Numerical Simulation of the Mechanical Behavior of Fiber-Reinforced Cement Composites Subjected Dynamic Loading

: The problem of damage accumulation in ﬁber-reinforced concrete to structures supporting underground workings and tunnel linings against dynamic loading is insufﬁciently studied. The mechanical properties were determined and the mechanism of destruction of ﬁber-reinforced concrete with different reinforcement parameters is described. The parameters of the Concrete Damaged Plasticity model for ﬁber-reinforced concrete at different reinforcement properties are based on the results of lab experiments. Numerical simulation of the composite concrete was performed in the Simulia Abaqus software package (Dassault Systemes, V é lizy-Villacoublay, France). Modeling of tunnel lining based on ﬁber-reinforced concrete was performed under seismic loading.


Introduction
In recent years, a significant number of scientific papers have been devoted to the development of new compositions of cement matrices and the use of modified multicomponent fibers in concrete compositions for static and dynamic loads [1][2][3][4].
Determining the mechanical properties of fiber-reinforced cement composites under dynamic loading, establishing correlations among their composition, structure and properties, justifying the correct mathematical model and determining its parameters represent a complex problem at the moment. If this problem is solved, the efficiency of building structures operating under dynamic loading can be improved, i.e., with respect to an economic point of view because of lowering material consumption and correct results of analytical and numerical approaches.
The Finite Element Method (FEM) is commonly used in determining the non-linear relationship of force-displacement and following crack development in reinforced concrete [5,6]. The analytical model of plastic behavior of polymeric fiber and concrete is quite complicated [7,8]. In this study, the commercially available Simulia Abaqus software package was used. Using Abaqus for performing the computational experiment makes it possible to reproduce the phenomenon in the most detailed way, including visualization for analysis and comparison of the obtained numerical data with experimental results [9][10][11][12][13].
The analysis of scientific publications in the field of research showed that problem of damage accumulation in concrete and fiber-reinforced concrete tunnel linings under dynamic loading is insufficiently studied [14][15][16][17].
The aim of the paper is to substantiate the mechanism of damage accumulation in the tunnel lining with the circular outline using the model of plastic behavior of concrete for the evolution of damage. For discrete reinforcement of concretes, BarChip 54 macrofiber was used. Macrofiber quantities were 0, 3, 5 and 7 kg/m 3 . The mechanical properties of macrofibers are indicated in Table 1.

Test Methods
Compressive strength tests were performed according to EN 12390-3 [18] standard. In these tests, cubic specimens with dimensions of 150 × 150 × 150 mm were used. They were brought to destruction directly between the flat steel plates of the testing machine.
Crack Mouth Opening Displacement (CMOD) tests were conducted as per the requirements of the EN 14651 [19] standard. Specimens in the form of a prism (beam) were used to determine the relationship of force-CMOD. The ratio of height to width (diameter) of specimens was assumed to be 4. The requirements for preparing the specimens have to comply with the BS EN 12390-1 [20] standard. The value of CMOD is the movement of the external faces of the incision made in the center of specimen when it deflects from the loading. The width of the slot on the specimen should not exceed 5 mm and its depth should be 25 mm ± 1 mm.
For laboratory research, the "Toni Technik ToniPRAX" testing machine (Toni Technik Gmbh, Berlin, Germany) was used, which implements uniaxial compression of the specimens with a maximum force of 3000 kN and three-point bending of the specimen with a maximum force of 100 kN. The testing machine must operate in a loading-controlled mode during compressive strength tests and in a displacement-controlled mode during CMOD tests.
For measuring the crack opening during CMOD tests, the high precision displacement transducer "Controls Group P0331/E" (Controls S.P.A., Milan, Italy) was used. This displacement transducer has a measuring capacity of 5 mm and sensitivity of 10 −3 strain/mm.
The CMOD tests requires the fatigue pre-cracking stage. During this stage, the flexural loading is applied to the specimen at a constant rate of 0.02 mm/s until the Crack Opening Displacement (COD) reached 0.3 mm, after which specimens were subjected to approximately one million cycles of loading. The loading was applied between 10% and 90% of the elastic limit. Frequency was 5 Hz. After the fatigue pre-cracking stage, the specimen was fractured with a constant 0.02 mm/s rate.
Details showing a specimen, supporting and loading system as well as displacement transducer are illustrated in Figure 1.
90% of the elastic limit. Frequency was 5 Hz. After the fatigue pre-cracking stage, the specimen was fractured with a constant 0.02 mm/s rate.
Details showing a specimen, supporting and loading system as well as displacement transducer are illustrated in Figure 1.

