Charis Ntontoros (Dodoros) presentation at ANSYS Convergence Conference 2016

ANSYS Convergence Regional Conference in Athens
Charis Ntontoros (Dodoros)
 30th of June, 2016

2
 Introductory Information:
 Experienced on Strength Calculations of Ship and Offshore
Structures
 Independent Structural Engineer based in Greece
 Partner of C-Job & Partners BV
 Naval Architecture and Engineering Office based in the
Netherlands
 Project References: Passenger, Cargo Ships – Heavy Lift
Vessels with Cranes of Operational Capacity up to 150 tons,
Yachts…
 Dredgers, Rock Dumping Vessels, Jack-Up Vessels, Tugs..
 Able to Perform Projects from Concept to Detail Design
30-6-2016ANSYS Convergence Regional Conference in Athens

30-6-20163
 Current Presentation Demonstrates two Analyses
Performed with Ansys:
 Part A:
Static Analysis on Rock-Dumping Fallpipe Tower Structure
 Part B:
Vibration Analysis on Thruster Foundation Structure

4
 A Few Words on the Project:
 Clients based on the maritime sector always need to increase
their operational abilities by upgrading their offshore structure
capabilities
 Rock-dumping vessels of 26,000 tons loading capacity are used
to install rocks in water depths up to 1,500 meters by means of
flexible fallpipe buckets
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure

5
 Rock - Dumping Vessel in Figures…
Structure

6
 Rock - Dumping Vessel in Figures…
Structure
30-6-2016
Fall Pipe Tower

7
 A Few Words on the Project :
 The fall pipe tower, located at the deck of the vessel, is
designated to carry the resulting loads from installed equipment
during operation
 The structure has been designed to operate in the most efficient
way in respect to the steel strength characteristics, operational
effectiveness and weight optimization
 34 different equipment items are installed on the fall pipe tower
structure, such as Winches and Pulleys
 Several Working and Sailing Scenarios can occur during the
lifetime of the vessel
 Multiple Load Cases (about 40) have been investigated
 All Results are assessed in accordance to the rules and
regulations provided by the certified classification societies
 Using Ansys, a representation of the Stress Occurrences and
Deflections is succeeded
Structure

8
 Pre-Processing: Creating the Structural Model
 Model has been created in SpaceClaim
 Model consists of Surfaces and Lines meshed with Plates and
Beam Elements
 Some parts were already modeled with solids in other designing
software and later imported in .STEP files in SC
 Solids have been converted to Midsurfaces through Midsurface
Tool in SC
 All parts of the model have been checked for their connectivity
(Shared Topology)
 Shared Node mesh has been achieved.
 Thickness property has been assigned in SC
 Parts which have been converted from solids to midsurfaces have
kept their thickness property in SC
Structure

9
 Pre-Processing: Preparing the Calculation Model
 Importing to Ansys Mechanical
 Preparing Name Selections and Meshing
 Multiple Element Size has been Assigned so as to Minimize
Calculation Time
Structure

10
 Element Types Used:
Shell181, Beam188, Mass21, Conta175, Target170
 Tower Structure Consists of Beam Elements
 Ship Structure (Hull) Consists of Plate Elements
Structure

11
Structure
Tower Meshed with
Beam Elements
Hull Meshed with
Plate Elements

12
 The beam like structure has been modeled with surfaces for 1
meter height above deck so as to smoothly transit the stresses on
the hull structure
 Unrealistic Hot Spots were avoided
 Tower’s Beam and Ship’s Plate Element Nodes were Connected
with Contact Elements
 MPC Formulation with Coupled U to ROT  This option is useful
when you wish to fully constrain one contact side completely to
another.
Structure

13
Structure

14
 Multiple equipment was installed such as Winches, Pulleys etc.
 Equipment itself was not modeled
 Equipment mass was applied at their actual CoG with point
masses
 In order to simulate the rigidity of the equipment the dummy
beams connecting the point mass to the structure were assigned
with rigid behavior
Structure

15
Structure

16
 Boundary Conditions:
The model has been fixed constrained on the nodes of the plate
elements at the lower end
Structure

17
 Post-Processing: Calculation & Validation of Analysis
 Extend of the Model - Validation
 Stresses were decreased at the lower part of the model
 Stresses were increased close to the boundaries
 Extension of the model was finally sufficient
 Reaction Forces retrieved were equal to the sum of the applied
loads and self weight of the structure
Structure

18
 Post-Processing: Calculation & Results
 Stress Results:
 Equivalent and Shear Stresses as required from the classification
societies
 Top/Bottom – Including out of plane bending (conservative approach)
 Stiffness Results:
 Total Deflection
Structure

 Post-Processing: Calculation & Validation of Analysis
30-6-201619
 Stress Results:  Stiffness Results:
Structure

