.now that the first stage is ended how can i calculate the mass flow rates and modify the settings?

and also please see is this correct?

i corrected it as below functions:
but is there a way(a keyword like patchAverage that doesn't work for phi thats surfaceScalarField) to calculate all of mass entered and exited in and out of a patch after the run(post-processing)?

dear Hakon.i did what you said.now there is swak folders that have sum of phi on cells from the time i added the function.now how can i obtain phi on before time folders?
Thanks.

Please, I am not on-line all the time. Be patient. Do not post four follow-up posts. Think before you write. And please also remember that the people here on this forum help you as volunteers, they are not paid consultants. You should re-think the way you ask questions and treat other people. If I answer or helps you, that gives me no further obligations to answer any further questions.

I really think you should learn how to use internet search functionality, both Google and at this forum. Neither me nor other members on this forum am in a position to give you the complete and full answer all the time. In such cases I usually post from my memory, and assume that you are able to do the rest of the work yourself, like correcting bugs and do simple lookups in documentation, user manuals, examples and tutorials.

You, on the other hand, simply demand that the people that helps you give you the complete solution all the time. That is not how things work (at least not for me). I really think you should consider a visit to this forum: http://www.cfd-online.com/Forums/cfd-freelancers/

Btw: I think the answer to your question is the tool execFlowFunctionObjects

im sorry my friend.we are here to help eachother.i only propound my question to reach an answer for myself and for others need it now or in future.its nice to remember we god belivers in all religions believe that all knowledge page we write or learn someone remains and help us in other world.the knowledge value is higher than this assumpsions and comparison to money.
Thank you very much again for posts

the command execFlowFunctionObjects gives this error:
is there another command for that specific for SWAK4FOAM functions?

its odd if nothing has made yet for mass flux post processing after run.then should i delete all folders and begin from zero again to write mass flux in folders?

if anyone knows a post processing keyword or function please guide me.
Thanks all.