Computational fluid dynamics
The CFD simulations were performed using ANSYS software (ANSYS Inc.,
Cannonsburg, PA). The geometry and mesh of a mixer was generated with
Workbench ANSYS 18.1 or newer versions (ANSYS Inc., Cannonsburg, PA).
For demonstration, the drawings of a SUM-100 mixer are shown in Figure 1
as an example. The computational domain of a mixer was divided into an
inner rotating cylinder zone centered with impeller and an outer
stationary zone. The diameter and height of the cylinder rotation zone
were ≥ 1.2-fold diameter of impeller (D) and ≥ 3-fold impeller blade
height, respectively. The interface between the rotating and stationary
zones was defined as Frozen‐Rotor interfaces. Since the impeller has an
angle from the vertical center line of the mixer, tetrahedral elements
were used in both zones of the mixer. The complete mesh consisted of
> 30,000 elements per liter, except for XDM-200 vessel that
had 2,647 elements per liter due to its simple cubic shape. In all
cases, the minimum orthogonal quality was > 0.15 and the
maximum skewness was < 0.90 to ensure acceptable mesh quality.
It should be noted that two outlets shown in Figure 1 do not really
exist in a mixer and they were added as the outflow boundaries to drain
out excessive fluid due to acid addition and keep a constant working
volume for simulation. The port diameter of an outlet equals to that of
the acid inlet. For these two outlets, one (outlet-1) was located at the
liquid surface as the mirror image of the inlet, while the other
(outlet-2) was located on the sidewall at the height of the impeller
clear distance. The volume fraction of two outlets were determined by
simulation tests.
CFD simulations were performed with ANSYS FLUENT 18.1 or newer version
using the k ‐ε turbulence model coupled with the species
transfer model. The first step simulation started with k ‐εturbulence model using the PAE as the only fluid under the steady
condition. All solid walls were no-slip boundaries. The top liquid
surface was the boundary of a flat surface with free‐slip wall. The
agitation speed was assigned to rotation zone and impeller shaft. All
other set-up parameters of the first step simulation used FLUENT default
values. The solution was converged when all residuals reached
< 0.0001 or simulation reached 10,000 iterations. The relax
factor of turbulent kinetic energy (k ) and turbulent dissipation
rate (ε ) were the first order of windup in the first
2,000 iterations, and then shifted to the secondary order of
windup if the solution was not converged.
After converge of the initial k ‐ε turbulence model, the
species transfer model was added for the second step simulation, the VIA
simulation. The FLUENT set-up parameters are presented in Table II. The
boundary of inlet was changed from wall tomass-flow-rate-inlet using the PAE as the inlet fluid at the
target flow rate, while the boundaries of outlet-1 and outlet-2 were
changed from wall to outflows with volume fractions of
designed values. The simulation was performed under steady condition for
2,000 iterations. This transient sub-step was required to introduce and
stabilize inlet flow. The simulation was then shifted into the
transition condition and the inlet fluid was changed from PAE to 0.1 N
HCl. The simulation time step was 0.05 s. At each time step, the
solution was converged when the values of all residuals reached
< 5 × 10-5 or iterations reached 20.MF0.1N HCl was defined as the volume-averaged
mass fraction of 0.1 N HCl and its value was recorded at each time step
during simulation. Iso-surface of a MF0.1N HClvalue could not be defined yet at 0 s, which would be done at 1 s flow
time. The simulation was paused at 1 s flow time. Iso-surface of pH 3.3
was defined by the corresponding MF0.1N HCl value
as the boundary of low-pH zone. The simulation was then resumed and the
vertex-averaged area of pH 3.3 iso-surface
(ApH3.3 ) value was recorded at each time step
during simulation. The simulation was complete when the flow time
reached the VIA duration.