1.
ANSYS Convergence Regional Conference in Athens
Charis Ntontoros (Dodoros)
 30th of June, 2016

2.
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
ANSYS Convergence Regional Conference in Athens
30-6-2016ANSYS Convergence Regional Conference in Athens

3.
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
ANSYS Convergence Regional Conference in Athens
ANSYS Convergence Regional Conference in Athens

4.
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
30-6-2016ANSYS Convergence Regional Conference in Athens

5.
5
 Rock - Dumping Vessel in Figures…
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

6.
6
 Rock - Dumping Vessel in Figures…
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure
30-6-2016
Fall Pipe Tower
ANSYS Convergence Regional Conference in Athens

7.
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
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

8.
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
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

9.
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
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

10.
10
 Pre-Processing: Preparing the Calculation Model
 Element Types Used:
Shell181, Beam188, Mass21, Conta175, Target170
 Tower Structure Consists of Beam Elements
 Ship Structure (Hull) Consists of Plate Elements
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

11.
11
 Pre-Processing: Preparing the Calculation Model
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure
30-6-2016ANSYS Convergence Regional Conference in Athens
Tower Meshed with
Beam Elements
Hull Meshed with
Plate Elements

12.
12
 Pre-Processing: Preparing the Calculation Model
 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.
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

13.
13
 Pre-Processing: Preparing the Calculation Model
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

14.
14
 Pre-Processing: Preparing the Calculation Model
 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
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

15.
15
 Pre-Processing: Preparing the Calculation Model
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

16.
16
 Pre-Processing: Preparing the Calculation Model
 Boundary Conditions:
The model has been fixed constrained on the nodes of the plate
elements at the lower end
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

17.
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
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

18.
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
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

19.
 Post-Processing: Calculation & Validation of Analysis
30-6-201619
 Stress Results:  Stiffness Results:
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure
ANSYS Convergence Regional Conference in Athens

20.
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
Part A: Static Analysis on Rock-Dumping Fallpipe Tower
Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

21.
21
 A Few Words on the Project:
 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
30-6-2016ANSYS Convergence Regional Conference in Athens

22.
22
 The Jack-Up Vessel in Figures…
Part B: Vibration Analysis on Thruster Foundation Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

23.
23
 A Few Words on the Project:
 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
Part B: Vibration Analysis on Thruster Foundation Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

24.
24
 The Thruster Foundation & Rudder Propeller:
Part B: Vibration Analysis on Thruster Foundation Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

25.
25
 A Few Words on the Project:
 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
Part B: Vibration Analysis on Thruster Foundation Structure
30-6-2016ANSYS Convergence Regional Conference in Athens
The Thruster Foundation
Imported to Ansys

26.
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
Part B: Vibration Analysis on Thruster Foundation Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

27.
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
Part B: Vibration Analysis on Thruster Foundation Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

28.
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
Part B: Vibration Analysis on Thruster Foundation Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

29.
29
 Post-Processing: Modal Analysis
Part B: Vibration Analysis on Thruster Foundation Structure
30-6-2016ANSYS Convergence Regional Conference in Athens
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.
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
Part B: Vibration Analysis on Thruster Foundation Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

31.
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
Part B: Vibration Analysis on Thruster Foundation Structure
30-6-2016ANSYS Convergence Regional Conference in Athens
@23.225Hz
@21.800Hz

32.
32
 Post-Processing: Harmonic Analysis (Forced Vibration)
 Relevant Stress Plots are exported from Ansys Mechanical at the
frequencies where peaks are noted. @ 23.225Hz
Part B: Vibration Analysis on Thruster Foundation Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

33.
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
Part B: Vibration Analysis on Thruster Foundation Structure
30-6-2016ANSYS Convergence Regional Conference in Athens

34.
34
!THANK YOU FOR YOU ATTENTION!
ANSYS Convergence Regional Conference in Athens
30-6-2016ANSYS Convergence Regional Conference in Athens

35.
18-3-2015Froude Lunchlezing35
Your future, in the Maritime Industry