Results
The following mechanical properties of non-reinforced concrete were obtained: Young's modulus 30 GPa; compressive strength 25.7 MPa; tension strength 3.8 MPa.
The behavior of concrete under bending is presented in Figure 2. The following mechanical properties of fiber-reinforced concrete were obtained: Young's modulus 30 GPa; compressive strength 28.7 MPa; tension strength 4.2 MPa at a

Results
The following mechanical properties of non-reinforced concrete were obtained: Young's modulus 30 GPa; compressive strength 25.7 MPa; tension strength 3.8 MPa.
The behavior of concrete under bending is presented in Figure 2.
90% of the elastic limit. Frequency was 5 Hz. After the fatigue pre-cracking stage, the specimen was fractured with a constant 0.02 mm/s rate.
Details showing a specimen, supporting and loading system as well as displacement transducer are illustrated in Figure 1.

Results
The following mechanical properties of non-reinforced concrete were obtained: Young's modulus 30 GPa; compressive strength 25.7 MPa; tension strength 3.8 MPa.
The behavior of concrete under bending is presented in Figure 2.  The behavior of fiber-reinforced concrete under bending is presented in Figure 3. fiber amount of 3 kg/m 3 , 4.6 MPa at the fiber amount of 5 kg/m 3 and 5.0 MPa at the fiber amount of 7 kg/m 3 . The behavior of fiber-reinforced concrete under bending is presented in Figure 3.

General Information about the Model of Plastic Behavior of Concrete with Damage Accumulation (Concrete Damage Plasticity Model)
The concrete damage plasticity model is designed to describe the mechanical behavior of concrete under uniaxial, biaxial and volumetric stress conditions with insignificant values of lateral compression [20][21][22]. The mechanical behavior of concrete in the model is based on isotropic elastic damage in combination with isotropic plastic behavior for compression and tension that allows describing irreversible deformations in concrete. This approach is suitable because it is assumed that macrofibers in concrete has a chaotic orientation, and due to its sufficiently large content, it is possible for the models to assume the same hardening of concrete in all possible directions. Two main mechanisms of concrete destruction, namely, the formation of separation cracks and plastic destruction under compression, are considered in the model. This approach allows using the model under simple or cyclic static loads or dynamic loads. The model takes into account concrete reinforcement with individual rods, meshes or dispersed reinforcement. The dispersed reinforcement of concrete in the model is set in terms of the amount of energy required for the formation and full opening of a crack.
Parameters used to set the properties of the concrete damage plasticity model with accumulated damages:  The concrete damage plasticity model is designed to describe the mechanical behavior of concrete under uniaxial, biaxial and volumetric stress conditions with insignificant values of lateral compression [20][21][22]. The mechanical behavior of concrete in the model is based on isotropic elastic damage in combination with isotropic plastic behavior for compression and tension that allows describing irreversible deformations in concrete. This approach is suitable because it is assumed that macrofibers in concrete has a chaotic orientation, and due to its sufficiently large content, it is possible for the models to assume the same hardening of concrete in all possible directions. Two main mechanisms of concrete destruction, namely, the formation of separation cracks and plastic destruction under compression, are considered in the model. This approach allows using the model under simple or cyclic static loads or dynamic loads. The model takes into account concrete reinforcement with individual rods, meshes or dispersed reinforcement. The dispersed reinforcement of concrete in the model is set in terms of the amount of energy required for the formation and full opening of a crack.
Parameters used to set the properties of the concrete damage plasticity model with accumulated damages: Ultimate uniaxial tension strength f ctm ; • Diagram of concrete deformations in the axes "force versus CMOD" from bending test (see Figures 2 and 3); • Dilation angle ψ measured in the p-q plane at high confining pressure. The value should be between 0 and 30 degrees; • The ratio of initial equibiaxial compressive yield stress to initial uniaxial compressive yield stress α f . Recommended default value: 1.16 [23]; • Flow potential eccentricity Ie. The eccentricity is a small positive number that defines the rate at which the hyperbolic flow potential approaches its asymptote. Recommended default value: 0.1 [23]; • The ratio of the second stress invariant on the tensile meridian to that on the compressive meridian coefficient of the shape of plastic surface flow K c . Recommended default value: 0.667 [23].
The values of these parameters were determined based on tests (see Section 3), requirements of regulatory documents, numerical modeling [24][25][26][27] as well as recommendations set out in the scientific and technical documents [28][29][30][31][32]. The parameters of the model of plastic behavior of concrete with damage accumulation are summarized in Table 2. Damage is usually characterized by the degradation of stiffness. An isotropic scaled damage model from the continuum damage mechanics is introduced in Abaqus to describe the stiffness degradation, which can be represented by Equation (1) under uniaxial loading [23]: where σ represents the stress, ε and ε pl represent, respectively, the total and plastic deformation, E represents the initial (undamaged) Young's modulus and d represents the damage factor, which characterizes the degradation of the elastic stiffness and has values in the range between 0 (undamaged) and 1 (fully damaged). The diagrams in the axes "tensile damage parameter versus CMOD" based on experimental data of CMOD tests are shown in Figure 4. These diagrams are directly used by the concrete damaged plasticity model as additional parameters to correctly simulate the accumulation of damage in concrete.

