Hi, I want to calculate mass
 

Hi,
I want to calculate mass flow across a BC, which should be a general problem for most people who work with CFD. But I cannot find any standard utility in the 1.4.1 release that can help me. Is it just me ... ?
I have found a utility "calcmassflow" on the openfoam wiki. But that was apperantly created for version 1.2 and after som fiddling with correcting library paths to get wmake to work, I gave up.

Can anyone help?

Regards
Jens

Hi Jens OpenFOAM calculates t
 

Hi Jens
OpenFOAM calculates the massflow at every surface in every timeStep. To create a file which contains the flux-data (filename = phi) for every writeInterval you have to tell it OF.
Therefore look at the fvSchemes dictionary in <root>/<case>/system
For more Infomation on fvSchemes read the UserGuide
page: U-104 + U-109 (chapter 4.4.7)

Now you have the flux and need to postprzess it. Therefore you need to integrate phi at your boundary. There is a OF-utility named patchIntegrate.
The Problem is that phi is defined as "surfaceScalarField" and patchIntegrate only integrates "volScalarField". To integrate phi you have to modify the patchIntegrate Tool to read and integrate surfaceScalarFields.

Hf
Max

Hello Jens, A Good day to y
 

Hello Jens,

A Good day to you!

I have been using a modified version of the calcMassFlow utility that you found on the OpenFOAMWiki.

This version of the utility has the following features:
1. Ability to process a decomposed case (detected by the presence of multiple "processor<x>" folders)

2. A dictionary based selection of the patches across which to calculate the Massflow.

3. If a Density value in the dictionary greater than unity is found, it is used to directly calculate the flow in [kg/s], if the density line is commented out in the dictionary, the output is printed in [m^3/s] and [l/min].

4. Works on OpenFOAM 1.4, 1.4.1, 1.4.1-dev, etc..etc...

If you are only going to be working with single processor simulations, I can give you a slightly different version of the code, which is significantly faster (since the code overhead for multiprocessor supoort is not there).

http://www.cfd-online.com/OpenFOAM_D...s/mime_zip.gif calcMassFlow.zip

Have a nice day!

Philippose

Hello! As Jens I need to ca
 

Hello!

As Jens I need to calculate the massFlow through a BC. I've found phi files and the patchIntegrate tool, but I'm not able to modify it :S

Then, I am really interested in the calcMassFlow utility. But I am new in C++ and OpenFoam wmake.

So, it would be great if you could explain me how to use the calcMassFlow utility developed by Philippose. In which folder should I download it?? (applications/bin/linuxGcc4DPOpt ??) Or what tutorial should I read to compile it?? Any help will be appreciated.

Have a nice day !!

Gaby

Hello Gabriela, Good evenin
 

Hello Gabriela,

Good evening to you!

Sooo.... here are the steps you need to follow to compile and use calcMassFlow...

I am assuming that you have a working OpenFOAM installation, and that you are able to compile things using wmake....

1. Unzip the file "calcMassFlow.zip" to the folder: [home]/OpenFOAM/[username]-[OFVersion]/applications

2. Go into the created folder "calcMassFlow"

3. type "wmake"

4. The utility compiles, and installs the executable file in the folder:
[home]/OpenFOAM/[username]-[OFVersion]/applications/bin/linuxGCC4DOpt

The above four steps basically complete the compilation / installation of the utility.

To use it... you need to do the following:

1. In the folder "calcMassFlow" mentioned earlier, there is a sample "calcMassFlowDict" file.... copy this file into the "system" folder of your case.

2. Modify the entries under "patchNames" to the names of the patches through which you want to calculate the massflow.

3. Optionally, you can uncomment the "rho" line, and specify the density of the medium you simulated, in case you want the massflow in units "kg/s" instead of "m^3/s"

4. Go to the root folder of your case, and as usual, type:
calcMassFlow <root> <case> [-time t]

or

calcMassFlow <root> <case> [-latestTime]

or

calcMassFlow <root> <case>


That should be it....

Hope everything works as expected :-)!

Enjoy!

Philippose

Hello Philippose ! Good Eve
 

Hello Philippose !

Good Evening!!

I've followed all your steps and finally it worked very good !!!

Thank you so much! and I hope this would be useful to other Foamers !!! :-)

Gabriela

Hello Philippose,

Does this utility work with OF-1.5.x?
I have a compressible case so I cannot give a rho value. Do you have suggestion?

I would like to calculate mass flow rate at inlet in kg/s.

I guess I will try it anyways.

Thanks for your time,
Rachel

Mass flow in a plane into the field
 

Hi all,

Thanks for the posted utility in this thread.

