Архивы Articles - Crane FEM Consulting

Approach for Measuring a Ship to Shore Crane Actual Wheel Load

Knowing the real crane deadweight, center of gravity (COG) and wheel loads instead of nominal ones is crucial for many reasons. One of the reasons relates to the checking the quay strength where the crane is going to be installed and it should be based on the crane maximum real wheel loads. Another example could be the crane transportation by sea on the deck of the vessel (Starykov & Van Hoorn, 2017). In this case predicting the precise value of the crane deadweight and its COG plays a key role in accurate calculation of the vessel stability, acceleration calculation from the ship motions and the vessel’s deck strength. This paper demonstrates a new approach to finding the crane wheel load and in the result the deadweight and COG position. This method does not need special arrangement and uses combination of strain gauge measurements and Finite Element (FE) analysis only. The application of the method is demonstrated on example of the ship loader for which the possibility of capacity increase has been assessed.

INTRODUCTION

One of the main limitations to the crane design is the maximum allowable wheel load, which mainly comes from a quay structure strength. Usually, this parameter is obtained from the crane FE model. The main source of mismatching with reality is that the model provides the nominal wheel loads, i.e., corresponding to the nominal dimensions and nominal weights of the structure elements. But in reality, the tolerances for weight and dimensions introduce the difference in position of COG and crane dead weight. As the wheel load is a crucial characteristic it should be controlled more precisely. If the crane was a smaller structure it would be possible to weigh it directly using a special platform or using a heavy lift to determine the real COG position and weight. For the contemporary quay cranes, which weight comes up to 1500 tones (Bartošek & Marek, 2013), using direct weighing would be a challenging task. Another area where the value of the crane deadweight and COG could be used are for the crane sea transportation. In this case knowing the dead weight and COG is critical for the ship stability and vessel acceleration calculation.

APPROACH DESCRIPTION

This work is proposing an approach that allows measuring the crane wheel load magnitude using strain gauges (Tutak, 2014) with further processing with FE analysis (Werkle, 2021). The method could be described as crane ‘weighing’ using the strain gauges. The approach’s main steps are:

Step 1. The stress in the crane travel wheels appears in the area between the wheel pin/shaft and the contact of the rail with the wheel, see Fig.1 and the rest of the wheel is unloaded. Using this observation, a strain gauge is attached to the crane travel wheel at pos. 1 (Fig. 1. a) to the area with no stress.

Step 2. Start crane moving and as the result of wheel rotation the area with the strain gauge becomes loaded by the wheel load (pos. 2, Fig. 1. b) and during the further rotation the stress there disappears again.

Strain gauge positions: a) pos. 1 – strain gauge is unloaded;
b) pos. 2 – strain gauge area is deformed by the wheel load. — Fig. 1. Strain gauge positions: a) pos. 1 – strain gauge is unloaded;
b) pos. 2 – strain gauge area is deformed by the wheel load

Step 3. The measured signal is proportional to the wheel load magnitude, but in order to find out the load in tons the additional step, calibration, is needed that would allow to transfer the original signal of mV/V to tons. The calibration is crated using calibration beam and the FE analysis of the wheel model

APPLICATION TO THE SHIP LOADER

The described approach is demonstrated for project of ship loader modification, when its capacity had been increased twice from 2000 t/h to 4000 t/h. One of the milestones of this project was to assess the increased magnitude of the wheel load with its further comparison with the maximal allowable load on the quay. This approach could be extended to the different types of cranes, like boom level-luffing cranes, quay cranes (ship-toshore cranes) that have the same travel arrangement, when the crane moves along the rails laying along the quay. Due to the lack of data on the ship loader structure element weights and its total COG the proposing experimental approach utilizing strain gauge measurement has been developed.

Fig. 2. Top view of ship loader and its travel arrangement

The ship loader has four supports: two sea side (labeled A and B) and two land side (labeled C and D), see Fig. 2. Each sea support has 4 wheels, and each land support has 3 wheels, see Fig. 3. The strain gauges have been attached to the outmost wheels of each support.

