**1. Introduction**

Concrete is currently the most widely used building material. Although many structures are built with concrete, the use of normal strength concrete (NSC) still has some limitations, such as low tensile strength and low ductility. Improving the mechanical properties of concrete to obtain higher strength and higher ductility has been widely of concern. Ultra-high-performance steel fiber concrete (UHPFRC) is a new type of fiber concrete, with high strength, fracture toughness, and ductility. Its compressive strength and tensile strength are generally over 150 MPa and 7 MPa, respectively [1–5], and even the tensile strength can reach 15 MPa [6]. Ultra-high-performance concrete has been applied and investigated in many kinds of engineering structures, such as concrete structures [7–9], seismic design [10,11], etc. For the material level, numbers of studies have been conducted on the influence of fiber types, fiber orientations, geometric shapes, dosages, and other factors on the mechanical properties of ultra-high-performance concrete [12–19]. Numerous experimental studies have been carried out on high-performance concrete components, which include full-size prestressed beams [20–22], reinforced beams [23–26], columns [27], slabs [28], etc.

Extensive tests are required at the material and structural levels in order to develop standard analytical procedures and design specifications for UHPFRC, which will take a lot of time and cost. Therefore, verifying the concrete material models in the existing finite element software by conducting a limited number of well-formulated tests on the material and structure levels is a way to save time and cost. The verified concrete material model and finite element modeling method can be used to establish extended analysis of various design parameters. In addition, the influences of changes in geometry, load cases, and reinforcement on mechanical properties of UHPFRC can be investigated. The finite element software ABAQUS is equipped with the concrete damage plasticity (CDP) model developed for NSC, which is a mature and reliable tool for predicting the mechanical behavior of NSC [29–31]. Compared with NSC, the material properties of UHPFRC have higher tensile strength and ductility, which makes the shape of a material constitutive curve substantially different from NSC. In order for CDP model to be used to simulate UHPFRC, the parameters of CDP model need to be calibrated. Tysmans et al. [32] used CDP model to simulate the behavior of high-performance fiber concrete composites under biaxial tension. Mahmud et al. [33] and Singh et al. [34] calibrated the CDP model through the UHPFRC material test and used the calibrated model to simulate the test results of the UHPFRC beam [24]. It was reported that the calibrated CDP model can accurately and effectively predict the load-displacement curves and plastic damage distributions of UHPFRC components.

Similar to the investigations of NSC, the investigations of UHPFRC need to be developed to the structural level as well as the material and component level. However, it is very expensive to establish a full-scale structural test, which is seriously restricted by the test conditions. When the calibrated CDP model is used to simulate a single UHPFRC component, the reduction of mesh size and the increase of number of elements will significantly increase the calculation time, while larger mesh size will lead to convergence problems [34]. Therefore, it is difficult to use solid elements to simulate all of the UHPFRC of the whole structure. Fortunately, the multi-scale finite element simulation strategy can solve this problem. The simulation strategy uses solid elements to simulate the key parts of the structure that need to be paid attention to, and adopts the macro-scale elements such as truss or beam elements for the other parts. Its advantage is to use limited computing resources to ensure the requirements for simulation accuracy and to improve computational efficiency. So the simulation strategy has been well applied in structural failure analysis, seismic design, optimization of structural system, etc. [35–39]. The key problem of the multi-scale finite element simulation strategy is to establish an accurate interface-coupling constraint relationship, so as to ensure the scientific and reasonable coordination between different scale elements. The multi-point constraint method is based on the relations of displacement coordination [40] or energy balance [41] between macro-scale and micro-scale elements at the interface, and the constraint equations containing the degrees of freedom of nodes of different scale elements are established at the interface [42,43]. However, a single multi-point constraint relation has the limitation that the stress state and deformation of the connection interface appear distorted after the material enters the plastic stage [44].

