## 2 Materials and Methods
### Numerical Model and Data-Driven Determination of Material Properties  
In this section, the characterization of the material response obtained with the tensile test and DIC is presented and how it has been used to calibrate a mesoscale model. Twill carbon fiber fabric is constituted by orthotropic bundles of fibers (tows) interwoven in \begin{table}
\begin{tabular}{c c c c c} \hline
**Specimen** & \(I\) [mm] & \(w\) [mm] & \(D\) [mm] & _w/D_ \\ \hline C20 & 250 & 24 & Unnotched & — \\ C21 & 250 & 24 & 2 & 12 \\ C22 & 250 & 24 & 4 & 6 \\ C23 & 250 & 24 & 8 & 3 \\ C31 & 250 & 36 & 3 & 12 \\ C32 & 250 & 36 & 6 & 6 \\ C33 & 250 & 36 & 12 & 3 \\ \hline \end{tabular}
\end{table} 
Table 1: Specim dimensions: length \(l\), width \(w\), hole diameter \(D\), and width-to-diameter ratio _w/D_. Figure 1: The 2 \(\times\) 2 twill fabric unit cell. (**a**) Detail of the specimen surface captured before testing; (**b**) schematization of the previous image, showing how the vertical (warp) and horizontal (wref) fiber tows are woven; and (**c**) further simplification used to build the FEM, with two material orientations (shown in two shades of gray) and two layers of integration points. Global coordinates are shown in black, with \(y\) being the tensile loading direction. Local material coordinates are in orange; 1 is the “fiber direction” and 2 is the “matrix direction” [25]. orthogonal directions, as is visible in an image of a specimen in Figure 1a and represented schematically in Figure 1b. Under mechanical loading, complex stress and strain fields arise in the material due to this heterogeneity. While the surface strain field is readily available via DIC, obtaining the stress field requires further processing of the experimental data. This study made use of a simplified 2D shell finite element model that is able to properly capture the stress, as was developed in [25]. A more concise description of the model is reported in this section. Each open-hole tensile test was reproduced numerically with a finite element model, replicating each specimen's specific material distribution. The mesoscale heterogeneity is modeled using two orthotropic materials with identical properties and orthogonal orientations (Figure 1c). A map of the fiber orientation on the surface of the specimen is reconstructed, using image processing and positional data from DIC, and the material orientation is assigned to each corresponding element in the FEM with an automated algorithm developed in Python. This mapping process, implemented in MATLAB R2021b, is described in Figure 2. The rows with vertically aligned fibers are visible in the images of unpainted specimens, due to their reflectivity. Their location on the specimen's surface is identified via a K-means image clustering on the image and also via position data from the calibrated DIC analysis. A map of the material orientation is then built using the known unit cell dimensions of the twil fabric. The finite element mesh is automatically generated from the specimen image with the open-source meshing software GMSEH v.4.8.4 and parsed to LS-DYNA ([[https://lsdyna.ansys.com/](https://lsdyna.ansys.com/)]([https://lsdyna.ansys.com/](https://lsdyna.ansys.com/))). The laminate is modeled with a single layer of four-node Belyhtscko-Tsay shell elements with a number of through-thickness integration points equal to twice the number of layers in the specimen. Each ply in the physical composite specimens is, indeed, represented by two layers of through-thickness integration points, to capture the structure of interlocking rows (Figure 1c). A mesh convergence study led to the identification of an ideal mesh size of 0.5 mm, corresponding to 10 \(\times\) 20 elements for each fiber tow. Mesh refinement around the hole gave a minimum mesh size of 0.05 mm. The material model used was orthotropic linear elastic *MAT_002 from LS-Dyna.