Ship loader and its travel arrangement - sea side support — Ship loader and its travel arrangement – sea side support

Ship loader and its travel arrangement - land side support — Ship loader and its travel arrangement – land side support

Step 1. Strain gauges are attached to the wheels in the “unloaded” area, away from area with stress from wheel / rail contact, see Fig. 4.

Fig. 4. Strain gauge attachment to wheel, pos. 1.

Step 2. Firstly, the crane is put into position for which the wheel load is measured. In case of ship loader, the boom has been put in horizontal position and all the sections are pulled out. According to the port authority the experiment was allowed without any cargo on conveyor belt only. The effect of cargo has been added to the wheel loads later by hand calculations. Secondly, the crane is moved using gantry travel so that the wheel rotates approx. 160 deg. allowing the strain gauge to pass the “stressed area”. The moment of the time during the wheel rotation when the strain gauge is in “stressed area” shows the maximum strain. The signal from strain gauge during the wheel rotation comes to the amplifier and then to the “analog to digital convertor” (ADC) which converts electrical voltage to the digital signal. An example of a typical signal from a strain gauge is shown in Fig. 5.

Fig. 5. Strain gauge signal during wheel rotation

The strain gauge maximal strains during wheel rotation are obtained using calibration beam and are shown in Table I and II.

TABLE I: MAXIMAL STRAIN GAUGE RELEVANT DEFORMATIONS FOR THE BOOM UP POSITION

TABLE II: MAXIMAL STRAIN GAUGE RELEVANT DEFORMATIONS FOR THE BOOM DOWN POSITION (WITHOUT MATERIAL ON THE BELT)

Step 3. Measured signal transformation into wheel load. In order to obtain the correlation equation between the measured strain and the wheel load, the finite element model has been created using FE analysis, Fig. 6 a. During this analysis a set of calculations has been performed in which the wheel load varied from zero to 40 tons with the increments of 1 ton. The result of one of the analyses is shown in Fig. 6 b. In order to reduce the scope of the problem only the half of the model has been created using symmetry boundary conditions.

Fig. 6. The gantry wheel finite element model. a) boundary conditions;
b) vertical relevant deformation plot.

The model symmetry property has been used during analysis. Based on the analysis the calibration curve is created (Fig. 7).

Wheel load - strain correlation curve. — Fig. 7. Wheel load – strain correlation curve.

The analytical form of correlation curve is shown in Fig. 7. is:

𝑃 = −77662,5 ∙ 𝜀?

where Р – wheel load, tons; 𝜀𝑍 – vertical relevant deformation of the strain gage location. The result of the relevant deformation recalculation to the wheel load is shown in Table III and Table IV.

TABLE III: WHEEL LOAD IN TONS AND THE UNEVENNESS OF ITS DISTRIBUTION AMONG WHEELS FOR THE BOOM UP POSITION

The maximum wheel load values, acting during the cargo being on the conveyor belt, have been determined by combination of the calculation data and measured wheel loads.

TABLE IV: WHEEL LOAD IN TONS AND THE UNEVENNESS OF ITS DISTRIBUTION AMONG WHEELS FOR THE BOOM DOWN POSITION (WITHOUT MATERIAL ON THE BOOM BELT CONVEYOR)

WHEEL LOAD IN TONS AND THE UNEVENNESS OF ITS DISTRIBUTION AMONG WHEELS FOR THE BOOM DOWN POSITION (WITHOUT MATERIAL ON THE BOOM BELT CONVEYOR) — * The significant difference in wheel load magnitude may be a result of a
poor equalizer joints’ condition.

Nominal weight of the ship loader is 247 352 kg. According to the measurements the ship loader weight for boom up position is 235 069 kg and for boom down position is 223 321 kg. Thus, the total measurement error: for boom up position is 5,0% and for boom down position is 9,7%. To minimize this error the strain gauges should be used for each wheel which would eliminate the effect of the poor equalizer joints’ conditions on the measured value.

