[Thural]

Dear Users,

I am new CFX user and want to simulate aeration and mixing processes in wastewater tank.
My model is an open mixing tank which contains 2 horizontal agitators in different location and air diffuser grid on bottom of tank. it is a batch tank model.
Instead of using propeller for agitators, I have created subdomain 1 and subdomain 2 for each agitators. I used general momentum source and gave values (including low and high) to the proper momentum source component in order to obtain water flow inside tank.
However, there is only water flow inside and around of subdomains. Water velocity in the tank is zero.

I have seen and read relevant momentum source posts here but I still can not solve this problem. What might be the main reasons of zero velocity in the tank?
As far as I understand from the relevant posts, momentum source is the one of the main methods used to initialize the fluid flow.

Thanks in advance

[ghorrocks]

Please post an image of what you are getting and your output file.

[Thural]

Originally Posted by ghorrocks

Please post an image of what you are getting and your output file.

Good day,
I uploaded screenshot of CFD-post which shows the velocity but output file size exceeds the limit. Zip file size with compressed docx is still more than allowed size.

[ghorrocks]

The output file is a text file. Just post it as is, compressed if needs be. Don't put it in Word.

Your image is very weird. It shows some flow local to what I presume are the impellers, but also some bands of flow as well. This appears to not be conservative. Are you sure it is converged?

[Thural]

Originally Posted by ghorrocks

The output file is a text file. Just post it as is, compressed if needs be. Don't put it in Word.

Your image is very weird. It shows some flow local to what I presume are the impellers, but also some bands of flow as well. This appears to not be conservative. Are you sure it is converged?

Good day,

I have applied momentum source term approach with different values. The images of water velocity vector, plane and output file are below. I used "axial thrust of the mixers per cylindrical volume of subdomain" as a general momentum source and pictures, output file are belong to this method.
The result of simulation shows that water velocity vectors move out from the subdomain and return to backside by creating recirculation zone around of the each subdomain.
Also, I have used -C( Water.Velocity w - wspec) equation for momentum source term with momentum source coefficient. When I use high values such as C=10^5, max value of the velocity is too high which is not acceptable. Although water velocity is not zero inside the tank, there is recirculation around the subdomains again with very high speed(~100 m/s). it seems like after high speed recirculation around the subdomains, water flow destroy the barrier in front of them.
By decreasing value of C, I got reasonable values for water velocity, but there was no fluid motion inside the tank except around of subdomains like previous picture. And still have water flow recirculation around subdomains in each case.
What can be the reason of recirculation?

Thanks in advance.

[ghorrocks]

Firstly - in my previous post I requested you to just post the output text file, not to put it in word. But you have put it in word again. This is the last time I will look at a word file, I will be ignoring any future word files.

You have not defined a source term coefficient. It is very difficult to converge without this defined. Your problems look like you are just getting poor convergence and this is explained by you not using a source term coefficient.

[Thural]

Thanks for your quick reply. I have already used momentum source coefficient in my previous simulations and got similar results.

[ghorrocks]

Can I have a look at your output file again? Just post it as a text file, compressed if needs be.

[Thural]

Good evening,

You can find it in the following ZIP folder.

[ghorrocks]

* You are using single precision. Double precision will help.
* You have defined the time step size. How did you work this out? If it was a guess it is almost certainly wrong. Adaptive time stepping is recommended, homing in on 3-5 coeff loops per iteration. (UPDATE: I see your run is converging with 6 coeff loops per iteration so it is not too far off, but still a little bigger than recommended)
* You have not defined momentum source term coefficient. This is very important, it won't converge without this set correctly.
* you have set max coeff loops = 16, min=6. The recommended settings is max=10, min=0.
* Have you checked your convergence criteria is good enough? Have you done a sensitivity analysis?
* You can try the coupled volume fraction solver. Sometimes that helps a lot.
* You have second order time stepping. I would use first order while you do this basic debugging, and go back to second order once it is working reliably.

[Thural]

Mr. Horrocks,

Thank you for your detailed explanation and help. I am going to implement your ideas on the simulation as soon as possible.