Determination of Concrete Stress-Strain Diagram under Uniaxial Tension Simulation
The approach of constructing the diagram of the extreme deformation of concrete under uniaxial tension is used based on the results of concrete test under bending. It consists of selecting the parameters of the model of plastic behavior of concrete based on the results of a numerical experiment.
The sequence of selection of damaged concrete plasticity model parameters is shown in Figure 5 as flow chart.

Determination of Concrete Stress-Strain Diagram under Uniaxial Tension Simulation
The approach of constructing the diagram of the extreme deformation of concrete under uniaxial tension is used based on the results of concrete test under bending. It consists of selecting the parameters of the model of plastic behavior of concrete based on the results of a numerical experiment. The sequence of selection of damaged concrete plasticity model parameters is shown in Figure 5 as flow chart.

Determination of Concrete Stress-Strain Diagram under Uniaxial Tension Simulation
The approach of constructing the diagram of the extreme deformation of concrete under uniaxial tension is used based on the results of concrete test under bending. It consists of selecting the parameters of the model of plastic behavior of concrete based on the results of a numerical experiment.
The sequence of selection of damaged concrete plasticity model parameters is shown in Figure 5 as flow chart.  The selection of the model parameters sequence includes: 1.
Approximate the parameters of the model of plastic behavior of concrete with fracture, which are determined taking into account the data published in scientific papers [23] and experimental data in representation of stress-strain and stress-displacements diagrams of a specific specimen of concrete or fiber-reinforced concrete.

2.
Create the finite-elements model of concrete beams using three-point bending to build the virtual experiment.

3.
If the results of the virtual experiment differ up to 10% (the peak value of the load at which the crack originates must differ up to 5%) from the experimental laboratory data, then proceed to Step 4. If the condition is not met, the model parameters are corrected and Step 3 of the virtual experiment is repeated.

4.
Create the finite-elements model of the concrete specimen under uniaxial tension to build the virtual experiment.

5.
Process the obtained data of numerical modeling at Step 4 and present them using the axes "axial stress" and "tensile rupture crack opening."