CONCLUSION

In this study, a new approach was proposed to calculate crane weight, COG and wheel loads based on strain gauge measurements and FE analysis. The key advantages of this method are summarized below:

The method allows to find the real wheel load distribution, which is critical for the quay and also for the whole crane transportation on the deck of a vessel. • The method has a potential to be utilized for

The method has a potential to be utilized for validation of a crane’s nominal weight and nominal position of its COG that have been obtained during the crane design stage using hand calculation or FE analysis.

Wheel load measurement time is moderate, which makes the procedure effective.

Regarding the limitation of the presented method, the following aspects could be pointed out:

The wheel drawings are needed for the analysis.

The method allows to measure the wheel load for the cases that could be reproduced (i.e. it is impossible to force the wind to blow with different speed and different directions to allow to find the worst wind attack angle etc.). But these effects could be considered in addition using hand calculation.

Fatigue Life Assessment Approaches Comparison Based on Typical Welded Joint of Chassis Frame

Abstract

There are many approaches to the durability calculation that are used in engineering practice. At the same time the existing accident studies show that the leading position is still hold by fatigue failures. This means that there is still no universal approach to fatigue problem solution, and the existing approaches have their limitations. In addition, there is lack of information about the comparison between the precision of the obtained results using different approaches. In this paper different fatigue life calculation methods, like nominal stress, hot spot stress, notch stress and fracture mechanics are used to calculate the durability of T-type welded joint. The obtained results are compared with the fatigue test ones and the approaches, which give the closest results, are found.

Introduction

Time varying working loads are typical for metal constructions of chassis frames, material handling machines, ship hulls etc. According to accident studies for offshore structures [1], that took place in the North Sea, for period from 1972 to 1992, all reasons have been split into several groups according to their significance:

fatigue 25%;
structure collision with a ship 24%;
dropping objects 9%;
corrosion6%

In spite of the existence of different guides and approaches that have being used for fatigue design the significant part of failures caused by fatigue reveals the imperfection of using analysis methods. That is why the development of a new methodology is the pressing issue.

Modern fatigue design approaches are based on stress information about designing joint received from the finite element analysis of a structure. This gives the possibility of using the local stress in the probable area of the fatigue crack appearance instead of using nominal stress in the joint and broadens horizons for further enhancements.

Metal fatigue phenomena has been attracting a lot of researchers‘ interest for a long time and with the welding invention this interest even increased. The main problem was that all of researches solved particular problems (i.e. the effect of mean stress on the durability etc.) but there was no general practical approach with thorough step by step recommendations for the practicing engineers how to perform the analysis. The situation is changed during last decade when International Institute of Welding [2, 3, 4, 5], British Standard [6, 7], DNV [8, 9] have represented researches that are summarized in particular guides for the fatigue analysis with detailed description of practical utilization of the approaches, starting from mesh description and finishing with recommendations about what type of S-N curve to use.

With the aforementioned guides in the place the question of the analysis result validation has appeared. Thus, many researches have their goal to compare the fatigue experiment and analysis results [10, 11, 12, 13]. The main problem in our opinion is that in those researches only one method of the analysis is compared with the test results. But at the same time in engineering practice at least four of them are frequently used:

nominal stress approach;
hot spot stress approach;
notch stress approach;
fracture mechanics approach.

In this paper the comparison between main analytical approaches and test results for the fatigue life assessment has been done. This comparison could help to the practicing engineer to decide which approach to the durability analysis is more accurate for designing of similar joints.

For the analysis the T-type welded joint (Fig. 1) is chosen. Despite the fact that this type of connection is typical for a chassis frame, it is not covered in the researches. All the existing analysis, done for the T weld connection [10, 12, 13], have their welded gusset plate serving for stress concentration purpose only, when in the T-weld connection that is studied, the force and moment are transmitted to the main plate (crossbeam) through the gusset plate (longeron).

In the following chapters the durability of the joint is obtained using testing and different analysis approaches. The results are discussed in chapter “Discussion of the obtained results”.