I am interested to calculated mass flow rate in a plane in the field, not patches as inlet/outlet,

do you have any idea, what should i do?

Thanks,
Hamed

Hello Philippose,

Thank you for your great utility!

Do you know how I can run it in parallel? When I have a parallel case and run the utility detects all the processor directories and calculates the mass flow rate correctly. However, for big cases, this goes very slow as the program itself only uses 1 CPU.

When I run the program does not detect the processor directories anymore, causing it to do nothing.

How can I solve this?

steady BC, time dependent flux, density species
 

Hi All,

i have checked out calcMassFLow, nice tool!
But i have encountered some difficutlies...

First I dont understand this (perhaps someone could give me a hand)

so we have Volume/Time = Area* velocity
mass/Time = Volume/Time * density

so I asume if rho =1 we come out with Volume/Time.
If rho !=1 , we have to multiply with rho and end up with mass/time...ok byt why is the code then
and not if(rho.value() != 1.0) ?????

Second question:

I have two species coming out my inlet.
C3H8 and "air", how can I specify the different densities for each? There is only one entry for density in the dict.

Third question ( migth be slightly off-topic, i apologize for that) :
If I dont specify the density, using an compressible solver, phi needs to be calculated with density.
we have p=rho R T;
My BC are:

so NOT time dependent BC.

I am using reactingFOAM and my velocity Field shows eddys from resulting from unsteady BC... :confused:
This goes along with the time depending flow I have:

The flux is oszillating....WHY ???????
I have no clue why this is happening and it messes up everything...

PLZ help!

regards!

Hello

I would like to compare the massflow produced by this utility to the one I get un fluent.

In fluent, when you have a 2D case, it extrudes a third dimension of 1 meter to calculate the massflow.

I would like to know how it works here with this code? What's the value of the third dimension? Where is it created? How to change it?

Thanks for the help

[QUOTE=philippose;185787]Hello Gabriela,

Good evening to you!

Sooo.... here are the steps you need to follow to compile and use calcMassFlow...

I am assuming that you have a working OpenFOAM installation, and that you are able to compile things using wmake....

1. Unzip the file "calcMassFlow.zip" to the folder: [home]/OpenFOAM/[username]-[OFVersion]/applications

2. Go into the created folder "calcMassFlow"

3. type "wmake"

4. The utility compiles, and installs the executable file in the folder:
[home]/OpenFOAM/[username]-[OFVersion]/applications/bin/linuxGCC4DOpt

The above four steps basically complete the compilation / installation of the utility.

To use it... you need to do the following:

1. In the folder "calcMassFlow" mentioned earlier, there is a sample "calcMassFlowDict" file.... copy this file into the "system" folder of your case.

2. Modify the entries under "patchNames" to the names of the patches through which you want to calculate the massflow.

3. Optionally, you can uncomment the "rho" line, and specify the density of the medium you simulated, in case you want the massflow in units "kg/s" instead of "m^3/s"

4. Go to the root folder of your case, and as usual, type:
calcMassFlow <root> <case> [-time t]

or

calcMassFlow <root> <case> [-latestTime]

or

calcMassFlow <root> <case>


Hi philippose

I tried to compile(wmake) the file that you had attached but it throws me the following error, can you help me with this


SOURCE=calcMassFlow.C ; g++ -m32 -Dlinux -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -O3 -DNoRepository -ftemplate-depth-40 -I/home/research/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude -I/home/research/OpenFOAM/OpenFOAM-1.6/src/meshTools/lnInclude -IlnInclude -I. -I/home/research/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude -I/home/research/OpenFOAM/OpenFOAM-1.6/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linuxGccDPOpt/calcMassFlow.o
In file included from calcMassFlow.C:198:
/home/research/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude/createPhi.H: In function ‘int main(int, char**)’:
/home/research/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude/createPhi.H:50: error: ‘U’ was not declared in this scope
make: *** [Make/linuxGccDPOpt/calcMassFlow.o] Error 1


Thanks in advance.

Hi,

I have OF 1.7.0 and Paraview 3.8.0. How can i calculate flow rate of patches?

[QUOTE=subash;263350]I had the same issue and simply inserted

This makes the code to read the velocity field from the solution.
Now I have no compiler errors any more.

mass flow calculation in OF 1.6
 

Hi Foamers,

I need your help in calculating the mass flow rate in OF 1.6 at the boundary patches.
Plz help.

with rgds,
-Gopal.

Hey Gopal,
have you tried the utility 'calcMassFlow' yet?

I have tried the CalcMassFlow utility. It requires compilation of the utility. I am finding it difficult to compile as it is written for the older versions (1.2 or 1.3) I guess. I am using v1.6 for my calculations.

It will help me a lot if somebody can guide me thru.

thanks.

