**4. Development of the finite element model for fuse-equipped infill wall**

In the finite element model, material nonlinearities were considered because of nonlinear moment-rotation and force-deformation responses of steel frame connections, equivalent infill wall struts, tie-down anchors, and the fuse element. Large deformation and geometrical nonlinearities existed due to movements and contact between infill wall and frame. In this study, ANSYS finite element analysis program [55] was employed. Five different finite element types from ANSYS element library were used for modeling. The uniaxial BEAM3 element with compression, tension, and bending modeling capabilities was used to model the frame members. PLAIN42 element was used to model the masonry infill wall. CONTACT12 element was employed to model the interaction between infill and frame, and COMBIN39 spring element was considered to model the diagonal strut representing the masonry infill and rotational spring representing beam-column joint. Finally, COMBIN40 element was used to model the proposed structural fuse component.

To model a bare steel frame, BEAM3 element with three degrees of freedom (two translations and one rotation) at each node was used. PLAIN42 element with four nodes and two translational degrees of freedom per node was used as a plane stress element to model the infill wall. COMBIN39 element with two nodes and with up to three translational degrees of freedom per node can be used as a unidirectional element (e.g., uniaxial compression-tension element or purely rotational spring). The longitudinal option with two degrees of freedom per node was used to model the diagonal struts to represent effective infill and also tie-down rebars. The rotational option was used to represent the frame's beam-column connection. CONTACT12 element with two nodes and two translational degrees of freedom at each node was considered to model a gap between two surfaces, which can be in compression contact or at no contact and may also slide relative to each other considering Coulomb friction. This element was used to model the interaction between infill wall and frame when equipped with fuse. When there is interaction between the two surfaces, the normal stiffness and tangential (shear) stiffness may be active. A negative normal force represents contact between the two surfaces through a linear spring, while a positive normal force means lack of contact. On the other hand, when there is a negative force and the tangential force is less than the product of the normal force and friction coefficient, the two surfaces do not slide freely and are governed by the tangential spring stiffness. However, the two surfaces slide when the tangential force equals that product. COMBIN40 element is a special element to provide stiffness and damping to one side of a gap modeled in series. This two-node element with one degree of freedom per node (e.g., translational or rotational) can be

sizes can be used. Furthermore, the out-of-plane movement of the infill wall can be restricted

**Figure 8.** Test results on one-fourth scale frame and infill wall with wood disk fuses: (a) one-fourth scale experimental

The process of pilot study leading to the test specimen shown in **Figure 8** consisted of initially developing load-deformation relations for isolated disk element to obtain the average capacities. Then isolated masonry walls were tested under in-plane shear loading to determine their capacities. Finally, the fuse disks were chosen such that they will break prior to masonry infill shear capacity. The detail of the experimental study is explained in Ref. [53]. In this chapter, only the computer-modeling aspect of masonry infill walls equipped with rigid-brittle structural fuse elements is presented. The objective of this chapter is to discuss development of a finite element model for the system (infill-fuse-frame) and validate it by using the results of tests on masonry infill walls (without fuse) available in the literature. In the process of developing the

using different available mechanisms as appropriate to a given design.

setup; (b) steel rod tightened against wood fuse; and (c) steel rod puncturing wood fuse [53].

34 New Trends in Structural Engineering

specialized for different applications by appropriate assignment of values for spring stiffness coefficients, damping coefficient, mass value, gap size, and a limiting sliding force.

used for the beam-column joints. The load–displacement diagram for the model when subjected to monotonically increasing displacement was quite close to the experimental results. The bare frame showed to have an initial stiffness of about 3.22 kN/m. The failure mechanism consisted of formation of four plastic hinges in the four beam-column connections, which are

Finite Element Modeling of Masonry Infill Walls Equipped with Structural Fuse

http://dx.doi.org/10.5772/intechopen.77307

37

The infill wall was modeled initially using the single-diagonal strut model [56] shown in **Figure 10(b)**. This was accomplished by adding a nonlinear diagonal compression strut to the bare frame model. However, the nonlinear rotational springs at the beam-column joint were substituted by frictionless hinges, in order for the diagonal strut to take the entire lateral load. The force-deformation model [56] was used for the strut representing the infill wall. The threediagonal compression strut [57] shown in **Figure 10(c)** was also used as a second alternative for infill model. The force-deformation models were developed based on equations in Ref. [57] using the geometry and material properties of the modeled specimen (WD7). The infilled

**Figure 10.** ANSYS models for (a) bare frame; (b) infilled steel frame with single-diagonal strut model; and (c) infilled

steel frame with three-diagonal strut model [53].

represented by rotational springs in the model (**Figure 10(a)**).

From the result of a comprehensive review of experimental and analytical studies on infill wall systems [22], an appropriate specimen was chosen for development of finite element modeling in this work. The approach for finite element model validation consisted of initially modeling the bare steel frame, then adding brace elements following methods in Refs. [56] (single-diagonal strut model) and [57] (three-diagonal strut model). The last step in developing the model was to add fuse elements.

