[Joe walker1]

For a project I am simulating a 2D sliding mesh model of a rushton turbine mixing tank on ansys fluent.
I am currently struggling with measuring mixedness. I was wanting to simulate 2 different coloured waters mixing time.
https://www.afs.enea.it/project/nept...ug/node342.htm
I was trying to follow this guide but I don't understand what to do with the cell conditions.
I generally need guidance about how to do the whole process, any advice is greatly appreciated.

[NickFL]

This can be done in a number of ways. One way that is often done it to create a mixture of two fluids with the same property. I am assuming it is a closed mixing tank (i.e. no inflow/outlfow). If so, then simply patch a small region of the domain with the tracer fluid. You can then create volume monitors on the transient run for min/max/average values of the tracer. From here you can see how the tracer is distributed in the domain.


Furthermore, if you have created a steady-state flow field, you could even turn off the solution for the continuity/momentum and turbulence equations. This means it is only solving scalar transport, and that is much quicker.

[Joe walker1]

Hi,
Thank you for the response. I am still quite new to fluent so I have a question regarding the last part of you message. When you say steady-state flow field, do you mean I run the solver until my results have converged, then follow you guidance afterward?

[NickFL]

Yes what I am calling a steady-state solution is a solution that is converged, not just to residuals are under 1e-3, but really drive them out to where it approaches an asymptotic. Then you know that is as good as you are going to do with that grid. Also monitor other points and verify they are not varying with iteration.



Once you have that flow field, by turning off the flow and turbulence equations, you are basically just freezing it. As long as your second mixture fluid has the same properties as the first, then we can just solve these (actual "the" because it only solves one) transport equation(s) because the flow field wouldn't change. Think of it like putting dye in the water, we are just giving some of the material a new name so that we can follow it.

[Joe walker1]

Brilliant thank you.

[Joe walker1]

Hi, is there any change you can help me through the process again. I have completed the transient run, and turned off the energy equations, but I am confused as to whether I am adding a multphase "mixture" or I am just adding a species transport in the models tab.
am attempting to follow https://www.eureka.im/5375.html
As well as your guidance but I feel that there is some conflicting instructions in this link.

Any help is greatly appreciated.

[NickFL]

It is a multi-species simulation that you need to run.

1. Create a mixture with 2 components, let us say fluid-1 and fluid-2. Remember to keep the material properties the same.
2. Turn off the flow, turbulence and energy(?) equations. You should only have the 1 species equation left.
3. Create a small region in your domain. You will want to patch fluid-2 a Mass Fraction (MF) of 1 to this domain and leave MF of 1 everywhere else in the domain. Keep in mind to patch MF of 1 to fluid-2 to the region, we would set the MF of fluid-1 to be zero.
4. Create a monitor of max facet value, min facet value and volume average value of fluid-2. You can set up a plot and even write it to a file for post-processing in Excel or other programs.
5. Create contours of the fluid-2 component. Then create animations for these contours. The new cxa animations work quite well in Fluent.
6. Run the simulation.



I think that should be it.

[Joe walker1]

Hey, really appreciate the continued help. Not to pester you, but I am still having issues with my simulation. I believe I have set the simulation up as described, but it seems the patched region doesn't disperse through the transient run.
I believe I followed everything as described, however I only have the option of patching the phase 2 fluid.

I've attached a picture of the patch section and the contour at the final time step.
https://smallpdf.com/file#s=8b50551d...3-57575acc34cb

The patched region crosses the sliding mesh and the stationary region, however only the area of fluid inside the impeller region is dispersed.

Thanks again,
Josh

[NickFL]

Originally Posted by Joe walker1

I only have the option of patching the phase 2 fluid.

You mean species 2? The mass fraction of Species 1 is simply (1 - MFs2) where MFs2 is the mass fraction of species 2.


I cannot see your image. Use the image hosting on this forum it works well. Look at the steady state velocity contours. Do they make sense. When you patched the speices 2, you didn't re-initialize the flow field by mistake did you?

[Joe walker1]

Hi,
So upon reviewing the velocity contours, after I start the second simulation the velocities cease to be continuous over the 2 regions. Any suggestion to remedy this?

Thanks again Josh.

[NickFL]

Can you upload the images so we can see? If you turned off the flow equation solver, then the velocity field should not change.

[Joe walker1]

Hi, I have attached screenshots of what I've done. And I will attach pictures of the flow field after turning the equations off, in the next post.

[Joe walker1]

And this is the velocity profile and volume fraction of the second species after the sim is ran.
The section of the fluid inside the sliding mesh rotates but doesn't disperse and the section outside the impeller region just remains stationary.
Could it be that I should have the flow equation enabled and the turbulence model is the only one that should be disabled?

[NickFL]

You have it set up as a multiphase, but want a multi-species. And it looks like you reset the velocity field when you went to patch the dye to the volume. You just need to patch the one species equation and do not change the velocity.

[Joe walker1]

You're absolutely right! I had been using a multiphase mixture instead of a species transport model.
Everything is running fine now.
Thank you so much for staying with me, you've been amazing help!
I'm tempted to add you to the acknowledgments page of my thesis haha.

[NickFL]

Glad you did it correctly in the end. I've been doing this nearly 20 years now, so I have seen and made a lot of mistakes. It is better to get it fixed before you finish your thesis. It is never good to see big mistakes at the defense and after the thesis has been printed.


Good luck to you at your defense and remember you know the topic better than anyone in the room.