I want to calculate the mass of recirculation in a flow field using CFX post. Any idea how to calulate it. Any help on this regard will be appreciated. Thanks in advance. Kali

Hi,

Define a plane or some sort of surface which the recirculating flow goes through and use the function tool to get the mass flow rate of it. You can define the plane/surface manually or define some sort of isosurface which defines it.

Regards, Glenn Horrocks

Glenn, Its not easy to define a plane or iso-surface defining the individual recirculating zones. Please tell me if you have any other idea. Thanks, Kali

If you want to calculate the mass flow of the reversed flow in a specific plane in an area with recirculation, here's how to do it:

1) Create the plane of interest 2) Create a Contour Plot based on the plane with Velocity u (or v or w) as variable. Set range to User Specified and min = -100 and max = 100, or other symmetric values that extend the velocities. Set the # of Contours to 3! That gives a contour plot with 2 colours. One colour being positive u values and the other negative values. 3) Create a User Surface with the "From Contour" method. Set the Contour level to 2 or 3. 4) Calculate the mass flow of the User Surface using the function Calculator. massFlow()@User Surface 1

Michael Bo

Hi Kali,

It seems like you want the mass, rather than the mass flow (net mass flow would be zero anyhow).

You might be able to create an isovolume (Volume object) based on Total Pressure. Typically, the total pressure within the recirculation zone will be much lower, due to the losses. From this isovolume you can then calculate the total mass.

Alternatively, you could add an "Age" variable to your solver run. This will calculate the age of the fluid as it passes through your domain. Since fluid gets held up in a recirculation zone, the "Age" will be greater than that outside the recirculation.

To calculate Age, go back to Pre and create an additional variable of type "Volumetric" and units of [s].
LIBRARY:
ADDITIONAL VARIABLE: age
Option = Definition
Units = [s ]
Variable Type = Volumetric
END
END
Under Domains>Fluid Models, activate the additional variable ans set the option to Transport Equation. Leave Kinematic Diffusivity unchecked.
FLOW:
DOMAIN: StaticMixer
FLUID MODELS:
ADDITIONAL VARIABLE: age
Option = Transport Equation
END
END
END
END
Create a subdomain which includes your entire domain mesh with a source term for Age equal to 1 [] (i.e. 1 second per second). This source term will then accumulate time, as the integral of 1 dt is 't'.

If you like, you can turn off the other equations by adding the appropriate model override parameters, for instance:

FLOW:
EXPERT PARAMETERS:
solve energy = f
solve fluids = f
END
END

Finally, you may want to increase your timestep, at least on the age equation. This will speed things up significantly. You should only need a few multiples of you timescale to be done. Don't bother converging, especially if you have a recirculation zone, as time will continue to accumulate in these areas, causing the solution to stall.

Now write the def file and run it. Hopefully this works out for you.

Best regards,
Robin

Hello Kali,

The most important is that you define the boundary of the vortex. This itself is an active area of research. Some of the criteria are the ones suggested by Glenn and Robin. You could also do a google search on (vortex, definition, Hussain) and you will see that there are a number of definitions and each of them is good for certain type of flows. A recent article of Haller could give you an idea: http://web.mit.edu/ghaller/www/vortex.pdf

I have used in the past the helicity and the second invariant of the velocity gradient. These are quite easy to implement in post using CEL and work quite well for internal flows.

I hope that this helps a bit.

Kind regards, Yulian

Hello Robin, I am also working on similar problem to determine Residence time distribution.I defined AGE variable and Subdomain and started the simulation with previous result file as Initial guess.But i got an error message " The following objects have been referenced but not defined:

SUBDOMAIN: Subdomain 1

ccl2flow: * command language error *

Message: Undefined references

Context: define_name_table "

Then i started the simulation without initial guess and it is running without any errors.My previous result file has no sub domains defined. Do i need to define Sub domains for the first run?

Please help me. Thank you. Regards, Siva

Hi Siva,

This problem can be resolved by using the interpolate option with your previous results file.

CFX does not seem to recognise the old and new domains to be the same due to the new sub-domain. Interpolating the old results will overcome this.

Regards

Paul

Hello Paul, Thank you very much for your help. I have one more question regarding interpolation. I did interpolation from command prompt. After interpolating results to new definition file it will stop by saying " * Finished interpolation successfully. * ". My question is do i need to use the old result file as initial guess for new run? or can i start directly from newly interpolated definition file?

Because,if we start from GUI it will automatically start the run after interpolation whereas from command prompt first we use cfx5interp command and in the next step we start the simulation with cfx5solve command.

Regards, Siva

Hi Siva,

You should start directly from the .def file. (Help files > Solver Manager > Managing Your CFD Run > Tools Menu > Interpolate)

The old results file has not been changed so contains all the values for the old domain without the sub-domain. This is no longer of any use.

Have Fun

Paul

[ashtonJ]

Dear all,
I would like to measure the mass or the volume of recirculation zone. Has anybody figured out how to do that? If yes, please let me know.
Thanks
AshtonJ

[ghorrocks]

The first problem is you have to define the recirculation zone. This is not easy in 3D in general, but for your flow there may be a definition.

[ashtonJ]

Hi Glenn. I identify the recirculation zones in 3D based on flow streamlines. I just need to figure out how to quantify the recirculation regions.

[ghorrocks]

No, I mean define them mathematically. Sure, you can draw streamlines and the recirculation is obvious, but writing a mathematical function which matches the obviously visible streamline is not easy.

Once you can define the recirculation mathematically then it is easy: You define that as a region in CFD-Post and use the calculator to give the volume.

I am not aware of a universal definition of a recirculation volume so you are going to have to find some way of defining it for your case.