CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Residence time distribution (RTD) for dummies (http://www.cfd-online.com/Forums/openfoam-solving/114149-residence-time-distribution-rtd-dummies.html)

vanekp March 6, 2013 04:07

Residence time distribution (RTD) for dummies
 
Hello foamers,

I'm a total newbie in OpenFOAM and I'm supposed to do a RTD analysis for static mixers with quite a complex geometry. I searched the internet for a week now and I couldn't find the desired information so I'm turning to you, more advanced users.

So far I followed a procedure:
1. Steady-state solution of laminar flow with simpleFoam (which I would like to edit in future to calculate also a temperature transfer).
2. I took the U file from the last time folder and copied it into new case folder into 0.
3. I used scalarTransportFoam on calculated velocity field to inject a tracer T at the inlet boundary.

And now I got stuck with how to evaluate a concentration of the tracer at the outlet boundary so I could create RTD plot.

Could any of you give me a "cook book for dummies" how to proceed with the rest and if there would be any simpler way to deal with it then copying the U file by hand?

Thank you very much for any suggestions.

gschaider March 10, 2013 12:38

Quote:

Originally Posted by vanekp (Post 411877)
Hello foamers,

I'm a total newbie in OpenFOAM and I'm supposed to do a RTD analysis for static mixers with quite a complex geometry. I searched the internet for a week now and I couldn't find the desired information so I'm turning to you, more advanced users.

So far I followed a procedure:
1. Steady-state solution of laminar flow with simpleFoam (which I would like to edit in future to calculate also a temperature transfer).
2. I took the U file from the last time folder and copied it into new case folder into 0.
3. I used scalarTransportFoam on calculated velocity field to inject a tracer T at the inlet boundary.

And now I got stuck with how to evaluate a concentration of the tracer at the outlet boundary so I could create RTD plot.

Could any of you give me a "cook book for dummies" how to proceed with the rest and if there would be any simpler way to deal with it then copying the U file by hand?

Thank you very much for any suggestions.

Calculating the average of a field on a patch could be done with the patchAverage-Utility that comes with OpenFOAM (for the written data). Calculating the average during the run can be done with a function object. The two function objects that I know are both part of swak4Foam: patchAverage and patchExpression (more general)

Copying over U: not that I know. There are functionObjects that solve the tracer during the solution of the regular fluid equations, but these won't help you

tomf March 11, 2013 06:15

Hello Vanekp,

Maybe a different approach: if you include a unit source in your scalar transport equation, you get your residence time distribution for the entire volume. In that case, set the value at the inlet at 0, and you will see "fresh" fluid entering.

Regards,
Tom

chegdan March 11, 2013 22:22

Hi Vanekp,

I have done passive scalar transport in a manner similar to what you are doing. To answer your question about the concentration at the boundary:
  1. You will need to measure Mixing-Cup average at the outlet: Instead of just an average concentration at the outlet, you will need to determine a velocity weighted average similar to patchMassFlowAverged function object from simpleFunctionObjects. For an incompressible flow, the mass flow averaged is equal to the velocity-weighted average is equal to the mixing-cup average. This average will most accurately represent an experimental average that you can measure in the lab.
  2. The method of taking the steady-state velocity profile and decoupling the velocity and concentration field only works with the assumption that the tracer and fluid are of exactly the same physichcemical properties...i.e. its a passive scalar :D.
  3. If you use the function object I suggested, you will be given a text file with two columns that you can plot and visualize over time.

If you decide to move on to turbulent flow modeling, you need a few more things to correctly calculate the RTD. In scalarTransportFoam, you will need to add the affects of turbulence on your passive scalar through a transport equation similar to
Code:

                fvm::ddt(C)
              + fvm::div(phi, C)
              + fvm::SuSp(-fvc::div(phi), C)
              - fvm::laplacian(D, C)
              - fvm::laplacian(Dturbulent, C)

This was posted on http://www.cfd-online.com/Forums/ope...tml#post280210 and has worked for me in getting accurate RTD's derived from flows calculated from simpleFoam. Dturbulent is the turbulent viscosity divided by the turbulent Schmidt number (i.e. the gradient diffusion hypothesis). Its a simple solver to program yourself. Good luck!

vanekp March 13, 2013 04:11

Thank you all for the advice.

I was told the same thing about the patchMassFlowAverage by my colleague. So far I'm interested only in laminar flows, so the adjustment is not yet necessary but in the future I'll have to do it.

So I've set up everything according to the advice, I wrote a very simple shell script, which runs the sequence mySimpleFoam (simpleFoam with added solution of temperature) -> copying the velocity fields U and phi -> running scalarTransportFoam with patchMassFlowAverage function object included. So I'm now able to get the RTD curve quite nicely.

But now I'm dealing with problems with the solution. The velocity fields seem to be calculated well and when I run the scalarTransportFoam at the beginning everything seems to go right and at one point the solution goes totally 'bananas' and the Flow Average gets even negative (and even into range of -1e15) which I don't even understant how is it possible to go negative.

