(a) Simulations setup

The numerical solution of the continuity, momentum, energy and species equations was computed using a CFD proprietary code (ANSYS Fluent 16), based on the finite volume method. In this work, a steady state, three-dimensional, viscous, turbulent and incompressible (since the maximum Mach number is below 0.3) flow was assumed. Pressure–velocity coupling was taken care of by the segregated, pressure-based solver, the Semi-Implicit Method for Pressure-Linked Equations (SIMPLE) algorithm [33]. Summary details of spatial discretization are presented in Table 1. The convergence criteria were set to 10−<sup>6</sup> for the thermal energy and chemical residuals and 10−<sup>4</sup> for residuals from mass, momentum, turbulence kinetic energy and turbulence energy dissipation rate. Relevant physical and chemical quantities were monitored to assure convergence.



The governing equations solved are the continuity equation (Equation (21)), momentum equation (Equation (22)), energy equation (Equation (23)) and conservation equation for chemical species (Equation (24)):

$$\frac{\partial \rho}{\partial t} + \frac{\partial}{\partial x\_i} (\rho u\_i) = 0 \tag{21}$$

$$\frac{\partial}{\partial t}(\rho u\_i) + \frac{\partial}{\partial \mathbf{x}\_i}(\rho u\_i u\_j) = -\frac{\partial p}{\partial \mathbf{x}\_i} + \frac{\partial}{\partial \mathbf{x}\_i} \left[ \mu \left( \frac{\partial u\_j}{\partial \mathbf{x}\_i} + \frac{\partial u\_i}{\partial \mathbf{x}\_j} \right) \right] + \frac{\partial}{\partial \mathbf{x}\_i} \left( -\rho \overline{u\_i' u\_j'} \right) + \rho \mathbf{g}\_i + F\_i \tag{22}$$

$$\frac{\partial}{\partial t}(\rho c\_p T) + \frac{\partial}{\partial \mathbf{x}\_j} \left(\rho u\_j \mathbf{c}\_p T\right) - \frac{\partial}{\partial \mathbf{x}\_j} \left(K \frac{\partial T}{\partial \mathbf{x}\_j}\right) = \mathbf{S}\_T \tag{23}$$

$$\frac{\partial}{\partial t}(\rho Y\_m) + \frac{\partial}{\partial x\_j} \left(\rho u\_j Y\_m\right) = -\frac{\partial}{\partial x\_j} f\_{m,j} + R\_m + S\_m \tag{24}$$

Notice that for steady simulations, time-dependent terms become zero.

(b) Turbulence

A laminar regime was forced in the monolith because of small Reynolds numbers due to low velocity and very small hydraulic diameter inside channels.

In the other parts of the domain, Reynolds-averaged Navier–Stokes (RANS) approach was employed with the realizable *k* − *ε* model [34] selected. This model has the same turbulent kinetic energy equation as the standard *k* − *ε* model but holds an improved equation for *ε*. Compared to standard *k* − *ε*, it shows better performance for flows involving: planar and round jets (predicts round jet spreading correctly), boundary layers under strong adverse pressure gradients or separation, rotation, recirculation or/and strong streamline curvature [34].

(c) Computational domain

Simulation domain comprehends the area of interest for energy recovery. Great energy is lost in the muffler [35] and energy harvesting must be performed before it. After-treatment processes, such as chemical reactions within the DOC, might be affected by a temperature change caused by some sort of energy recovery device [36]. Consequently, energy recovery should take place between after-treatment devices and the muffler, as pointed out in [14]. The simulation domain includes the DOC and the exhaust pipe (see Figure 6). DOC must be included, since exothermal chemical reactions taking place in it can modify gas temperature. In order to obtain a properly-developed velocity profile at the inlet, an extruded entrance zone is added to the physical domain.

**Figure 6.** Three-dimensional geometry model of the exhaust system.
