# Study on Bending Performance of Tightly Spliced Truss-Reinforced Plate-Honeycomb Flat Beam
## 3 Test Results and Discussions
### Finite Element Analysis  
#### 3.4.1 Establishment and Validation of the Model  
ABAQUS was used for numerical analysis, in which the models were established based on the dimensions and reinforcement in the experiment. The plastic damage constitutive relationship model is used for concrete materials, and the ideal elastic-plastic model is used for steel. The concrete and steel sections use the C3D8R element, while the steel bars use the T3D2 element. The overall size of the element in the honeycomb beam is 30 mm \(\times\) 30 mm,  
Figure 16: Stress distribution of honeycomb holes in bending and shear sections. (**a**) DTCB1; (**b**) DTCB2; (**c**) DTCB3; (**d**) DTCB5. appropriately densified around the honeycomb hole. The element size of the concrete is 20 mm \(\times\) 60 mm. In addition, the steel bars were meshed in the size of 60 mm. In terms of contact properties, the contact between steel and concrete adopts a coulomb friction contact model, where the normal direction is hard to contact, and the tangential friction coefficient is a penalty function contact of 0.3. The embedded property is used between steel bars and concrete. The boundary conditions for loading are consistent with the experiment. On this basis, numerical analysis was conducted on specimens DTCB1, DTCB2, DTCB3, DTCB4, and DTCB5. Taking DTCB1 as an example, the compressive damage and state of the concrete and the Mises stress distribution of the honeycomb beam are shown in the following Figure 17. The distribution of damage stress in each specimen and the yield characteristics of the steel beam are consistent with the experiment. The test results and finite element analysis results of the bending bearing capacity of composite flat beam specimens are shown in Table 4, where \(M_{ys}\) is the measured value of the midspan bending moment test when the specimens yield, \(M_{ym}\) is the calculated value of midspan bending moment finite element analysis results when the specimens yield, \(M_{us}\) is the measured value of midspan bending moment test when the specimens fail, and \(M_{um}\) is the calculated value of midspan bending moment finite element analysis results when the specimens fail. \begin{table}
\begin{tabular}{c c c c c c c} \hline \hline \multirow{2}{*}{**Specimens**} & \(M_{ys}\) & \(M_{ym}\) & \multirow{2}{*}{**Error**} & \(M_{us}\) & \(M_{mm}\) & \multirow{2}{*}{**Error**} \\  & **(kN\(\cdot\)m)** & **(kN\(\cdot\)m)** & & & **(kN\(\cdot\)m)** & & \\ \hline DTCB1 & 81.3 & 80.8 & \(-\)0.62\% & 107.5 & 94.5 & \(-\)12.09\% \\ DTCB2 & 83.1 & 86.6 & 4.21\% & 110.0 & 98.5 & \(-\)10.45\% \\ DTCB3 & 75.7 & 78.8 & 4.10\% & 100.0 & 91.9 & \(-\)8.10\% \\ DTCB4 & 86.4 & 88.7 & 2.66\% & 115.0 & 105.6 & \(-\)8.17\% \\ DTCB5 & 82.6 & 80.4 & \(-\)2.66\% & 105.0 & 92.5 & \(-\)11.90\% \\ Average & - & - & 1.54\% & - & - & \(-\)10.14\% \\ \hline \hline \end{tabular}
\end{table} 
Table 4: Comparison between finite element simulation value and test value of flexural capacity. Figure 17: Failure mode of DTCB1. (**a**) Compress failure of concrete; (**b**) strain diagram of steel beam. The error between the simulated calculation value of yield bending moment and the measured value in the experiment is within \(\pm\)5%, with an average error of 1.54% and a mean square error of 0.0273. The simulated values of the ultimate bending moment of the specimen are generally lower than the measured values, with a maximum error of \(-\)12.09%, an average error of \(-\)10.14%, and a mean square error of 0.0173. The simulated calculation results of the yield bending moment and initial stiffness value of the specimen are basically consistent with the physical test results, indicating that the model has good consistency with the test in the elastic stage.