Numerical Model of CMOD Tests
The numerical model of concrete under bending (see Figure 6) consists of three separate parts (a concrete beam, two supporting bars and a loading bar). Interaction among parts is carried out through special contact conditions-"hard" contact with friction penalty. A concrete beam is modeled by solid deformable finite elements and it consisted of about 1600 hexagon finite elements of second geometric order. The supporting and loading bars are modeled by finite elements describing an absolutely rigid body. separate parts (a concrete beam, two supporting bars and a loading bar). Interaction among parts is carried out through special contact conditions-"hard" contact with friction penalty. A concrete beam is modeled by solid deformable finite elements and it consisted of about 1600 hexagon finite elements of second geometric order. The supporting and loading bars are modeled by finite elements describing an absolutely rigid body. The dimensions of the beam and the distance between the supporting bars are taken according to the scheme in Figure 1.
The following sequence of numerical experiments is adopted: − Stage 1-establishing contact interaction among the tested concrete beam, supporting and loading bars; − Stage 2-transferring the concentrated loading from the bar to the beam. The maximum deflection during the numerical experiment did not exceeded 2 cm. This amount was sufficient to obtain a complete ultimate diagram of the concrete beam deformation.
The diagram in the axes "force" and "CMOD" was constructed based on the test results and compared with the data from laboratory tests under bending (see Figure 7). The dimensions of the beam and the distance between the supporting bars are taken according to the scheme in Figure 1.
The following sequence of numerical experiments is adopted: -Stage 1-establishing contact interaction among the tested concrete beam, supporting and loading bars; -Stage 2-transferring the concentrated loading from the bar to the beam. The maximum deflection during the numerical experiment did not exceeded 2 cm. This amount was sufficient to obtain a complete ultimate diagram of the concrete beam deformation.
The diagram in the axes "force" and "CMOD" was constructed based on the test results and compared with the data from laboratory tests under bending (see Figure 7).

Numerical Model for the Simulation of Concrete under Uniaxial Tension
The numerical model for testing concrete under uniaxial tension is shown in Figure 8. The following dimensions of the specimen were used during the simulation: 15 × 15 × 55 cm with a weakening area of 10 × 10 × 6 cm at the center. Attenuation in conditions of homogenous uniaxial tension is necessary to localize plastic deformations in a certain area to track the width of the crack opening as well as to specify the area of plastic deformations and accumulation of damage in concrete in an obvious form. In real tests, conventional prism specimens with a cross-sectional area of 10 × 10 mm were used.

Numerical Model for the Simulation of Concrete under Uniaxial Tension
The numerical model for testing concrete under uniaxial tension is shown in Figure 8. The following dimensions of the specimen were used during the simulation: 15 × 15 × 55 cm with a weakening area of 10 × 10 × 6 cm at the center. Attenuation in conditions of homogenous uniaxial tension is necessary to localize plastic deformations in a certain area to track the width of the crack opening as well as to specify the area of plastic deformations and accumulation of damage in concrete in an obvious form. In real tests, conventional prism specimens with a cross-sectional area of 10 × 10 mm were used. Figure 8. The following dimensions of the specimen were used during the simulation: 15 × 15 × 55 cm with a weakening area of 10 × 10 × 6 cm at the center. Attenuation in conditions of homogenous uniaxial tension is necessary to localize plastic deformations in a certain area to track the width of the crack opening as well as to specify the area of plastic deformations and accumulation of damage in concrete in an obvious form. In real tests, conventional prism specimens with a cross-sectional area of 10 × 10 mm were used. A concrete specimen is modeled by solid deformable finite elements, which consists of about 9850 hexagon finite elements of a second geometric order. Numerical simulation was performed at the following boundary conditions: displacements at the bottom are prohibited in all directions; displacements of the top of the model are prohibited in the horizontal plane; positive forced displacement applied in the vertical direction, which simulate the process of uniaxial tension of concrete specimen. The displacement value was no more than 5 mm, which is sufficient to simulate uniaxial tensile testing of all the materials under consideration (non-reinforced concrete of B15 strength class, non-reinforced concrete of B25 strength class, fiber-reinforced concrete of B25 strength class with a fiber amount of 3, 5 and 7 kg/m 3 ).
A typical pattern of specimen deformation in a numerical experiment is shown in Figure 9. A concrete specimen is modeled by solid deformable finite elements, which consists of about 9850 hexagon finite elements of a second geometric order. Numerical simulation was performed at the following boundary conditions: displacements at the bottom are prohibited in all directions; displacements of the top of the model are prohibited in the horizontal plane; positive forced displacement applied in the vertical direction, which simulate the process of uniaxial tension of concrete specimen. The displacement value was no more than 5 mm, which is sufficient to simulate uniaxial tensile testing of all the materials under consideration (non-reinforced concrete of B15 strength class, nonreinforced concrete of B25 strength class, fiber-reinforced concrete of B25 strength class with a fiber amount of 3, 5 and 7 kg/m 3 ).
A typical pattern of specimen deformation in a numerical experiment is shown in Figure 9. Based on the test results the diagrams were performed in the axes "axial stress" and "tensile rupture crack opening." These diagrams are shown in Figure 10. They are used as a basis for obtaining the diagrams shown in Figure 4. Based on the test results the diagrams were performed in the axes "axial stress" and "tensile rupture crack opening." These diagrams are shown in Figure 10. They are used as a basis for obtaining the diagrams shown in Figure 4. Based on the test results the diagrams were performed in the axes "axial stress" and "tensile rupture crack opening." These diagrams are shown in Figure 10. They are used as a basis for obtaining the diagrams shown in Figure 4.

