# Fractional Flow Reserve (FFR) Estimation from OCT-Based CFD Simulations: Role of Side Branches
## 2 Material and Methods
### Blood Flow Modeling  
The 3D reconstructed vessel models (in STL format) were imported to ANSYS ICEM CFD V.19 (ANSYS Inc., Canonsburg, PA, USA), where the fluid domain was meshed using tetrahedral elements for the computational fluid dynamic (CFD) simulation. A grid independence study was carried out to confirm the ability of the mesh to calculate the pressure with a relative error <0.01%, and the final computational mesh contained ~500,000 elements for the idealized models and ~2,000,000 elements for the patient-specific vessel models. In addition, a prism layer mesh of 4 layers with an initial thickness of 0.02 mm and a growth rate of 1.3 was employed at the wall boundaries to well resolve the flow dynamics in the boundary layer region. During meshing, a mesh smoothing algorithm was initiated to maintain a specified minimum mesh quality of 0.3, which allowed the subdivision of the elements. The final mesh had an average skewness ~0.4, where the maximum skewness was less than 0.85. These mesh quality and skewness ranges are deemed as good-quality mesh in ANSYS ICEM CFD.  
The blood flow was modeled using CFD solver ANSYS CFX (ANSYS Inc., Canonsburg, PA, USA) by solving incompressible Navier-Stokes equations. A steady-state flow condition was used for calculating the FFR estimation. FFR is a time-averaged measure that is calculated over several cardiac cycles, and steady-state simulations have been used in previous work to estimate FFR [15]. Moreover, insignificant relative errors (<1%) between the transient and steady CFD solutions have been reported for FFR estimation [16]. Laminar blood flow was assumed, and a density of 1050 kgm\({}^{-3}\) was used.  
The fluid flow governing equations for the mass continuity and momentum conservation is given by Equation (1) and Equation (2), respectively.  
\[\
abla\cdot U=0 \tag{1}\]  
\[\rho(U\cdot\
abla)U=-\
abla P+\
abla\cdot\tau \tag{2}\]  
Here, \(U,\rho,P,\tau\) stand for velocity vector, density, pressure, and stress tensor, respectively. Stress tensor \(\tau\) is related to the strain rate by Equation (3),  
\[\tau=\mu(\
abla U+(\
abla U)^{T}-\frac{2}{3}\delta\
abla\cdot U) \tag{3}\]  
where \(\mu,\ \delta\) denote the dynamic viscosity of the fluid and Kronecker delta function. To model the viscosity \(\mu\), the Carreau model [17] was used. The Carreau model captures the non-Newtonian, shear-thinning behavior of blood using Equation (4),  
\[\mu=\mu_{\infty}+(\mu_{0}-\mu_{\infty})\left[1+\left(\lambda\hat{S}\right)^{2 }\right]^{\frac{n-1}{2}} \tag{4}\]  
where \(\mu_{\infty}\) and \(\mu_{0}\) are the viscosity value when the shear rate reaches infinity and zero, respectively. \(\hat{S}\) is the shear rate. \(\lambda\) and \(n\) denote the time constant and the power law index, respectively. The following values were used in the simulations: (\(\mu_{\infty}=\) 0.0035 Pa s, \(\mu_{0}=\) 0.25 Pa s, \(\lambda=\) 25 s, and \(n=\) 0.25) [18]. These values were selected by fitting the Carreau model to the viscometry measurements of [PERSON] et al. [17] obtained for whole blood over shear rates ranging from 0.01 to 50 s\({}^{-1}\).  
Ansys CFX employs second-order discretization in space using a finite volume method (FVM)-based approach. The second-order upwind scheme is selected for solving the momentum equation. The software solves the coupled continuity and momentum equations using a co-located grid approach [19].