Investigation of Sandwich Panel Under High Temperature Loading Using Finite Element Analysis

Corresponding Author: Sajjad Sayyar Roudsari Department of Computational Science and Engineering, North Carolina A and T State University, Greensboro, NC 27411, USA Email: ssayyarroudsari@aggies.ncat.edu Abstract: Structural and nonstructural members are always encountered with extreme loading conditions. In case of nonstructural members, the failure happens much sooner due to lack of load capacity. The nonstructural elements are not designed for structural loading conditions. However, they might be impacted to other loading types such as fire. In recent years, the use of 3D panel is one of the most common partitions in the world. In this research, the effect of fire on 3D panel partitions is presented. To achieve this goal, ABAQUS finite element software is employed to simulate the 3D panel. The 3D panel is embedded inside steel frame. In order to have an accurate result, two validations are performed including steel frame and the steel frame with 3D panel. In the study, 5 different fire loadings 200, 400, 600, 800 and 1000°C are applied into the model. Results include loaddisplacement diagram and stiffness and ductility factors. The results indicated that as fire load increases, the stiffness and ductility factor are reduced.


Introduction
Structures are often subjected to extreme loading conditions such as seismic earthquake and may have defects or high rate temperature, flooding, etc., (Sayyar Roudsari et al., 2019a;2019b;2019c;Sohi et al., 2020). These structures may have internal and/or external partitions which play a vital role in structural design. The partitions can be designed to have the loading capacity such as masonry wall or it can be used as light weight nonstructural member such as 3D panel. In contrast to structural members, 3D panel usually designed without adequate loading capacity under extreme conditions. The 3D panel is not a structural member but it may help to reduce the weight of structure leading to less shear force (He and Hu, 2008;Long, 1977). Schaeffer (1993;Schubel, 2005) have studied sandwich panel loaded under low velocity impact loading condition. They use woven carbon sheets and PVC foam to construct the panel. The tests were performed as quasi-static with low rate impact and static loading conditions. They investigated the load-strain response for both conditions and the results showed that using quasi-static method is more accurate in predicting the damage and response of sandwich panel. Hamid and Fudzee (2013) investigated the performance of a sandwich panel subjected to seismic loading condition. They casted Insulated Sandwich Wall Panel (ISWP) with two boards and one core. The board was cement fiber while the core of the wall was made from polyurethane material. The quasi-static load was applied laterally and strength-drift data were recorded. Their results indicated that the cracks start propagating at the foundation and the aluminum channel frame was buckled. Poluraju and Appa Rao (2018) conducted experimental tests on squat 3D sandwich walls under both vertical and lateral loading conditions. Four walls were constructed. Samples were 11251250 mm in dimension. The weld meshing reinforcements were considered in two walls and additional reinforcement was applied for two other specimens. The design criteria were validated with Europe-8 and ACI-318 codes. Their results showed that using additional reinforcement can remarkably enhance the ultimate stiffness and strength. Crewe et al. (2018) conducted experimental tests on four sandwich panel walls which were made according to ISO 13784-1. The wall thickness was 100 mm with the dimension of 2.43.62.4 as width, length and height, in order. The fire load was applied to the wall and increased with the time. In other word, the fire was applied to reach 100 kW within 10 min. Then, it was increased to 300 kW in the next 10 min. The modification factor and validation were also performed in their study. The results showed that the use of combustible insulation does not protect the wall very well. In some cases, it causes growing fire and expose in the large area. Many researchers have discussed the effect of material properties on sandwich panel, as well as the performance of the partitions such as 3D panel under seismic conditions (De Matteis and Landolfo, 2000;Krzyżak et al., 2016;Ravi, 2017). However, there are few studies regarding the sandwich panel under fire or high temperature condition. These researches were mainly focused on the effect of fire on the panel in terms of energy, the temperature growth and damage of the panel (Bonner et al., 2020;Cooke, 2004;Roudsari and Abu-Lebdeh, 2019;Smolka et al., 2013;Wang and Foster, 2017).
In this study, the sandwich panels are evaluated under five different high temperature loading conditions. ABAQUS software is employed to simulate temperature loading. The panel contains two concrete walls embedded with reinforcement and a foam. The loaddisplacement diagrams are carried out and analytical investigation including stiffness, ductility is discussed.

