## 2 Materials and Methods
### Numerical Modelling  
As it has been reported in the introduction, to increase and develop the use of a geopolymer mortar (with or without fibers) in the construction industry, a fundamental step is to check the affordability of the available material model to be implemented in FEM software. This remark is even more important for the geopolymers intended as a new type of concrete, and therefore, affordable numerical models are required to design structures realized with such materials. Among FEM software, ANSYS is one of the leading one, and it was adopted in this paper to numerically reproduce the experimental results reported in the next section. As a material model available in the ANSYS library, the selected one was the coupled damage-plasticity microplane, which is regarded as very affordable in the case of simulating engineering materials consisting of various aggregate compositions  
Figure 1: Experimental set-up: (**a**) compression test (the specimen is located inside a specific joint device as prescribed by the relevant standard); (**b**) splitting test; (**c**) three-point bending test.  
with differing properties (for example, concrete modeling, in which rock and sand are embedded in a weak matrix of cements). The numerical analysis was performed iteratively assuming the Young' modulus \(E\), the ultimate strength in compression and that of the splitting test (obtained from the experimental tests as described in the next section) and the Poisson ratio \(\
u\) (equal to 0.2, from literature) as known parameters. The microplane model requires the following parameters to be assigned: the biaxial strength \(f_{b}\), the coefficient \(D\) (governing the hardening of the material), the \(\gamma_{c0}\), \(\gamma_{t0}\), \(\beta_{c}\) and \(\beta_{t}\) parameters, which govern the damage behavior (\(\gamma_{c0}\) and \(\gamma_{t0}\) represent the damage thresholds, \(\beta_{c}\), and \(\beta_{t}\) represents the damage evolution constants) in tension and in compression, the parameters \(R_{c}\) and \(R_{t}\), representing the cap hardening constants (in compression and in tension, respectively) and the parameter \(\sigma_{cv}\) (representing the intersection of the compression cap and Drucker-Prager yield function). A detailed explanation of the meaning of these parameters can be found in the ANSYS manual [41] and in the references reported. Following the suggestions in [41], for all the fiber contents, \(f_{b}\) was set equal to 1.38 \(f_{c}\) (compressive strength), and the parameter \(R_{c}\) was set to 2, \(R_{t}\) to 1, \(\sigma_{cv}\) to \(-6.66\) MPa and \(\gamma_{t0}\) to zero. The adopted values of the remaining parameters are reported in Section 3.2. The first step was to perform preliminary analyses to check the mesh convergence, and in Figure 2, the adopted models for the compression, splitting and three-point bending tests are respectively reported. The element type for geopolymers was CPT215, whereas the supports were meshed with 8-node SOLID185. Surfaces subjected to contacts were meshed with a CONTA174 contact element assuming a frictional coefficient equal to 0.2. The analyses were conducted in the displacement control with a rate of 0.005 mm/min.  
Figure 2: FEM models: (**a**) compression test; (**b**) splitting test; (**c**) three-point bending test.