Do any of you have experince with this kind of behaviour and how to resolve it?

tomf March 13, 2013 05:16

Hello Vanekp,

Did you also copy the phi file from the latest timestep your simpleFoam run? It is calculated during the simple loop and corrected for conservation of mass instead of interpolated from the velocity field at the startup of scalarTransportFoam. This means you have a divergence free field to start with.

You can test this quite easily by running the solver twice, once with and once without the copied phi field.

Regards,
Tom

vanekp March 13, 2013 09:44

Thank you for the advice.

But yes I have copied both U and phi files. But I found out, that the problem is with the solution as the solution starts to oscilate, so I'm trying to figure out where is the problem, why the solution oscilates

Jonas Ansoni March 27, 2013 14:04

Hello Foamers!!

I'm calculating the RTD as described by Daniel, using patchMassFlowAverged. However, I need these values ​​to calculate the variance. I made a python script to perform these calculations, but I'm having trouble reading the output file, as shown below:

Code:

#      Time      f_in      f_out
      0.002          1          0
      0.004          1 1.923e-122
      0.006          1-3.486e-112
      0.008          1-3.193e-108

      0.01          1 4.059e-107

It is possible to control the printing precision? I've tried changing the writePrecison, but it did not work.

Code:

massFlowAverageC
    {
                type patchMassFlowAverage;
                functionObjectLibs ( "libsimpleFunctionObjects.so" );
                fields ( C );
                patches ( f_in f_out );
                factor 1.0;
                verbose true;
    }


Jonas Ansoni March 27, 2013 14:15

Hello Foamers!!

I'm calculating the RTD as described by Daniel, using patchMassFlowAverged. However, I need these values ​​to calculate the variance. I made a python script to perform these calculations, but I'm having trouble reading the output file, because some columns are getting together, as shown below:

Code:

#      Time      f_in      f_out
      0.002          1          0
      0.004          1 1.923e-122
      0.006          1-3.486e-112
      0.008          1-3.193e-108
      0.01          1 4.059e-107

It is possible to control the printing precision? I've tried changing the writePrecison (controlDict), but it didn't work.

Code:

massFlowAverageC
    {
                type patchMassFlowAverage;
                functionObjectLibs ( "libsimpleFunctionObjects.so" );
                fields ( C );
                patches ( f_in f_out );
                factor 1.0;
                verbose true;
    }

Thanks

chegdan March 27, 2013 15:05

what about making two function objects, one for f_in and another for f_out? they will be in separate folders and files.

Jonas Ansoni March 27, 2013 21:50

Hi Daniel!

Thank you for your prompt reply. I already tried that. The result was as shown below: :(

Code:

#      Time      f_out
      0.002          0
      0.004 1.923e-122
      0.006-3.486e-112
      0.008-3.193e-108

Best regards
Jonas

vanekp April 4, 2013 05:34

Quote:

Originally Posted by Jonas Ansoni (Post 416865)
Hi Daniel!

Thank you for your prompt reply. I already tried that. The result was as shown below: :(

Code:

#      Time      f_out
      0.002          0
      0.004 1.923e-122
      0.006-3.486e-112
      0.008-3.193e-108

Best regards
Jonas

I might not be the best to talk, but as I think, it should be possible to write a script that gets these values for you. The number of charakters in the lines is always the same. Might that be an idea?

Jonas Ansoni April 5, 2013 13:30

Good idea vanekp!!!

I did this and worked. Follows the python script to read this archive.

Code:

import numpy as np

time, c_out = np.genfromtxt(prjDirC, skiprows = 1, delimiter=(13,13), unpack=True)

Thanks...

jeicek May 14, 2014 15:17

Quote:

Originally Posted by vanekp (Post 413596)
Thank you all for the advice.

I was told the same thing about the patchMassFlowAverage by my colleague. So far I'm interested only in laminar flows, so the adjustment is not yet necessary but in the future I'll have to do it.

So I've set up everything according to the advice, I wrote a very simple shell script, which runs the sequence mySimpleFoam (simpleFoam with added solution of temperature) -> copying the velocity fields U and phi -> running scalarTransportFoam with patchMassFlowAverage function object included. So I'm now able to get the RTD curve quite nicely.

But now I'm dealing with problems with the solution. The velocity fields seem to be calculated well and when I run the scalarTransportFoam at the beginning everything seems to go right and at one point the solution goes totally 'bananas' and the Flow Average gets even negative (and even into range of -1e15) which I don't even understant how is it possible to go negative.

Do any of you have experince with this kind of behaviour and how to resolve it?

Hello guys

Can anybody help me?,, How should I implement the patchMassFlowAverage function object?

chegdan May 14, 2014 15:48

Quote:

Originally Posted by jeicek (Post 491861)
Hello guys

Can anybody help me?,, How should I implement the patchMassFlowAverage function object?


By reading through the post online and trying example like the one at

http://www.cfd-online.com/Forums/ope...tml#post416812

and looking at the wiki page here. You will need to compile the libraries outlined in the other post

http://www.cfd-online.com/Forums/ope...tml#post491866


All times are GMT -4. The time now is 11:41.