Numerical Simulation of Interaction of Tunnel Lining with Rock Mass under Seismic Loading
The numerical simulation was performed in the framework of setting a plane strain in the Simulia Abaqus software package. The general design scheme included in the model is shown in Figure 11.

Numerical Simulation of Interaction of Tunnel Lining with Rock Mass under Seismic Loading
The numerical simulation was performed in the framework of setting a plane strain in the Simulia Abaqus software package. The general design scheme included in the model is shown in Figure 11. Calculations on the numerical model were implemented in two stages. Simulation of geostatic loading formation in the tunnel lining from the self-weight of the host rock mass was performed in Stage-1. In Stage-2, the simulation of a seismic impact propagating as a wave disturbance through the calculated area of the rock mass was performed.
The model of a linearly deformable body with the parameters presented in Table 3 was used as a mechanical model of a rock mass. Modeling of the behavior of concrete and fiber-reinforced concrete of the tunnel lining was performed using the Damaged Concrete Plasticity model. Model parameters were determined based on laboratory tests data and they are summarized in Table 2. Table 3. Physical and mechanical properties of rocks [15]. Calculations on the numerical model were implemented in two stages. Simulation of geostatic loading formation in the tunnel lining from the self-weight of the host rock mass was performed in Stage-1. In Stage-2, the simulation of a seismic impact propagating as a wave disturbance through the calculated area of the rock mass was performed.
The model of a linearly deformable body with the parameters presented in Table 3 was used as a mechanical model of a rock mass. Modeling of the behavior of concrete and fiber-reinforced concrete of the tunnel lining was performed using the Damaged Concrete Plasticity model. Model parameters were determined based on laboratory tests data and they are summarized in Table 2. The boundary conditions on the finite element model were formulated in a specific way to correctly model the seismic impact. The boundary area of the model was divided by a single layer of infinite elements, the main task of which was to extinguish the seismic wave passing through the model boundary. Thus, the effect of wave reflection from the boundary and subsequent related phenomena, such as the possible interference of direct and reflected seismic waves, were excluded.
The parameters of the natural stress state of the host rock mass were determined, taking into account the estimated tunnel depth of 120 m.
The seismic impact was modeled by applying forced accelerations on the inner face of the model, set component-by-component for the directions of the axes of the coordinate system. The accelerogram of a real earthquake that occurred in Friuli in 1976 shows a magnitude of about 6.5. The component-by-component decomposition of this accelerogram is shown in Figure 12. The main task of modeling was to state the dependencies of the damage formation in the concrete lining during its dynamic loading under the calculated seismic impact a well as to identify the influence of fiber amount in concrete on its resistance to the ac cumulation of these damages. To solve this problem, all calculations were performed under the same conditions for the variants when the tunnel lining is made o non-reinforced concrete and of fiber-reinforced concrete with the fiber amount of 3, 5 and 7 kg/m 3 .
The calculated zones of material damage of the tunnel lining under seismic impact a different time intervals are shown in Figure 13, provided that the tunnel lining is made o non-reinforced monolithic concrete or from fiber-reinforced concrete with a polypro pylene macrofiber amount of 3, 5 and 7 kg/m 3 . The quantitative damage indicator show how much of the initial strength and stiffness is lost by concrete in the current time in terval due to the crack development. The main task of modeling was to state the dependencies of the damage formation in the concrete lining during its dynamic loading under the calculated seismic impact as well as to identify the influence of fiber amount in concrete on its resistance to the accumulation of these damages. To solve this problem, all calculations were performed under the same conditions for the variants when the tunnel lining is made of non-reinforced concrete and of fiber-reinforced concrete with the fiber amount of 3, 5 and 7 kg/m 3 .
