## 3 Numerical Studies  
The application of the iFEM method for strain field reconstruction using uniaxial strain data is presented using an example problem of a biaxially loaded square plate. The reconstructed strain field is further assessed to detect the presence of damage on the plate. The plate had a length \(L=3.8\) m, thickness \(2t=3.8\) mm, and is made of an Aluminium alloy (Young's modulus, E = 73 GPa, and Poisson's Ratio, \(\
u=0.3\)). The plate is subjected to a uniform biaxial load of magnitude \(10^{5}\) N/m. The damage on the plate is modeled as a crack, and three different damage scenarios of the plate (varying size, position, and orientation of the crack) are investigated (see Figure 2a),  
* Damage Case-1: a 25 cm long crack is embedded at the center of the plate (crack position coordinates, \(\{x_{c},y_{c}\}=\{1.9,\ 1.9\}\)), with the crack front parallel to the vertical axis.
* Damage Case-2: a 10 cm long crack is embedded near the corner of the plate (\(\{x_{c},y_{c}\}=\{3.1,\ 3.1\}\)), with the crack front parallel to the vertical axis.
* Damage Case-3: a 25 cm long crack is embedded at the center of the plate (\(\{x_{c},y_{c}\}=\{1.9,\ 1.9\}\)), with the crack front oriented at \(45^{0}\) with the vertical axis.  
Because of the pure membrane loading involved in this example problem, only the first term in Equation (8) is relevant for this iFEM application [33]. This is because the membrane response is totally decoupled from the bending and transverse-shear deformations.  
A high-fidelity FE model of the plate is developed in ABAQUS using the S3R element, a 3-node constant-strain shell element with reduced integration. A mesh convergence study is performed to ensure the convergence of the FE results. The FE model provided the simulated experimental strain measurements required for the iFEM analysis. The embedded crack is modeled in ABAQUS using the seam feature [34], which created a set of overlapping duplicate nodes along the crack front. The FE model for Damage Case-1  
Figure 2: The damaged plate model showing: (**a**) crack size and position for all three damage cases (each crack represents a separate damage scenario), and (**b**) FE mesh used for Damage Case-1.  
used a total of 3368 elements, with a dense mesh near the crack tip (see Figure 2b). The uniform biaxial loading condition is implemented in the FE model by prescribing a uniform distributed load on the top and right edge of the plate and imposing symmetric displacement boundary conditions on the left and bottom edge of the plate. The iFEM analysis is carried out using the 4-node iQS4 element [25]. The iFEM mesh used has 16 elements along the plate length, leading to a total of 256 inverse elements (mesh is shown in Figure 3). The absence of suitable displacement boundary conditions in the iFEM model can lead to a singular system matrix, **K** (see Equation (14)), resulting in no available iFEM solution. Hence, the present iFEM model used symmetric displacement boundary conditions on the left (\(u=w=\theta_{y}=\theta_{z}=0\)), and bottom (\(v=w=\theta_{x}=\theta_{z}=0\)) edge of the plate (similar to the FE model).  
The results of the iFEM reconstruction are presented as contour plots of the maximum principal strain  
\[\epsilon_{p}=\frac{\varepsilon_{xx}+\varepsilon_{yy}}{2}+\sqrt{\left(\frac{ \varepsilon_{xx}-\varepsilon_{yy}}{2}\right)^{2}+\gamma_{xy}{}^{2}}. \tag{15}\]  
A damage index, \(I_{D}\), which provides a normalized value of \(\varepsilon_{p}\) within the range [0, 1] is also proposed  
\[I_{D}=\frac{\varepsilon_{p}-\varepsilon_{p}\big{|}_{\min}}{\varepsilon_{p} \big{|}_{\max}-\varepsilon_{p}\big{|}_{\min}}, \tag{16}\]  
where \(\varepsilon_{p}\big{|}_{min}\) and \(\varepsilon_{p}\big{|}_{max}\) define the minimum and maximum values of \(\varepsilon_{p}\) for a reconstructed strain field. The damage index is used in setting thresholds for damage localization.