USE OF LIMIT ANALYSIS METHODS TO ASSESS THE STRUCTURAL CAPACITY OF SUBSEA SYSTEMS AND COMPONENTS

With advances in computational modeling techniques, limit load methods are gaining wider acceptance as a tool for determining the integrity of structural and pressure containing systems. The objective of a limit load analysis is to size a vessel or structure considering nonlinearities such as elastic-plastic material properties and non-linear strain-displacement relations. It is even possible to use experimental methods to determine the loading capacity of a structure [1]. In subsea and offshore environments, there are a variety of conditions that can lead to the need for limit analyses. Case studies are presented in this paper that feature scenarios including external pressures, pipe axial tension and bending, and dropped object impact loads. The limit load technique applies an appropriate initial magnitude for each load type and uses an analysis model or test set-up to increase the load until a lower bound load is calculated. The lower bound value is determined by incrementally increasing the load until the structures can no longer support additional loading without gross plastic deformation. This paper presents how limit load techniques were used to address the structural integrity of four engineered systems. These include the design of a subsea vessel under elevated external pressures, assessing the remaining buckling resistance of a dented subsea flowline, determining the effects of impact loads on an export riser, and evaluating the ability of a composite repair to reinforce a corroded riser using experimental methods. SUBSEA ELECTRONIC HOUSING A manufacturer of electronic equipment for subsea applications needed to optimize a design to achieve maximum water depths. Using a conceptual design, several analyses were performed using limit load methods. The primary design considerations involved geometric requirements associated with battery sizes and a design depth of 3,000 meters (9,840 feet). Initial efforts to size the dimensions of the design involved the use of a finite element model with shell elements. Once the geometry for the design was finalized, a limit analysis was performed using a model with solid eight-node hexagonal elements. The final analysis results demonstrated that the final geometry was adequately designed for the 3,000 meter depth requirement. Additionally, full-scale testing involving an external pressure of 10,000 psi proved the adequacy of the design. The sections that follow are some of the details on the analysis methods and results. Preliminary Shell Model Initial work involved using classical mechanics equations for basic sizing purposes. Once overall dimensions were determined, a preliminary finite element model using shell elements was constructed. In a design process, the shell element has an advantage in that its local thickness can be modified as an input variable, whereas solid elements require a complete reconstruction of the model geometry whenever dimensions such as wall thicknesses are changed. Figure 1 is a view of the basic shell finite element model. Using the shell element model, wall thicknesses were determined for specific regions of the subsea housing that could meet both the geometric and operating requirements of the design criteria. The results of this portion of the analysis determined the geometry for the final design. The final analysis involved the construction of a solid model that included the main body of the housing, the lid, simulated bolting, and contact interaction between the lid and body. Both the shell and solid models used limit load analysis. Elastic perfectly-plastic material properties for the aluminum 7075 material were input into the finite element model and external pressure was ramped up until convergence of the model was no longer possible. Because the primary intent of this project was development of a final design, the sections that follow provide specific details on the methods and results associated with the analysis of the solid element model. Solid Model Analysis The analysis of the three-dimensional finite element model using solid elements involved the following details: • Geometry included the outer cylinder of the main body housing, internal ribs oriented radially outward, 0.85-inch thick internal plate, and a 0.90-inch thick lid. • Contact was modeled between the lid and the main body housing. Contact was generated on top of the ribs and in the recessed portion on each end of the housing. • Bolting to attach the lid to the housing was accomplished by connecting nodes on the lid and body. This connection method was used for eight (8) regions on the housing located 45 degrees apart circumferentially. • A symmetry plane was invoked half-way between the ends of the housing. This cut the 0.85-inch internal plate in half. As with the shell model, this boundary condition prevents nodes on the symmetry plane from displacing in the 3-direction and prevents rotations about the 1-direction and 2-direction. • External pressure was of 10,000 psi was applied to all outside surfaces of the housing model including the lid and the cylinder. This value that exceeds that design requirement of 3,000 meters (approximately 4,370 psi), but was thought to be high enough that convergence would be unlikely for the current design.