The calculated zones of material damage of the tunnel lining under seismic impact at different time intervals are shown in Figure 13, provided that the tunnel lining is made of non-reinforced monolithic concrete or from fiber-reinforced concrete with a polypropylene macrofiber amount of 3, 5 and 7 kg/m 3   Seismic impact from an earthquake causes the formation of breakaway cracks in the lining of non-reinforced monolithic concrete due to the appearance of significant tensile stresses in certain parts of the lining at particular time intervals.
The location and numbering of the characteristic points of the tunnel lining are shown in Figure 12. The curves of changes of the highest and lowest principal stresses at the characteristic points of the tunnel lining made of non-reinforced monolithic concrete are shown in Figure 14.
Appl. Sci. 2021, 11, x FOR PEER REVIEW 13 of 16 Seismic impact from an earthquake causes the formation of breakaway cracks in the lining of non-reinforced monolithic concrete due to the appearance of significant tensile stresses in certain parts of the lining at particular time intervals.
The location and numbering of the characteristic points of the tunnel lining are shown in Figure 12. The curves of changes of the highest and lowest principal stresses at the characteristic points of the tunnel lining made of non-reinforced monolithic concrete are shown in Figure 14. The analysis of changes of the stress state of the tunnel lining at characteristic points over time allows confirming the assumption about the formation of tensile stress in zones of damage appearing before damage accumulation. The compressive stress is not high enough to cause the material damage.
The curves' damage accumulation at the characteristic points of the tunnel lining over time are shown in Figure 15. The analysis of changes of the stress state of the tunnel lining at characteristic points over time allows confirming the assumption about the formation of tensile stress in zones of damage appearing before damage accumulation. The compressive stress is not high enough to cause the material damage.
The curves' damage accumulation at the characteristic points of the tunnel lining over time are shown in Figure 15. The localization of damage zones and the sequence of their formation over time were stated as a result of modeling. First of all, the zones of greatest damage with length about 3.5 m are formed in the lining along the tunnel contour. The zones are located symmetrically relative to the tunnel axis at the angle about 45° counter clockwise to the vertical. Second, the formation of damage zones with a length of about 2.5 m occurs along the tunnel contour. The zones are located symmetrically relative to the tunnel axis at the angle about 50° clockwise to the vertical. Thus, the lining of non-reinforced monolithic concrete as a result of the calculated seismic impact from an earthquake is not destroyed, but the accumulation of structural defects occurs in the form of separation cracks, which locally weaken the rigidity and load-bearing capacity of the lining by 8-30% relative to the initial indicators. Most likely, repair work to eliminate the separation cracks formed in the material [33][34][35][36][37] would be required in the tunnel lining in such conditions in practice.
Calculations of tunnel lining made of fiber-reinforced concrete with polymer macrofiber amount of 7 kg/m 3 show that the presence of a sufficient amount of fiber in the concrete composition allows avoiding damage in the tunnel lining under dynamic loading. The fiber amount of less than 7 kg/m 3 , namely 3 and 5 kg/m 3 , reduces the level of damage to the lining structure after seismic impact. This can be explained by the fact that the presence of fiber increases the total amount of energy that must be spent on concrete destruction in comparison with non-reinforced concrete of the same class of compressive strength. This can significantly increase the seismic resistance of the tunnel lining. In practice, repair work in the tunnel after a seismic impact not exceeding the calculated magnitude would not be required if the lining made of fiber-reinforced concrete with the fiber amount of 7 kg/m 3 was used, since separation cracks in the structure of the lining material are not formed.

