Applying Computational Fluid Dynamics Technology in Bioprocesses-Part 1 - Computational fluid dynamics is a powerful tool to optimize processes. - BioPharm International
Applying Computational Fluid Dynamics Technology in Bioprocesses-Part 1
Computational fluid dynamics is a powerful tool to optimize processes.
 Apr 1, 2010 BioPharm International Volume 23, Issue 4

MODEL SETUP

The key to a successful CFD analysis of a bioprocess is to choose correct models based on underlying physics and biochemistry. These models also require the right boundary conditions and initial conditions.

Currently, there are two broadly categorized computational approaches for modeling the interaction between phases in multiphase flows: the Euler-Lagrange approach8–11 and the Euler-Euler approach.12–17 In the Euler-Lagrange approach, the fluid phase is treated as a continuum by solving the time-averaged Navier-Stokes equations, whereas the dispersed phase is solved by tracking a large number of particles through the calculated flow field. The Euler-Lagrange approach typically deals with the dispersed second phase by occupying a low volume fraction, even though high mass loading is acceptable. The particle trajectories are computed individually at specified intervals during the fluid phase calculation. In the Euler-Euler approach, the different phases are treated mathematically as interpenetrating continua. Because the volume of a phase cannot be occupied by the other phases, the concept of phasic volume fraction is introduced. These volume fractions are assumed to be continuous functions of space and time and their sum is equal to one. Conservation equations for each phase are derived to obtain a set of equations that have similar structures for all phases. In both approaches, the continuum phase and discrete phase momentum equations are coupled through the drag source and sink terms, and through the volume fraction of the dispersed phase.

The flow in an agitated bioreactor typically is in a fully turbulent regime, although some emulsification processes may operate in a laminar or transitional regime because of the high viscosity of the mixture. Two methods often used to model the turbulent flow are the Reynolds-averaged Navier-Stokes (RANS) models and the unsteady large eddy simulation (LES) models. The direct numerical simulation (DNS) method is too computationally demanding for real applications.

RANS-based models have different variations, such as the standard k-epsilon, the Chen-Kim, the renormalized group (RNG), the realizable k-epsilon, and the k-omega, which all assume isotropic turbulence and do not show superiority of one over another,18 and the Reynolds stress transport models (RSTM), which incorporate the anisotropy characteristics by solving transport equations for Reynolds stress terms. However, the improvement on the accuracy of RSTM predictions over the k–e models is not conclusive.19–24 Based on the Kolmogorov theory, the LES models solve only for the large eddies explicitly, while the small-scale effects, below the filter size with corresponding wave number lying in the inertial convective subrange of the energy spectrum, are modeled using a sub-grid scale model. Good agreement between experimental data and model predictions on mean velocities and turbulence quantities in agitated tanks have been reported.22,25–33 LES requires less computational effort than direct numerical simulation (DNS), which is the most exact approach to model turbulence and can resolve the smallest eddies, but uses significantly more effort than methods that solve RANS.34

When modeling a rotating system such as in an agitated tank, the multiple reference frame (MRF) and the sliding mesh (SM) model often are used. The MRF model performs a steady-state calculation with a rotating reference frame in the impeller region and a stationary reference frame in the outer region. In this way, the effects of the impeller rotation are accounted for by the frame of reference, allowing for explicit modeling of the impeller geometry. The SM model allows the impeller region to slide relative to the outer region in discrete time-steps and performs time-dependent calculations using implicit or explicit interpolation of data at successive time-steps. The SM model is a more accurate representation of the actual phenomenon of the impeller rotation, but unfortunately a computationally demanding one.

The predictive capabilities of all available CFD models when applied to agitated bioreactors equipped with various impellers in up- or down-pumping mode are discussed in the reviews.23,24,36–38 In summary, all turbulent models can predict the mean flow-field and power number very well,23,30,31,39 and also can capture most of the key features of near-impeller flows with sufficient accuracy, but provide various degrees of agreement with experimental data on turbulent characteristics. The standard k-epsilon turbulence model combined with the MRF model, as commonly used in engineering CFD simulations of stirred tanks and often faulted for its assumption of isotropic turbulence, can model the turbulent flow with adequate accuracy if fine enough grids coupled with higher-order discretization schemes are used.38 The LES for modeling flow in stirred tanks has the advantage of capturing the instantaneous velocity field and vortex structures.22,25,28,30,31,40

 Figure 1
Cells growing in bioreactors take up nutrients from the culture medium and release products, byproducts, and waste metabolites. Mixing and sparging greatly influence the mass transfer phenomena required for an adequate supply of nutrients and removal of waste metabolites.35 Agitation is used to maintain cells in suspension, provide a homogeneous mix of nutrients, and prevent the accumulation of toxic gases. Multiple tasks and numerous choices of impellers make process scale-up extremely challenging. Figure 1 illustrates how CFD provides assistance in understanding the extracellular environment, optimizing the operation conditions, designing hardware configuration, and implementing scale-up and scale-down strategies.