# A Nonlinear Transient Analysis of a wave-loaded steel bulkhead on a semi-submersible drilling rig

SIMTEC Software and Services
10. Jul 2018
1 von 18

### A Nonlinear Transient Analysis of a wave-loaded steel bulkhead on a semi-submersible drilling rig

• 1. Ocean Rig – Engineering Department Structural Engineer - Kardasi Sofia “A Non-linear Transient Analysis of a wave-loaded steel bulkhead on a semi-submersible rig” ANSYS Mechanical - StructuresANSYS Mechanical - Structures 2018 ANSYS Convergence Conference2018 ANSYS Convergence Conference 5 July, Athens, Greece5 July, Athens, Greece
• 2. 2 PRESENTATION OUTLINE  Introduction – Scope of the presentation  ANSYS Tools selected  Model Description  Results  Connections Check  Conclusion  Further Capabilities
• 3. 3  Introduction – Scope of the presentation Leiv Eiriksson OR 5th Generation Deep Water Semisubmersible Drilling Rig, Bingo 9000 design For drilling operations in water depths 70-2285 m Operating in harsh environment DNV Offshore Technical Guidance (OTG 14) for Horizontal wave impact loads on topside structure from large and steep waves–annual probability of 10-2 , for ULS design conditions (developed as a result of fatality). Negative air gap: when the wave upwell elevation is higher than the underside of the deck box. What needs to be checked: The local structural integrity of the wave-loaded area The global integrity of the whole structure – Rig The safety related equipment and personnel safety.
• 4. 4  ANSYS Tools selected ANSYS Mechanical for StructuresANSYS Mechanical for Structures:: Finite Element ModelingFinite Element Modeling Strength Analysis: to check model’s performance & possible failure modes Material nonlinearities – plasticity Newton-Raphson Method for equilibrium iterations (Force – Displacement) Contacts Advanced nonlinear stress simulations & Large Deformation of parts Transient Analysis: the Full Method Convergence criteria – Nonlinear Controls
• 5. 5  Model Description GeometryGeometry 3D Model in Autodesk Inventor Bulkhead of an area of six windows at Port Side – Worst case scenario Deck Framing Structure & Plating at three elevations Longitudinal Bulkheads & Girders on the Side view Windows protection steel cover & bolted mechanism on the inside ANSYS Design Modeler – Simplification and clean-up of the model
• 6. 6  Model Description ANSYS Design ModelerANSYS Design Modeler Import 3D model into Geometry Suppress some bodies that will not be used in the analysis Midsurface: creation of surface bodies that are midway between existing solid bodies Surface Extension: close all the gaps between edge sets Divide all the bodies into two parts; one for the structure & one for the windows layout Activation of shared topology for bodies that are included in the same parts The model is ready to be edited in ANSYS Mechanical → Transient Structural AnalysisANSYS Mechanical → Transient Structural Analysis
• 7. 7  Model Description ANSYS MechanicalANSYS Mechanical Engineering Data Structural Steel, fy=355MPa Structural Steel 2: Plasticity properties added → Multilinear Isotropic Hardening
• 8. 8  Model Description ANSYS MechanicalANSYS Mechanical Assign the Contacts in the model BondedBonded BondedBonded BondedBonded FrictionlessFrictionless
• 9. 9  Model Description ANSYS MechanicalANSYS Mechanical Assign the Joints in the model FixedFixed zoomed viewzoomed view
• 10. 10  Model Description ANSYS Mechanical Named Selections – to apply easily the boundary conditions and the loads to the model  Mesh • Shared topology for bodies in the same parts • Mesh relevance: 100% & Fine mesh relevance center • Mesh sizing: 2t=32mm for the wave-loaded area • Mesh sizing: 5t=80mm for the other area, where t is the thickness of the bulkhead Mesh metric graph Element QualityElement Quality
• 11. 11  Model Description ANSYS MechanicalANSYS Mechanical  Loads – Pressure – Time History Graph Boundary Conditions Zero displacement is assigned at all the outer edges to show the connection with the deck.
• 12. 12  Model Description ANSYS MechanicalANSYS Mechanical  Solve the model → A Non-linear transient Analysis will be performed  Analysis Settings • Number of steps: 1 • Initial Time Step: 1e-003 sec • Minimum Time Step: 1e-004 sec • Maximum Time Step: 1e-002 sec • Time Integration: On • Large Deflection: On • Nonlinear Controls → Newton-Raphson Option, Force, Moment, Displacement & Rotation Convergence, Line Search: Program Controlled &&
• 13. 13  Results Total Deformation Von-Mises Stress Directional Deformation
• 14. 14  Results Equivalent Plastic Strain A critical value of the plastic strainA critical value of the plastic strain (0.25) is defined according to specific calibration cases. Buckling of the horizontal stiffeners An amount of approximately 0.05 of plastic strain is obtained with this failure mode. The primary failure mode is tension failuretension failure on the horizontal plating that receives the wave loads. Failure ModesFailure Modes A zone of permanent strain is created where the machinery deck meets the horizontal plane, close to the weld and in the vertical zones around the window.
• 15. 15  Connections Check  Welded connection: bulkhead-protection base  Bolted Connection: clevis pin-protection base According to: Eurocode 3: EN 1993-1-8 (2005), Design of steel structures-Part 1-8: Design of joints, May 2005
• 16. 16  Conclusion  Finite Element Simulation results show that the maximum plastic strain is less than the allowable values that are specified by the calibration cases. The non-linear methods that are used in this analysis dictate specialized checks of plastic deflections in order to obtain a converged solution.  From the connections check, it is proved that all of the connections are to the safe side.  The bulkhead, with its stiffeners and girders has adequate structural strength to withstand the wave pressure.
• 17. 17  Further Capabilities  Parameters → i.e the thickness of the cover plate of the window  Design Optimization → a combination of key parameters in the analysis  Space Claim → user-friendly working environment, advanced options
• 18. 18 Any questions ?