Fatigue test results

The article objective is to define the approaches that give the closest result of fatigue life assessment to ones taken from fatigue test for T-type welded joint of a chassis frame [14].

Specimens have been tested using symmetric stress cycle (R= -1). The crossbeam was fixed using 4 holes of 10 mm in diameter and the 2 forces were applied using the 2 holes of 14 mm in diameter in longeron.

The fact of the crossbeam vertical deformation amplitude increasing beyond 30 % has been used as a collapse criterion to stop the fatigue tests.

The six joints have been tested on 6 different stress levels (Table 1). The fatigue curve of Weibull type has been used

Using linear interpolation the following parameters of Eq. 1 have been found: m_w = -2.489; C_w=3.3319.

Table 1. Fatigue test results for T-weld joint crossbeam to longeron

Based on Eq. 1 the fatigue life for stress amplitude with 50% failure probability is 425 100 cycles.

Fatigue life with failure probability of 2.3 % has been calculated using next equation:

where d – standard deviation amount below mean value, z_P=2.3%= z_P=97.7%=2 (quantile for failure probability of 2.3%)

lg σ_N – standard deviation of lgN, 0.178, p. 20 [2] for the specimen amount n<10.

Fatigue life with failure probability of 97.7 % has been calculated using next equation:

Fig. 3. Test machine

Traditionally beam theory for nominal stress calculation is used for S-N curve. But that stress is not representative for current joint because the fracture happens not in the crossbeam outer layers but in the area of welding seam transition to the longeron (Areas 1 and 2, Fig. 1).

Fig. 4. Crossbeam stress calculation using finite elements of beam and shell types

Using the shell finite elements gives realistic results. Maximum stress in crossbeam for the beam finite element (Fig 3. c) is 81.5 MPa, and for shell finite element (Fig 3. f) is 159 MPa.

Moreover, stress state of crossbeam in the area of welding seam is not more uniaxial one but complex i.e. all three principal stresses have non zero magnitudes.

Nominal Stress approach

The first step of nominal stress analysis [6] is to find among the variety of joint types with boundary conditions (showed in standard) the one that corresponds to the designing joint. But for currently calculating T-type welded connection the similar joint type does not exist. For the first look joint 5.3 (class F2, Fig. 5. a.), clause 2, Table 1, [6] could be taken, but its boundary conditions are different from analysing connection: unlike to the join from the standard the gusset plate (longeron) does not takes any load. That is why it can not be used further on. The joint on Fig 5. b can not be used for calculating either, because its boundary conditions differ from designing joint’s ones. It is also not clear stress in which element is taken for nominal (loading scheme is not shown).

Hot spot stress approach

This approach [3] allows calculating the joint fatigue life using its stress-strain state data obtained from the finite element analysis. The following joint modelling techniques are suggested to be used:

modelling using shell finite elements. In this case welding seam is to be create in such ways:
- model without welding seams;
- using oblique shell elements to model welding seams;
- using shell element with increased thickness for welding seams modelling;
Solid modelling with volume finite elements. Idealized welding seam shape is used.

Modelling using shell elements

Model without welding seams

According to IIW Recommendations [3] welded element durability is to be calculated based on stress that acts in the weld toe. However, because of using linear elastic metal behaviour and the fact that the real weld profile is unknown on design stage, there is no possibility to use directly the stress read from welding toe. Instead, it has been proposed to use stress extrapolated value based on stress in the welding seam vicinity, so called Structural Stress.

For our case (model consists of 4 node linear shell finite elements with edge of 1.6 mm near the stress concentration point) the hot spot stress is given by:

where σ_0.4·t– stress value at the distance of 0.4·t from the weld toe (the first extrapolation point);

σ_1·t– stress value at the distance of 1·t from the weld toe (the second extrapolation point);

t – longeron thickness, 4 mm.

The finite element model of T-welded connection is shown in Fig. 6.

Fig. 6. Finite element model

The minimum thickness of the plate the approach is applicable for is 5 mm.

Area of the stress concentration has been meshed using two techniques (Fig. 7).