Finite Element Model
In this research, ABAQUS software is employed to model and analyze the sandwich panel. In the process, the validation is essential to perform the simulation. In order to validate the initial model, the sandwich panel is modeled using the sandwich panel proposed by Kabir et al. (2006). The wall has a dimension of 1200640140 mm as height, width and thickness, respectively. The wall was framed with two number of IPE120 as columns at each side and one IPE120 beam. The stiffeners are also used at the beam-columns joints. The mesh reinforcements were considered with 3.5 wires in each concrete wall. It should be noted that the panel is constructed with 40 mm thick foam sandwiched by concrete plates at each side of the wall. Figure 1, shows the schematic view of the sandwich panel. In Fig. 2, the geometry of sandwich panel is shown.
The ABAQUS software is used to simulate the validation model. Two different validations were performed. The first one was without inside wall while the second model included the wall. The concrete and foam were modeled with solid element (C3D8R). The beam and columns were created with shell element (S4R) and reinforcement was modeled by beam element (B31) (Fallahi et al., 2018). Additionally, the concrete compressive strength of 34.5 MPa was used. The Concrete Damage Plasticity model (CDP) is used to define concrete behavior Sayyar Roudsari et al., 2018;Soleimani and Sayyar Roudsari, 2015;. The Hyper-Foam criteria is exploited to define the foam behavior. Therefore, µ1, α1 and ν1 are 0.5, 2 and 0.33, respectively. The plasticity criteria are assigned for steel beam, columns and stiffeners. The yield and ultimate stress of steel were reported as 240 and 370 MPa, in order. Moreover, the yield and ultimate stress of the reinforcement wires were 4000 and 5200 MPa, respectively. Figure 3 displays the modeling of sandwich panel. The interaction between wall and frame are considered to be "Tie" and wires are connected to the concrete with "Embedded Region". The sandwich panel was subjected to Non-Linear Static General analysis. The lateral load is assigned as "Displacement-Control" and the bottom surface are totally fixed (Us and URs are equal zero). After the analysis and obtaining the results, the two validations are compared. In Fig. 4 and 5, the validation of model without Sandwich Panel (S-0-WS) and model with sandwich panel (S-0-NS) are shown. In Fig. 4 However, the temperature criteria need to be defined in model development. The conductivity and specific heat of foam are 0.028 and 1300, in order. The concrete conductivity is 0.0005 at 0°C and 0.00114 at each specific temperature. Also, the specific heat of concrete is assigned to be 1000. The steel material has the specific heat of 5225 and the conductivity of 0.04 at 0°C and 0.0518 each specific temperature. The ASTM E119 (ASTM, 1990) standard is employed for applying the high temperature loading. The Coupled-Temp-Displacement (Transient) analysis is selected. The temperature room is considered 25°C and surface coefficient is 0.01. The allowable temperature applies to be at most 10°C. Figure 6, shows the time-amplitude factor for finite element simulation. The vertical numbers are a factor of 1000 such as that 0.6 indicates 600°C. Figure 7, displays the interaction (left side) and boundary condition (right side) of high temperature analysis.

Results and Discussion
In this section, the load-displacement diagrams for specimens subjected to high temperature are shown in shows that increasing the temperature to 200°C (S-200) causes 5.50% reduction in load capacity. Similarly, the reduction in load capacity was 12.00% for (S-400), 18.00% for (S-600), 44.00% for (S-800) and 60% for (S-1000). Furthermore, the reduction in the displacement at failure was 0.7, 4.00, 5.50, 7.20 and 15.30% for S-200, S-400, S-600, S-800 and S-1000, respectively. In order to evaluate the effect of temperature on the sandwich panel wall, the parametrical study is essential. In this sutdy, the parametrical investigation is focused on stiffness and ductility factors. Equations 1 and 2 show the stiffness and ductility factor. In these equations, Vy, ∆y and ∆max are force at yield point, displacement at yield point and displacement at failure, in order. E and µ are stiffness and ductility, respectively. Figure 9, shows the bilinear graph for the stiffness and ductility. These two factors are computed for all specimens and displayed in Fig. 10 and 11: (ACI-Committee-201-1R-92, 1997). In Fig. 10, the stiffness of S-0WS (model with sandwich panel without fire load) compared to S-0-NS (model without neither sandwich panel nor fire) enhanced about 782%. It means that having the sandwich panel improved the stiffness from 3.53 kN/mm for S-0-NS to 27.6 kN/mm for S-0-WS. Also, the trend of stiffness reduction indicates that increasing the fire temperature reduces the stiffness of system. Comparing S-200 with S-0-WS demonstrates that 200 fire temperature causes 13.5% reduction of stiffness. Contrasting of S-1000 with S-0-WS model shows 67% reduction of stiffness. However, the comparison of S-1000 with S-0-NS declares that the stifnes of sandwich panel under 1000 Celsuis Degree has better performance than the model without sandwich panel (S-0-NS). Moreover, in Fig. 11, the ductility results show that the S-0-NS has only 3.88. Comparison of S-0-WS with S-200, S-400, S-600, S-800 and S-1000 indicates that the ductility reduction is about 5.8, 20.7, 24.5, 32 and 44%. Comparisn the ductility of S-0-NS with S-1000 shows that having sandwich panel improved the ductility factor about 2%.

Conclusion
Based on modeling and simulation of this research, the following results are concluded:  ABAQUS software can precisely predict the 3D panel behavior under fire loading conditions  Adding 3D panel can enhance the load capacity compared with frame without 3D panel  Increasing the fire load reduces the stiffness and ductility of 3D panel  The load capacity and maximum displacement of 3D panel are also decreased by increasing the fire loading