Learning Forum

[Anh Khoa To]

Hello everyone,

I am currently working on a simulation of a stirred tank using a Rushton turbine in ANSYS Fluent. The tank contains glycerin (with a density of 1260 kg/m^3 and viscosity of 600 cP) up to 30 cm, while the total tank height is 42.5 cm with air above the glycerin. To model these two phases, I used the Volume of Fluid (VOF) approach.

For the impeller rotation, I employed the sliding mesh technique. To better observe the flow dynamics, I introduced PVC particles as tracers, which have a density of 1380 kg/m^3 and are located at the tank's bottom. These tracer particles are modeled in Fluent using the Discrete Phase Model (DPM) with a diameter of 3mm, a mesh size of 1mm, and physical models including Saffman lift force, virtual mass force, pressure gradient force, and stochastic collision.

Viscous model used was laminar as impeller Reynolds number <100.

I've set up the simulation with SIMPLE for pressure-velocity coupling, and for spatial discretization, I'm using PRESTO! for pressure and Second Order Upwind for momentum. The volume fraction is treated with the compressive scheme, and least squares cell-based method is used. For the DPM particle injection, I used a surface injection with 18,668 particles.

However, at 0.931 seconds into the simulation, I encounter a floating-point error, despite having good mesh quality (minimum orthogonal quality of 0.48 and maximum skewness of 0.48).

Has anyone encountered a similar issue or does anyone have suggestions on how to resolve this floating-point error?

Any help would be greatly appreciated!

Thank you.

[Anh Khoa To]

here's the particle tracking picture at 0.928s, I don't know why the particles have higher velocity than the fluids.

[Rob]

I'm not sure what the image is showing me, but unless the impellor tip speed is around 7m/s you have a problem. 

Are you adding particles constantly, or only for a short period? How does the flow field look prior to it failing? Is the failure repeatable, or can you restart from a saved case & data and run beyond the initial failure time? 

[Anh Khoa To]

Thank you for your insights.

Tthe impeller tip speed in my simulation is approximately 0.8 m/s. The simulation results were consistent with expectations prior to the implementation of the DPM model.

1. I'm observing an unexpectedly high particle velocity magnitude of 720 m/s in my simulation results. While the velocity vector direction aligns with a previous particle-free simulation, the magnitude appears unrealistic.

2. To replicate experimental conditions, I've configured a single particle injection event at the simulation's start, with a stop time of 1e-8. 

3. My current time step size is 0.0005. I've attempted to reduce it to 1e-6 to address the error, but it persists. Further reductions would introduce computational constraints, making it infeasible to complete the simulation within a reasonable timeframe.

[Rob]

That looks like the particle volume fraction is excessively high, and that's giving you nonphysical source terms. Rather than a surface injection try a smaller volume somewhere in the domain, or release from the impellor mrf surface. 

[Anh Khoa To]

Thank you sincerely for your assistance.

I've come across recommendations on CFD forums suggesting that particle diameters should be less than 1/10th the size of the smallest mesh element. Could this guideline be a factor in my simulation, given that my particle diameter (3mm) exceeds my minimum mesh size (1mm)? Additionally, could the specific physical models I've chosen be contributing to the unexpectedly high particle velocities? Would switching from a stochastic collision model to a DEM  collision model potentially address the unexpectedly high particle velocities I'm observing?

[Rob]

Yes, particles need to be smaller than the cells - the approach assumes a point mass so if you break the guideline the source term maths gets messy. Don't go to the DEM model, that's computationally overkill for what you're doing and still has the cell size requirement. 

Have a look at what the particles are for. Do you need that many? Do they have to be 3mm? Do they need to be coupled with the flow? 

[Anh Khoa To]

Thank you so much

Because I did an experiment to observe the movement of particles in the flow, the particles used in the experiment had a diameter of 3mm, so I had to set the size like that.
If I divided the mesh more coarsely, the mesh quality could not be guaranteed even though I tried many times. With the smallest mesh size of 1mm, can I accept the error and work with a particle with a diameter of 1mm?

[Rob]

Turn off the particle interaction with the fluid. What are you trying to find out using the particles?  

[Anh Khoa To]

Thank you very much for your advice.

I use particles to see the phenomenon of particles being attracted to the low pressure area created by the impeller in the stirring vessel, and I also want to see the distribution of particles.

 

[Rob]

OK. Do they need to be tracked with the fluid through the whole simulation time, or can you run them on a frozen flow field for post processing? Ie solver the flow and then run particles afterwards. This assumes the particles don't effect the fluid flow. 

[Anh Khoa To]

In my experiment, the particles were initially placed at the bottom of the stirred tank before the mixing process began. I would like to replicate this setup in my simulation as well.

I have tried coarsening the mesh to ensure that the mesh size is larger than the particle size, but this has not been successful.

What do you think about the possibility that stochastic collision is not suitable and is causing the unphysical behavior I am observing? Could I assume that particle collisions can be neglected and perform a one-way coupling simulation? The total particle volume is 1.25% of the fluid volume.

[Rob]

Remember that if you're adding particles to the wall surface that it's the particle centre that's added there, so they're inside the viscous sublayer and may not want to move. Inject from a little higher up. With a volume fraction that low the particles shouldn't influence the flow, and are unlikely to collide - you shouldn't need the collision model. 

[Anh Khoa To]

Thank you for your valuable advices. I greatly appreciate that.

To address the particle injection position, could I utilize a solid-cone injection with a velocity of 0 to precisely place particles in the desired initial location? Also with cone injection, I can adjust number of particles.

 

[Rob]

I'd just put a plane/isosurface in a bit off the bottom. Parcel count doesn't really matter provided you have enough to show what's going on. 

[Anh Khoa To]

Thank you.

I have created iso-surface and olane but it doesn't seem to show up when using surface injection. Sorry to bother you, but how do I add surface for this injection?

[Rob]

Oops, you need to create a Plane. Isosurface might be on the enhancement list.... Sorry! 

[Anh Khoa To]

I know I'm asking too much, so sorry but plane seem not to work too. 

[Rob]

Ah, I'm using 2024R1, it must be a more recent addition to the code. I suggest updating, or have a look at injection files to position the particles if that's not possible. 

[Anh Khoa To]

Thank you so much. But as I mentioned above, could I utilize a solid-cone injection with a velocity of 0.

[Rob]

Yes, just be aware of what you're setting. 

[Anh Khoa To]

Thank you so much.