Results of finite element analysis are shown on Fig. 8; hot spot stress extrapolation calculation is put into Table 2.

In currently overlooking standard the fatigue life assessment is based on principal stress with the biggest range during cycle. However, if the angle between this stress direction and normal to the welding seam line is more than 60 degrees, the stress perpendicular to the welding seam must be used. In our case Sy is used.

Hot spot stress approach is much easier to use in comparison with the nominal stress approach because it is based only on two S-N curves to assess the fatigue life in a “hot spots”. They are known as FAT 90 and FAT 100. The numbers that come after letters „FAT“ indicate stress level in MPa that corresponds to fatigue life for 2·10⁶ cycle durability. The general equation for these S-N curves is as follows:

where

Δσ_hs= σ_hs__max-σ_hs__min – stress range in the «hot spot», σ_hs__max – maximum hot spot stress of a cycle, σ_hs__min – minimum hot spot stress of a cycle;

m – index of power, 3.0;

С – coefficient, 2·10¹²;

N – life cycle

Table 2. “Hot spot” stress approximation and durability assessment

* Durability corresponding to different failure probabilities than other than 2.3% are calculated acc. Eq. 2 and Eq. 3.

Plane model with shell finite elements. Welding seam is modelled by oblique shell elements

The main concept of welding seam modelling is shown in Fig. 9 and meshed model – in Fig. 10 a).

Fig. 9. Welding seam modelling with oblique shell elements

For this case first principal stress is perpendicular to the welding seam. That is why it is used for the further analysis.

Fig. 10. Example of welding seam modelling with oblique shell elements

Table 3. “Hot spot” stress approximation and durability assessment

Solid model with volume finite elements

Solid model of the crossbeam-longeron welding connection is shown in Fig. 11. To reduce the computation time during model stress analysis only one half of the model has been created. 20 node Solid finite element with decreased integration and edge size of 4 mm is used.

The distances from the weld toe to the extrapolation points are the same (0.4·t to the first (nearest to weld) extrapolation point and 1·t to the second extrapolation point). Stress analyses result is shown in Fig. 12.

Table 4. “Hot spot” stress approximation and durability assessment

Notch Stress approach

This approach [4, 5] demands solid model creation and volume finite element mesh using. For the plate thickness less than 5 mm the Notch Radius of 0.05mm instead of 1mm has to be used, Special attention must be paid to a weld seam modelling particularly in the area where welding seam material merges to the main metal (Fig. 14 b) because the stress in this area is used for the fatigue life estimation. Only one S-N curve uses for this analysis (FAT 630) which equation takes a form of:

In addition to the weld toe modelling radius (Fig. 13) the approach specifies the welding seam geometry creation method, finite element size etc.

Fig. 13. Welding seam modelling requirements

Fig. 14. Crossbeam-longeron welding connection model for Notch Stress Analysis

Due to the high level of detail needed for welding area modelling the scope of problem increases with the growth of the joint complexity. That is why calculation time could increase from i.e. 20 minutes to several days. In this case the Sub-modelling feature is very useful. It helps to create more dense mesh and retrieve more precise solution for the smaller part of a model.

For crossbeam-longeron joint welding seam area sub-model of a fatigue crack initiation is shown in Fig 15.

Fig. 15. Crossbeam-longeron welding connection sub-model

Table 5. Principal stress variation during cycle and durability assessment

* Durability corresponding to different failure probabilities than other than 2.3% are calculated acc. Eq. 2 and Eq. 3. According [5] standard deviation of the lgN=0.206.

Fracture Mechanics based approach

The central idea of the approach [2, 3] consists in the using Paris equation for assessment of the joint fatigue stress cycles number till failure:

According to [7] either of two types of the crack growth relationship (Fig.17) could be used.

Using Eq. 7 the crack length – stress cycle relationship could be obtained:

After solving integral equation Eq. 8 the stress cycle number could be defined (N=N₂-N₁) that is needed for crack growth from length 2a₁ to 2a₂.