Conclusions
The results of the laboratory tests of the specimen made of concrete and fiber-reinforced concrete justifies the parameters of the model of plastic behavior of concrete with damages accumulation. In this paper, the method of substantiating the parameters of mechanical models of materials based on performing virtual tests of specimens is shown and applied.
Calculations in the framework of a numerical model of the seismic impact on a tunnel lining made of concrete or fiber-reinforced concrete allowed describing the The localization of damage zones and the sequence of their formation over time were stated as a result of modeling. First of all, the zones of greatest damage with length about 3.5 m are formed in the lining along the tunnel contour. The zones are located symmetrically relative to the tunnel axis at the angle about 45 • counter clockwise to the vertical. Second, the formation of damage zones with a length of about 2.5 m occurs along the tunnel contour. The zones are located symmetrically relative to the tunnel axis at the angle about 50 • clockwise to the vertical. Thus, the lining of non-reinforced monolithic concrete as a result of the calculated seismic impact from an earthquake is not destroyed, but the accumulation of structural defects occurs in the form of separation cracks, which locally weaken the rigidity and load-bearing capacity of the lining by 8-30% relative to the initial indicators. Most likely, repair work to eliminate the separation cracks formed in the material [33][34][35][36][37] would be required in the tunnel lining in such conditions in practice.
Calculations of tunnel lining made of fiber-reinforced concrete with polymer macrofiber amount of 7 kg/m 3 show that the presence of a sufficient amount of fiber in the concrete composition allows avoiding damage in the tunnel lining under dynamic loading. The fiber amount of less than 7 kg/m 3 , namely 3 and 5 kg/m 3 , reduces the level of damage to the lining structure after seismic impact. This can be explained by the fact that the presence of fiber increases the total amount of energy that must be spent on concrete destruction in comparison with non-reinforced concrete of the same class of compressive strength. This can significantly increase the seismic resistance of the tunnel lining. In practice, repair work in the tunnel after a seismic impact not exceeding the calculated magnitude would not be required if the lining made of fiber-reinforced concrete with the fiber amount of 7 kg/m 3 was used, since separation cracks in the structure of the lining material are not formed.

Conclusions
The results of the laboratory tests of the specimen made of concrete and fiber-reinforced concrete justifies the parameters of the model of plastic behavior of concrete with damages accumulation. In this paper, the method of substantiating the parameters of mechanical models of materials based on performing virtual tests of specimens is shown and applied.
Calculations in the framework of a numerical model of the seismic impact on a tunnel lining made of concrete or fiber-reinforced concrete allowed describing the mechanism of damage formation in the form of separation cracks as well as confirming the effectiveness of using fiber-reinforced concrete in structures operating under dynamic loading.
Calculations of tunnel lining made of fiber-reinforced concrete with the polymer macrofiber amount of 7 kg/m 3 show that the presence of the sufficient amount of fiber in concrete composition makes it possible to completely avoid damage in the tunnel lining under dynamic loading. A fiber amount of less than 7 kg/m 3 , namely 3 and 5 kg/m 3 , reduces the damage level of lining structure after seismic impact.
In our view, the subsequent development of future research lies in multivariate modeling of the work of building structures in a spatial setting under dynamic loads to identify general patterns for determining the optimal amount of polymer fiber in concrete.