-Gopal.

Try these instructions

And if you occur any problems, then post the output error.
Be more specific about your problems, otherwise we cannot help you.

Hi Anne,

Thanks for the reply.
I have followed the steps. But still there are lot of errors. Plz see the attached log file.

with rgds,
-Gopal.

Okay. Basically the first error is the most important.
The compiler does not find the file fvCFD.H
Which version are you using exactly?

Please check if there is the file fvCFD.H in OpenFOAM-1.6/src/finiteVolume/lnInclude.

Hi thr,

I am using version 1.6.
I have included the path in the program calcMassFlow.C.
But still I am getting this error. Plz help.

================================================== ====================
[shindg2@cd80si0017 calcMassFlow]$ wmake
SOURCE=calcMassFlow.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-40 -I/home/edm/shindg2/.PKG/OpenFOAM/OpenFOAM-1.6/src/cfdTools/lnInclude -I/home/edm/shindg2/.PKG/OpenFOAM/OpenFOAM-1.6/src/cfdTools/general/lnInclude -I/home/edm/shindg2/.PKG/OpenFOAM/OpenFOAM-1.6/src/meshTools/lnInclude -I/home/edm/shindg2/OpenFOAM/shindg2-1.6/Libraries/cellFaceSetUtilities/lnInclude -IlnInclude -I. -I/home/edm/shindg2/.PKG/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude -I/home/edm/shindg2/.PKG/OpenFOAM/OpenFOAM-1.6/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/calcMassFlow.o
calcMassFlow.C:36:30: error: FaceSetUtilities.H: No such file or directory
calcMassFlow.C:37: error: ‘FaceSetUtilities’ is not a namespace-name
calcMassFlow.C:37: error: expected namespace-name before ‘;’ token
calcMassFlow.C: In function ‘int main(int, char**)’:
calcMassFlow.C:105: error: ‘flipSet’ was not declared in this scope
calcMassFlow.C:105: error: template argument 1 is invalid
calcMassFlow.C:105: error: invalid type in declaration before ‘=’ token
calcMassFlow.C:105: error: ‘checkFaceSetSides’ was not declared in this scope
calcMassFlow.C:111: error: ‘flips’ cannot be used as a function
make: *** [Make/linux64GccDPOpt/calcMassFlow.o] Error 1
[shindg2@cd80si0017 calcMassFlow]$
================================================== =====================

with rgds,
-Gopal.

Hi thr,

I am using version 1.6.
I have included the path in the program calcMassFlow.C.
But still I am getting this error. Plz help.

================================================== ====================
[shindg2@cd80si0017 calcMassFlow]$ wmake
SOURCE=calcMassFlow.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wno-strict-aliasing -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-40 -I/home/edm/shindg2/.PKG/OpenFOAM/OpenFOAM-1.6/src/cfdTools/lnInclude -I/home/edm/shindg2/.PKG/OpenFOAM/OpenFOAM-1.6/src/cfdTools/general/lnInclude -I/home/edm/shindg2/.PKG/OpenFOAM/OpenFOAM-1.6/src/meshTools/lnInclude -I/home/edm/shindg2/OpenFOAM/shindg2-1.6/Libraries/cellFaceSetUtilities/lnInclude -IlnInclude -I. -I/home/edm/shindg2/.PKG/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude -I/home/edm/shindg2/.PKG/OpenFOAM/OpenFOAM-1.6/src/OSspecific/POSIX/lnInclude -fPIC -c $SOURCE -o Make/linux64GccDPOpt/calcMassFlow.o
calcMassFlow.C:36:30: error: FaceSetUtilities.H: No such file or directory
calcMassFlow.C:37: error: ‘FaceSetUtilities’ is not a namespace-name
calcMassFlow.C:37: error: expected namespace-name before ‘;’ token
calcMassFlow.C: In function ‘int main(int, char**)’:
calcMassFlow.C:105: error: ‘flipSet’ was not declared in this scope
calcMassFlow.C:105: error: template argument 1 is invalid
calcMassFlow.C:105: error: invalid type in declaration before ‘=’ token
calcMassFlow.C:105: error: ‘checkFaceSetSides’ was not declared in this scope
calcMassFlow.C:111: error: ‘flips’ cannot be used as a function
make: *** [Make/linux64GccDPOpt/calcMassFlow.o] Error 1
[shindg2@cd80si0017 calcMassFlow]$
================================================== =====================

with rgds,
-Gopal.

