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 ?