20
 Post-Processing: Detailed Analysis, SubModeling &
Reporting
 Detailed stress analysis:
 Focusing on peak stresses
 Averaging Peak Stress values on the extend defined by Rules
 Requesting Membrane Equivalent Stresses with User Defined Result
 Sub-Modeling:
 Sub-models with refined mesh have been created from the global
model in areas of interest
 Exporting Stress Plots - Reporting:
 Automatically export defined stress plots with “Export Figures” Add-In
downloaded from the Ansys Customer Portal
Structure

21
 Self-elevating, Jack-Up vessels are commonly used for multiple
purposes in offshore projects, from drilling up to 114 meters
depth, to windmill park installations
Part B: Vibration Analysis on Thruster Foundation Structure

22
 The Jack-Up Vessel in Figures…

23
 The several structural areas of such vessels require detailed
engineering analysis
 One of these areas are the Thruster Foundations on which the
Rudder Propellers are bolted at

24
 The Thruster Foundation & Rudder Propeller:

25
 Thruster foundations are subjected to vibrational loads originated
by the rudder propellers
 The Rudder Propellers are designed by the manufacturer to
operate in a certain frequency range
 In accordance to the rudder propeller suppliers, the propeller
frequencies are to be “located” in a 25% range away from the
thruster foundation eigenfrequencies (natural frequencies), so as
to avoid excitation
The Thruster Foundation
Imported to Ansys

26
 A Few Words on the Project :
 First, a modal analysis is performed
 The frequencies under which the Thruster Foundation excites
are then known
 Some of the propeller frequencies given by the manufacturer were
belonging in the range of the foundation’s eigenfrequencies,
identified in the modal analysis
 An Harmonic (Vibrational) Analysis was required
 With the Harmonic Analysis it is possible to apply loads on a given
frequency range
 During the Harmonic Analysis the Force produced by the propeller
was induced on the foundation structure on the given frequency
by the manufacturer
 The Foundation Structure was excited by the propeller induced
force
 The expected peak stresses were then noted

27
 Pre-Processing:
 Modeling and Preparation of the Model in Ansys for calculation, is
very similar to the method followed for the Tower structure project
 No further explanation will be provided on this part

28
 Post-Processing: Modal Analysis
 It was known by the Rudder Propeller Manufacturer that the
propeller frequency range was between 15Hz and 25Hz
 During the Modal Analysis the first 20 Modes of the Thruster
Foundation have been requested
 From the 20 Modes, the Natural Frequency (Eigenfrequency) for
which resonance was noted on the Thruster Foundation was
equal to 21.853Hz and 23.267 Hz
 2nd and 4th Mode respectively

29
 Post-Processing: Modal Analysis
2nd Natural Frequency Noted on
the Foundation Structure, equal
to 21.853Hz
4th Natural Frequency Noted on
the Foundation Structure, equal
to 23.267Hz

30
 Pre-Processing: Harmonic Analysis (Forced Vibration)
 2 type of loads have been applied (Moments and Forces)
 A point mass was representing the mass of the Rudder Propeller
 Forces, Moments and Point Mass have been Applied on the
location where the Rudder Propeller was bolted at, with a Remote
Point
 Both moment and force loads are applied in the same phase
angle in a sinusoidal manner
 Moments and Forces have been applied under a frequency range
between 15Hz to 25Hz

31
 Post-Processing: Harmonic Analysis (Forced Vibration)
 Peak stresses are noted at the frequency area close to the
eigenfrequency of the foundation structure
 Relevant Graphs are exported from Ansys Mechanical
 Peak Stress at 21.800Hz  Close to 2nd Natural Frequency
 Peak Stress at 23.225Hz  Close to 4th Natural Frequency
 Max. Peak Stress about 80 Mpa
 Can reduce the service life of the vessel
@23.225Hz
@21.800Hz

32
 Post-Processing: Harmonic Analysis (Forced Vibration)
 Relevant Stress Plots are exported from Ansys Mechanical at the
frequencies where peaks are noted. @ 23.225Hz

33
 Post-Processing: Conclusions
 It is concluded that a fatigue analysis is required for the
assessment of the service life of the structure under the cyclic
loads imposed by rudder propeller
 Additional reinforcement will further increase the service live of
the vessel

34
!THANK YOU FOR YOU ATTENTION!

18-3-2015Froude Lunchlezing35
Your future, in the Maritime Industry

Charis Ntontoros (Dodoros) presentation at ANSYS Convergence Conference 2016

Recommended

Recommended

More Related Content

What's hot

What's hot (20)

Similar to Charis Ntontoros (Dodoros) presentation at ANSYS Convergence Conference 2016

Similar to Charis Ntontoros (Dodoros) presentation at ANSYS Convergence Conference 2016 (20)

More from SIMTEC Software and Services

More from SIMTEC Software and Services (20)

Recently uploaded

Recently uploaded (20)

Charis Ntontoros (Dodoros) presentation at ANSYS Convergence Conference 2016