Session: 13-03-03: General: Mechanics of Solids, Structures and Fluids III

Paper Number: 173268

Finite Element Analysis of Load Transfer and Stress Concentration in Multi-Plate Riveted Lap Joints 

This study presents a detailed finite element analysis (FEA) of a multi-plate, multi-rivet lap joint subjected to uniaxial tensile loading. The research is motivated by the need for improved understanding of stress distribution and load transfer mechanisms in riveted joints commonly used in aerospace and structural applications. The primary objective is to evaluate the structural performance of the joint particularly shear stress, von Mises stress, contact pressure, and displacement at critical interfaces such as individual rivets and plate layers. A mesh convergence study ensured result accuracy, particularly in high stress gradient regions.

The lap joint model consists of five aluminum alloy plates interconnected by fifteen inline solid rivets. The plates were assigned aerospace-grade materials based on their function: the two outer Fitting plates were modeled using 7050-T7451 aluminum, the Web plate used 2024-T4 aluminum, and both the Extrusion and Doubler plates were made of 7075-T6 aluminum. Material properties were defined using industry-standard mechanical values sourced from MMPDS (Metallic Materials Properties Development Standardization). A general contact interaction with a friction coefficient of 0.1 was applied to simulate the surface interfaces. The rivets were numbered sequentially from 1 to 15, with Rivet 1 located closest to the fixed boundary and Rivet 15 positioned nearest to the loaded surface. Boundary conditions were applied by fixing one end of the top and bottom Fitting plates to simulate support constraints. A pressure load of 12,000 lbf was applied on the opposite end of the Extrusion, distributed over an L-shaped surface, subjecting the assembly to a complex uniaxial loading condition with localized stress concentrations at geometric and loading discontinuities.

The mesh generation and convergence study were conducted using the finite element simulation tool Abaqus. All five components and fifteen rivets were meshed using C3D8R elements, forming a primarily hexahedral mesh. Due to geometric complexity, the Fitting plates included a combination of C3D8R and C3D4 elements across different partitions. The mesh convergence study was carried out by incrementally increasing the total number of elements across all components and monitoring key output parameters at predefined critical locations. For the rivets, shear stress (S12) and contact pressure (CPRESS) were observed at two distinct rivet locations. For the plates, S12 and displacement in the Y-direction (U2) were monitored at separate locations in the Extrusion plate, while CPRESS was tracked at a location in the Web plate. Convergence was considered achieved when successive mesh refinements resulted in less than 5% variation in all monitored output variables. The final converged mesh consisted of 18,566 elements, providing reliable resolution of stress fields and contact interactions while maintaining computational efficiency.

The simulation results revealed that the maximum contact pressure of 71,880 psi occurred at the 6th rivet, which also exhibited the highest von Mises stress of 40,810 psi among all rivets, identifying it as the critical load-bearing component in the joint. The 5th rivet experienced the highest shear stress of 9,647 psi, followed closely by the 6th rivet, which recorded a value of 9,248 psi. On the plate side, the Extrusion layer near the 15th rivet recorded a peak von Mises stress of 40,490 psi and a corresponding displacement of 0.166 inches in the Y-direction. The results also demonstrated expected stress concentrations near rivet holes due to geometric discontinuities and load transfer paths. The contact pressure distribution exhibited higher values near the fixed boundary and a gradual reduction toward the loaded end, with a secondary increase observed at the final few rivets.

The analysis highlights the role of geometric discontinuities, material interfaces, and contact interactions in generating stress concentrations within the lap joint assembly. Localized peaks in stress and contact pressure at specific rivets confirmed complex load transfer behavior. This study demonstrates the effectiveness of FEA in evaluating mechanically fastened joints and highlights the importance of mesh strategy in capturing localized phenomena, making it a valuable case study for engineers working on high-performance mechanical joints.

Presenting Author: Rakesh Kapania Virginia Tech

Presenting Author Biography: Dr. Kapania is the Norris and Wendy Mitchell Professor of Aerospace and Ocean Engineering. He obtained his BS in Aeronautical Engineering from Punjab Engineering College, Chandigarh India, MS in Aerospace Engineering from Indian Institute of Science, Bangalore, India, and Ph.D. in Aeronautics and Astronautics from the Purdue University, West Lafayette, IN.

Authors:

Vrutant Patel Virginia Tech
Courtney Fisher Columbia Helicopters, Inc.
Larry Pilkington Enstrom Helicopter Corporation
Rakesh Kapania Virginia Tech