As per fracture mechanics theory a crack starts to grow if SIF range exceeds some threshold value (), which is different for different grades. Only SIF ranges more than this threshold are considered in analysis.

The failure criterion for the fatigue testing of the crossbeam-longeron welding connection is the 30% of longeron deformation range increasing. This corresponds to the crack length of L=2a=35.5 mm.

The method of solving Eq. 8 is as follows:

Define the SIF variation as the approximation . To do this the models of the joint with different crack lengths are created and for each crack length the SIF is calculated (calculation results are shown in Table 6 and Table 7)
Substitute the obtained approximation into the integral equation Eq. 8 and integrate

The initial limit, a₁ corresponds to SIF threshold value of the material (170 for R=-1, acc. (48 c), 8.2.3.6 [7]). Final limit, a₂=17,75 mm comes from the failure criterion during test.

As the life of crack initiation for welded joints is a small part of the total life [15], we will neglect it. The minimum crack length is defined for each case based on threshold SIF.

After analysis it became clear, that SIFs for all three modes are nonzero. Next Eq. 10 and Eq. 11 have been used to calculate the effective SIF, corresponding to the complex loading, that takes into consideration SIFs for all three different modes. Linear elastic material model has been used.

Table 6. Crack growth modelling results

As all three SIF are not equal to 0 the equivalent SIF has to be used for further analysis.

First model for equivalent SIF calculation:

Second model for equivalent SIF calculation:

First Model for equivalent SIF calculation with one stage crack growth relationship

The SIF approximation is shown on the graph above as a trend line equation

where m – index of power, 3, clause 8.3.3.5, [7],

А – coefficient of proportionality, 5.21·10^-13, clause 8.3.3.5 [7],

a₁ for this case equals to 0.9 mm.

First Model for equivalent SIF calculation with two stage crack growth relationship

Total durability would consist of durability for two stages (stage A and stage B). For the Mean Curve (Table 10 [7]) the stage A/Stage B transition point is 196, which corresponds to a=1.15 mm.

where A₁=4.8·10^-18, m₁=5.1, A₂=5.86·10^-13, m₂=2.88,

For the Mean Curve + 2SD (Table 10 [7]) The stage A/Stage B transition point is 144, which is smaller than the threshold value and that why during the Stage A the crack will not propagate.

Table 7. Crack growth modelling results

Fig. 20. Approximation of SIF range vs. crack length relation (the polynomial approximation is shown above the trend line)

The SIF approximation is shown on the graph above as a trend line equation

Discussion of the obtained results

It has been found that for the case of Hot Spot stress approach analysis without weld seam modelling the local orientation of 1st principal stress near the gusset plate to main plate connection ends is not perpendicular to the welding seam and that is the reason for using stress component perpendicular to the seam. At the same time for the cases where the welding seam is modelled (both shell and solid models) the 1st principal stress is perpendicular to the welding seam. Thus, the local stress strain state in models without modelled seams does not reflect the reality and the fatigue analysis based on local stress in these areas is not correct.
The thickness correction for 4 mm plate, applied with „Hot Spot“ stress approach, when the higher FAT class is used, gives significant overestimation of the joint durability.
For the case when weld seam is NOT modelled the lower stress is , but for models with welding seam . As the result the stress range for the models without welding seam is approximately twice bigger than for model with seam modelled.

Conclusion

Having analysed obtained results for crossbeam – longeron welding connection and compared them with the fatigue test following conclusion has been done:

Fatigue life assessment based on Nominal stress approach could be utilized only if the geometry and boundary conditions (type of joint fixation and applying loads) of the analysing joint comply with the one from the existing schemes of the Codes, for which data has been originally obtained by fatigue testing. The biggest problem is that the Codes do not cover all possible types of boundary conditions. For example, in the case of crossbeam-longeron joint analysis this method could not be used because the appropriate loading scheme could not be found in the Standard.
The closest to the fatigue test results are given by the fracture mechanics approach based on equivalent Stress Intensity Factor calculated acc. Eq. 11 in combination with:
1. one stage crack growth relationship (difference with test is 3.75%; the result is NOT conservative as the calculated durability is more than the test results);
2. two stage crack growth relationship (difference with test is -16.75 %; the result is conservative as the calculated durability is less than the test results).
The worst correlation with the test shows the “Hot Spot” stress-based approach without the seam modelling.
“Notch Stress” analysis result is close to the one obtained using “Hot Spot” stress analysis.
Regarding to the “Notch Stress” approach its main merit is that only this method among described above could predict the durability for the cases where the crack initiates from the weld root. Thus, sometimes it is only one option for analysis.