Hey Gopal,

you are missing a library which is needed for the utility.
Look at this post, they have the same problems:

http://www.cfd-online.com/Forums/ope...massflowc.html

Here you can download the libraries:
http://openfoamwiki.net/index.php/Contrib_calcMassFlow

Follow the instructions which are neccessary for inserting the libraries. Then try it again :)

Anne

Hi Anne,

I have downloaded the required files /libraries. Thanks for the info.
I will give it a try and come back on this forum for some more help.

with rgds,
-Gopal.

Thanx philippose...
 

Thanx philippose....It works..really nice work....

Hi all,

I´ve made what Philippose told and I´ve been able to compile it, but when I execute de command calcMassFlowDic I´ve got a message error related with the variable phi:

Error... Patch: Name_of_my_Boundary not found
No phi for Time=4000 -> Skipping

Can anyone help me, please?

I understand, but... how??

Well. Is there a patch named Name_of_my_Boundary in your geometry? If yes: check the case (that is a favourite). The missing phi is more of a showstopper. Without it no mass flow will be calculated ... for that timestep (assuming this calcMassFlow is the utility I wrote and published http://openfoamwiki.net/index.php/Contrib_calcMassFlow year ago and haven't maintained for a long time. But maybe there is another utility of the same name floating around)

By copying and adapting the sources of the utility.

Personally I'd do that with swak4Foam. Either by using a patchExpression-function-Object during the simulation or the funkyDoCalc-utility afterwards (swak4Foam is one of the reasons why I don't maintain calcMassFlow anymore)

I´ll try

Thanks!

Dear Foamers,
I am trying to calculate the mass flow and/or the pressure force at any field or any section of the domain, which is not pre-defined patch like the inlet/outlet patch. This question has been asked back in 2009 by haghajani in this thread though it seems no one has tried to answer it or may be I couldn’t come across any other posts related to this issue

Would be great help if some one has done or modified the patchNames in order to calculate the mass flow at any section of the domain and lend me a hand on it.

Have a nice day!

Hi Mulualem,

I´m not so sure if I´m the adecuate person to help you. Anyway, I´ll try ^^

In ParaView, click Filters-->Slice and enter the coordenates of the plane you want to calculate the mass flow into the tab Properties.

Then, Filters--->Calculator and in Scalars choose U_X or U_Y depending on the direction of the mass flow you want to calculate.

Continue with: Filters--->Integrate Variables... You´ll see a chart in wich the U_X is, in fact, the mass flow in the x-direction. This is because when you apply the filter Integrate Variables, ParaView is multiplying each area of cell of the slice you´ve chosen for the variable U_X in this cell.

That´s all, hope it´s useful for you

Hi Paula,
Thank you very much for your quick reply. I will definately try your method and hope it works. I am still at my desk so will come back to you if I have encountered any problem.

This means I can even calculate the pressure forces at the same faces using using the p_rgh, am I right?

Thanks a lot!

Hi Paula,
I have been trying the steps you gave me to calculate the mass flow rate and it works fine. At least I can now work out to calculate the integral of the pressure at a chosen cross-section to obtain the pressure forces at that section.

Just I have one question though, If I want to calculate the flow rate at a small section of the face area (say a sum of cells in the domain face area), is paraView capable of choosing such kind of certain cells from the total face area of the domain?

Thanks!

Mulualem

Hi Mulualem,

Happy to know It worked :)

I don´t know the exact answer to your new question but I think there´s a filter called Select Extract Cells or something like that. Try it as the same way you used the other filter... and let me know if it works too ;)

Regards,

Paula

Hi Paula,
It works great.
Steps: After slice...go to filters>ExtractCellsByRegion
In the properties tab under the intersect with list, you can choose plane if you want to cut only one side of the face and set the coordinate but if you want to cut more than one side, you can choose box and work out with the translate, rotate and scale data in order to extract the exact surface area you want.

It has been great to talk to you and you saved a lot of my time. I have been looking the codes developed for this kind of post processing jobs but now I will put them aside for the time being and post-process my data using the paraView.

Thank you and have a nice weekend!

Best Wishes,

Mulualem

Great! It´s nice having been useful

Thanks for your reply !

Good luck! :D

Hi.
Have you finally found why was your flux oscillating?
Because i have the same problem (with steady boundary conditions).
Thanks
George

Mass flux output in a file
 

Hi,

Is there any body who knows how to write the fluxes given by calcMassFlow in a text file and not on the terminal where it normally does?

I want to plot the values on a graph but I don't know how to write them in a file!

NB. calcMassFlow is a ultility that gives the mass flux through patches.

Thank a lot

You're talking about http://openfoamwiki.net/index.php/Contrib_calcMassFlow ? Either use a script to extract that information from the output (I use for some strange reasons PyFoam) or use swak4Foam http://openfoamwiki.net/index.php/Co...e_calcMassFlow (that does output into a file too)