question about free surface in a model with magnetic stirring

[Anonymous]

Hi there,

I am trying to simulate the flow pattern in a tank with magnetic stirring, I did all the steps following the instruction in the forum but still cannot get expected results. And I also cannot see the option of the free surface when I do right click. what I can get is something like the picture show which I suppose is not correct because I cannot see the interface of fluid and gas. can anyone figure out what happens, any special details should be taken into consideration when I do this kind of simulation? I already refined and unformed the mesh for the stirring region and interface. 

[Jon.Wilde]

If you followed all the step, I think we might need to see the model to be able to efficiently help you. Could you share a support file (CFZ) with us?

Thanks!

Jon

[Anonymous]

Hi Jon,

Thank you very much for your quick reply. Sure I can share the model with you as attached. I suppose it should be like the below picture shows if I do free surface, but I cannot get that results. one more question is we can only see very limited vector compared with results, can I also do some settings to get more kind of vectors?

I attached the cfz file, please have a look. Cheers

[David.Short.]

Good morning @Anonymous,

Firstly when you want to model a free surface you must also model the air volume above it.

Take care however as must not assign air to this volume but assign the same fluid that is being stirred. You then assign the height of the fluid to your Ethylene Glycol volume as an initial condition. This is necessary because having fluid regions touching which have different fluid materials assigned causes solver error.

This documentation should help you get going!

I hope this makes sense and you can progress with your project.

All the best,

David

[David.Short.]

Hi @Anonymous,

Regarding vector visualization. Go to vector settings and pull the grid spacing slider down towards fine.

Thanks,

David 

[Anonymous]

Hi David, 

thanks for your kind reply, which is very helpful.

Actually, I got some other issues when I run the program. All the recommendations just say we should refine the mesh for the interface of fluid and gas when we do free surface, but how to decide whether it is good enough or not? how about 0.5 for my case? 

The videoes on Youtube show that we can just right-click to choose the free surface to see the interface but I cannot find that option. Is there anything goes wrong? 

The results I got after refining seem very hard to analysis, my computer always gets stuck when I see the results and the CPU usage is much less than 100%. is that because of the big data of the study or anything I can do to solve it?

Attached is the latest model that I set.

Cheers,

Jun

[David.Short. · Accepted solution]

Good morning Jun,

In terms of meshing for the free surface region I would start course and tighten it incrementally through a convergence study, meaning you must run multiple simulations (this is just the CFD way!). The mesh must be specific to the case so I can't really recommend a suitable refinement value.

Start with a course mesh (very little refinement) just to see where the free surface will end up during simulation as then you will have a rough idea of where you should refine the mesh. Then use a refinement region spanning the total area where the free surface interactions occur, both before stating the simulation and after convergence.

As a good starting point Matt (technical support in the USA) runs through a really good free surface example in this webinar (starting at minute 28:40), which relates closely to your project. This should give you a good idea of the mesh refinement requirements for your simulation.

Regarding:

The videoes on Youtube show that we can just right-click to choose the free surface to see the interface but I cannot find that option. Is there anything goes wrong? 

Please provide the link to a video where this process occurs as I haven't seen it before.

Regarding:

The results I got after refining seem very hard to analysis, my computer always gets stuck when I see the results and the CPU usage is much less than 100%. is that because of the big data of the study or anything I can do to solve it?

What are your machine specifications? as yes this could be RAM issue with the large mesh.

I hope this helps a little.

All the best,

David

[Anonymous]

Hi David,

Thank you very much for your kind help. These days I have been trying to simulate the model following your advice, it seems work currently, but I am still facing issues in terms of the time steps to run. For transient model, it seems the convergence plot can never be flat especially for my case, the velocity will keep fluctuating all the time. 

The simulation has been running for nearly 4000 iterations but still, the convergence plot does not show stable especially the area that I am interested (the second figure). could you please suggest that how to decide the simulation is good enough and I can say it is time to stop. 

meanwhile, I also attached the model that I am running now, could you please have a look that whether the setting is correct or needs any changes? Thank you very much 

[David.Short.]

Hi Jun,

I am glad to hear that you have been progressing with the project. 

When considering convergence of such a model it is probably most appropriate to look at the pressure data. Convergence data in Autodesk CFD is given as the average values through the model therefore when rotational flow is simulated the velocity convergence data is expected to oscillate. Therefore you you have converged pressure and nice smooth oscillations in the velocity plots then you can be fairly confident that the results are converged.

You should also look to see whether the free surface behavior looks smooth and realistic to give an indication of the validity of results.

Sadly I can't open your .cfz as it throws an error. Please test it on your machine and send a fresh one!

All the best,

David

[Anonymous]

Hi David,

Thank you very much for your kind reply. 

As we can see, the pressure get consistent very quickly probably like 200 iterations, but the oscillate plot of velocity does not look like repeated cycles especially for the area that I am interested in and I can see the obvious change of velocity and shear stress even though the pressure data if flat. Just wonder after getting convergence whether it means the velocity or other parameters will be the same or still keep changing? 

One more question is that for current simulation I see much deeper vortex than reality, which I assume is because I have suppressed almost all of the solid part of the model. But there would be friction or interaction between liquid and container which will reduce the spin speed, by that I mean, the RPM we set for the rotation region is higher than the reality. Am I right? Otherwise, the interaction of container to the liquid would reduce the movement of liquid to some extent. Should we consider that when we do the simulation? and how to do it?

Please see attached for the fresh file which was tested with my computer. It seems that I can only save as support file instead of archive or all results sets file which throws error all the time when I open them. 

[David.Short.]

Hi Jun,

Regarding convergence: Yes velocity convergence data will continue to vary once the simulation has converged as it is circular flow. However this variation should be smooth oscillations (representing the continual changes in flow direction).

Regarding friction: The frictional interaction between suppressed solids and the working fluid are still taken into account as the boundary between them are treated as non slip walls. You only need to mesh solids when you want to analyse heat transfer through them. In your case you can suppress all of the volumes except for the rotating region material and the working fluid volumes.

I think discrepancy with reality is due to the mesh. Apply refinement in areas of complex flow. Refinement regions should work well for this.

Hope this help,

David