In order to promote the development of finite element simulation of UHPFRC structure, a novel multi-scale finite element modeling strategy was proposed in this study. A novel combined multi-point constraint (CMPC) based on displacement coordination and energy balance was established, aiming at the problems of the tangential over-constraint and the requirements for nonlinear stress iteration existing in the single multi-point constraint method. The nonlinear constitutive relationship of UHPFRC is considered. The multi-scale models of UHPFRC components under various load cases were established in the finite element software ABAQUS. The comparative analysis results show that the proposed multi-scale modeling strategy can well predict the strain distribution and damage distribution of UHPFRC components while significantly reducing the number of model elements and improving the computational efficiency. This study provides an accurate and efficient finite element modeling strategy for the design and analysis of UHPFRC structure, which can promote the application and development of UHPFRC in the construction industry.

#### **2. Multi-Scale Modeling Strategy—Material Models**

#### *2.1. Calibrated Concrete Damage Plasticity (CDP) Model*

The concrete damage plasticity (CDP) model is a concrete material model for NSC in the finite element software ABAQUS. It is a mature and reliable tool for predicting the mechanical behavior of NSC [29–31]. In order for CDP model to be used to simulate UHPFRC, the CDP model needs to be calibrated. Some studies have shown that the calibrated CDP model can accurately and effectively predict the mechanics characteristic of UHPFRC. In this study, the stress-strain curve for UHPFRC in compression proposed by Singh et al. [34], modified from Lu et al. [45], is used to calculate the data of compressive behavior in the CDP model. The stress-strain curve of UHPFRC specimen of the uniaxial tension test [34] is used to define the tensile behavior in the CDP model. The curves of compression damage and tension damage in the CDP model are defined according to the studies in [33,46], respectively. The parameters of the CDP model adopted in this study are shown in Table 1.


**Table 1.** Parameters of the concrete damage plasticity (CDP) model of ultra-high-performance fiber-reinforced concrete (UHPFRC).

#### *2.2. Validation of the Model*

#### 2.2.1. Test Specimens

In this study, the UHPFRC beams named as B25-1 and B25-2 [34] are chosen for the validation analysis. The cross section, spans, loading configuration details and reinforcement detail of the all the beams are given in Table 2, where the tensile reinforcement consisted of 20 mm diameter rebar with a yield strength and ultimate strength of 525 and 625 MPa, respectively. The four point bending test applies the same concentrated load symmetrically at a distance of 250 mm from the middle of the beams, resulting in pure bending stresses between the load points.



#### 2.2.2. Finite Element Analysis (FEA) Model

According to the design diagram of UHPFRC beam specimen and the design of loading device, the corresponding finite element model of the test was established in ABAQUS with mesh size of 25 mm. The details of the reinforcement, mesh and load boundary condition of the finite element (FE) model are shown in Figure 1. The parameters of the CDP model adopted for the UHPFRC solid elements are shown in Table 1.

**Figure 1.** FE model of ultra-high-performance fiber-reinforced concrete (UHPFRC) beam test. (**a**) Reinforcement detail; (**b**) Mesh details; (**c**) Load boundary condition.

#### 2.2.3. Results of FEA Simulation and Test

The test results and simulation results of the four point bending test of the two UHPFRC specimens are shown in Figure 2, where (a) is the relation curve between the mid-span displacement of the beam and the external load, (b) is the failure pattern of the specimen B25-1, and (c) is the tension damage distribution of UHPFRC in the finite element model. It can be seen that the finite element model can simulate the whole entire load-displacement curve, including the descending section after yielding. The finite element simulation results are in good agreement with the experimental results. The test results and the finite element results of peak load and corresponding displacement of UHPFRC specimens are shown in Table 3. The ultimate load capacity of specimens B25-1 and B25-2 predicted by the finite element model is 3% and 6% higher than the test results, respectively. It can be seen from Figure 2a,b, the damage distribution simulated by the finite element model is similar to the crack distribution of the specimen. Meanwhile, the validity of the parameters selected of the FEA model in this paper is proved so the FEA model with the same parameters can be taken as the standard for the extended study.


**Table 3.** Comparison of the FE model results with test results.

**Figure 2.** Test results and simulation results of beam test. (**a**) Load-displacement curve; (**b**) failure pattern of the specimen B25-1; (**c**) Tension damage distribution of UHPFRC in the FE model.