One of the specimens in the tests in Ref. [58] on single-bay, single-story steel frame with CMU infill walls (labeled WD7) was chosen for finite element modeling. The specimens selected are described in detail in Ref. [22]. Lateral load was applied to the frame at the top. Specimen WD7 [58] included CMU infill wall with standard horizontal bed joint reinforcement constructed without any gaps between the infill and the steel frame. Load-deflection diagram for the specimen is shown in **Figure 9** including the bare frame and infilled frame tests. The figure also shows analysis results discussed subsequently.

The bare frame was modeled as shown in **Figure 10(a)** using the finite elements as explained in the previous section. The trilinear moment-rotation relationship proposed in Ref. [57] was

**Figure 9.** Load-deflection relation for single-bay, single-story system [53].

used for the beam-column joints. The load–displacement diagram for the model when subjected to monotonically increasing displacement was quite close to the experimental results. The bare frame showed to have an initial stiffness of about 3.22 kN/m. The failure mechanism consisted of formation of four plastic hinges in the four beam-column connections, which are represented by rotational springs in the model (**Figure 10(a)**).

The infill wall was modeled initially using the single-diagonal strut model [56] shown in **Figure 10(b)**. This was accomplished by adding a nonlinear diagonal compression strut to the bare frame model. However, the nonlinear rotational springs at the beam-column joint were substituted by frictionless hinges, in order for the diagonal strut to take the entire lateral load. The force-deformation model [56] was used for the strut representing the infill wall. The threediagonal compression strut [57] shown in **Figure 10(c)** was also used as a second alternative for infill model. The force-deformation models were developed based on equations in Ref. [57] using the geometry and material properties of the modeled specimen (WD7). The infilled

**Figure 10.** ANSYS models for (a) bare frame; (b) infilled steel frame with single-diagonal strut model; and (c) infilled steel frame with three-diagonal strut model [53].

**Figure 9.** Load-deflection relation for single-bay, single-story system [53].

specialized for different applications by appropriate assignment of values for spring stiffness

From the result of a comprehensive review of experimental and analytical studies on infill wall systems [22], an appropriate specimen was chosen for development of finite element modeling in this work. The approach for finite element model validation consisted of initially modeling the bare steel frame, then adding brace elements following methods in Refs. [56] (single-diagonal strut model) and [57] (three-diagonal strut model). The last step in develop-

One of the specimens in the tests in Ref. [58] on single-bay, single-story steel frame with CMU infill walls (labeled WD7) was chosen for finite element modeling. The specimens selected are described in detail in Ref. [22]. Lateral load was applied to the frame at the top. Specimen WD7 [58] included CMU infill wall with standard horizontal bed joint reinforcement constructed without any gaps between the infill and the steel frame. Load-deflection diagram for the specimen is shown in **Figure 9** including the bare frame and infilled frame tests. The figure

The bare frame was modeled as shown in **Figure 10(a)** using the finite elements as explained in the previous section. The trilinear moment-rotation relationship proposed in Ref. [57] was

coefficients, damping coefficient, mass value, gap size, and a limiting sliding force.

ing the model was to add fuse elements.

36 New Trends in Structural Engineering

also shows analysis results discussed subsequently.

frame models with the two types of strut models were subjected to monotonically increasing displacement with load-deflection plots compared to the experimental test results shown in **Figure 9**. The results of the two strut models show notable differences which is due to the assumptions made for force-deformation properties of the strut element. The three-diagonal strut model shows closer analytical results to the experimental test results.

wall were assumed to be in tight fit connection with the columns to provide shear transfer. The micro infill wall modeling required 396 PLAIN42 elements, 27 CONTACT12 elements,

Finite Element Modeling of Masonry Infill Walls Equipped with Structural Fuse

http://dx.doi.org/10.5772/intechopen.77307

39

The fuse element used in the model is intended to simulate an elastic behavior up to failure or breakage of the element as shown in **Figure 13**. Once the fuse element breaks, there is no force transfer through the fuse element. COMBIN40 element provides the required property, which is transfer of force only in compression. To provide for such behavior, a very small value (0.0025 mm) was assumed for the GAP specification in the element property data. The spring K1 in the COMBIN40 element was determined considering the force-deformation results of the fuse elements pilot tests. COMBIN40 element features "break-away" property appropriate

and 2 COMBIN39 elements.

**Figure 12.** Force-deformation responses for tie-down steel rebar [53].

**Figure 13.** Force-deformation responses for the rigid-brittle fuse element [53].

The next step in completing the finite element model (shown in **Figure 11**) was to add appropriate fuse elements and hold-down elements. At the location of the fuse element on the columns, two nonlinear rotational springs were added. The final steel frame model shown in **Figure 11** had a total of 33 BEAM3 elements and 6 COMBIN39 elements. The masonry infill wall was, then, modeled with PLAIN42 elements. To model the contact between infill wall and steel frame, CONTACT12 elements were added at top and bottom at each side. The model presented also shows vertical steel rebar hold-downs modeled with COMBIN39 elements with tension force-deformation properties shown in **Figure 12**. The bottom corners of the infill

**Figure 11.** ANSYS model for infilled steel frame with fuse elements [53].

wall were assumed to be in tight fit connection with the columns to provide shear transfer. The micro infill wall modeling required 396 PLAIN42 elements, 27 CONTACT12 elements, and 2 COMBIN39 elements.

The fuse element used in the model is intended to simulate an elastic behavior up to failure or breakage of the element as shown in **Figure 13**. Once the fuse element breaks, there is no force transfer through the fuse element. COMBIN40 element provides the required property, which is transfer of force only in compression. To provide for such behavior, a very small value (0.0025 mm) was assumed for the GAP specification in the element property data. The spring K1 in the COMBIN40 element was determined considering the force-deformation results of the fuse elements pilot tests. COMBIN40 element features "break-away" property appropriate

**Figure 12.** Force-deformation responses for tie-down steel rebar [53].

frame models with the two types of strut models were subjected to monotonically increasing displacement with load-deflection plots compared to the experimental test results shown in **Figure 9**. The results of the two strut models show notable differences which is due to the assumptions made for force-deformation properties of the strut element. The three-diagonal

The next step in completing the finite element model (shown in **Figure 11**) was to add appropriate fuse elements and hold-down elements. At the location of the fuse element on the columns, two nonlinear rotational springs were added. The final steel frame model shown in **Figure 11** had a total of 33 BEAM3 elements and 6 COMBIN39 elements. The masonry infill wall was, then, modeled with PLAIN42 elements. To model the contact between infill wall and steel frame, CONTACT12 elements were added at top and bottom at each side. The model presented also shows vertical steel rebar hold-downs modeled with COMBIN39 elements with tension force-deformation properties shown in **Figure 12**. The bottom corners of the infill

strut model shows closer analytical results to the experimental test results.

38 New Trends in Structural Engineering

**Figure 11.** ANSYS model for infilled steel frame with fuse elements [53].

**Figure 13.** Force-deformation responses for the rigid-brittle fuse element [53].

to simulate the condition of fuse breakage with subsequent zero force in the element, once the fuse capacity is reached. The fuse capacity is a function of the masonry infill wall shear strength. According to test results in Ref. [56], the infill wall had a capacity of 383 kN, which with a factor of safety of 4.0, yields a fuse capacity of 89 kN for the model. This value was used to specify FSLIDE, for which a negative value results in a drop to zero when the force in the element reaches the specified capacity (89 kN), while a positive value represents yielding or constant force equal to the capacity. In this case, only negative value was assigned.

and 267 kN). The figure shows two stages of response consisting of (a) prior to breakage of the fuse and (b) after breakage. During the first stage shown by line OA in **Figure 14**, the fuse transfers lateral loads from the frame to the infill wall and as such, the slope of the line OA represents the combined larger stiffness of the steel frame and the masonry infill wall. Upon breakage of the fuse at point A (capacity of fuse), there is sudden drop in the force level, line AB, followed by load-deflection relation along BC, which represents the response of the bare frame. This means that the infill wall is disengaged from the steel frame and only the bare

Finite Element Modeling of Masonry Infill Walls Equipped with Structural Fuse

http://dx.doi.org/10.5772/intechopen.77307

41

Comparison of the response of the model having fuse element with those of the bare frame and infilled frame in **Figure 9** shows that the stiffness of the system with fuse element is slightly smaller than that resulting from tested infilled frame (about 75% of the infilled frame). This, however, is about ten times the stiffness of the bare frame. Although as shown in **Figure 9**, higher strength fuse elements increase the strength capacity of the system, but it should be noted that the objective is to prevent failure of the wall. For example, based on the test results (shown on the figure), the tightly fitted masonry infill wall cracks around a lateral load of 378 kN. The smaller the fuse capacity, the larger will be the margin of safety against cracking.

The fuse element model shown in **Figure 13** describes a condition where upon breakage of the fuse, the force transfer across the fuse becomes zero. Since this could imply a shock-type response, but which is more like cracking of reinforced concrete or masonry system, it is possible to develop fuse elements that show more ductile response. For example, if the fuse element can be described by the trilinear or multilinear models shown in **Figure 15**, the corresponding load deflection plots for the infilled frame will be those shown in **Figures 16** and **17**, which show a more gradual drop of the force across the fuse and a smoother transition to the bare frame condition. It should be noted that depending on the mechanism of failure or design function of the fuse, different types of infilled frame response can be obtained. Examples of such mechanisms could include friction damper mechanism for energy dissipa-

**Figure 15.** Assumed force-deformation responses for fuse element (a) "trilinear" and (b) "multilinear" [53].

frame is resisting the total load.

tion and enhanced seismic response of the structure.