Acknowledgement

I would like to express my gratitude to the following my colleagues from Liebherr Mining Equipment for their valuable comments to may paper: James Witfield PE, Dr. Vladimir Pokras, Michael Karge.

Special appreciation is to my teacher, Doctor of technical science, Prof. Konoplyov A. V., for his permission to use the fatigue test results he has carried out.

References

Review of Repairs to Offshore Structures and Pipelines, Publication 94/102 Marine Technology Directorate, UK, 1994.
Fricke, Guideline for the fatigue design of welded joints and components XIII-1539-96/XV-845-96, 2010.
Niemi, W. Fricke and S.J. Maddox, Fatigue Analysis of Welded Components. Designer guide to the structural hot-spot stress approach, IIW-1430-00, 2007.
Fricke, IIW Guideline for the Assessment of Weld Root Fatigue IIW-Doc. XIII-2380r3-11/XV-1383r3-11, 2012
Guideline for the Fatigue Assessment by Notch Stress Analysis for Welded Structures IIW-Doc. XIII-2240r2-08/XV-1289r2-08 Wolfgang Fricke, 2010
BS 7608-1993 Fatigue design and assessment of steel structures, 1993.
BS 7910 Guide on methods for assessing the acceptability of flaws in metallic structures, 1999.
RP-203: Fatigue Design of Offshore Steel Structures, DNVGL-RP-0005:2014-06
Fatigue assessment of ship structures DNVGL-CG-0129, 2015
Baik, K. Yamada, T. Ishikawa, Fatigue Strength of Fillet Welded Joint subjected to Plate Bending, Steel Structures, 8 (2008) 163-169
Lassen, N. Recho, Fatigue life analysis of welded structures, ISTE, 2006
Comparison of hot spot stress evaluation methods for welded structures J-M. Lee, J-K. Seo, M-H. Kim, S-B. Shin, M-S. Han, June-Soo Park, and M. Mahendran, Inter J Nav Archit Oc Engng, (2010) 2:200~210
Lotsberg, Fatigue design of plated structures using finite element analysis, Ships and Offshore Structures, (2006), 45-54
General classification creation: Doctor of technical science thesis: 05.02.02/ Konoplyov A. V; Odessa National Polytechnical University. – O., 2013. – 39p. [inUkrainian] (Експериментально-розрахункові методи визначення границі витривалості деталей машин. Створення їх єдиної класифікації [Текст] : автореф. дис. … д-ра техн. наук : 05.02.02 / Конопльов Анатолій Васильович ; Одес. нац. політехн. ун-т. – О., 2013. – 39 с. : рис.)
Draper, Modern Metal Fatigue Analysis, Birchwood Park, Warrington : EMAS Pub, 2008.

Measured strain signal as a Boundary conditions for Finite Element submodel with application to crane structure residual life assessment

Abstract

The general flowchart of a crane structure residual life assessment could be split into two basic stages. On the first stage crane structure critical elements are determined usually using the Finite Element Analysis (FEA) for the given operational parameters (i.e. safe working load, maximum outreach and back reach, speed of mechanisms etc.). On the second stage the fatigue life of the critical elements is calculated using the same Finite Element (FE) model.

The key factor for such approach is the availability of the crane structural drawings, which allows to create precise FE model. And here the main problem appears that to find the drawings for the old machines is sometimes either a big problem or even impossible (i.e. the manufacturer company does not exist anymore). Similar problem could be challenging even for new cranes. The approach described in this paper allows to overcome the drawing absence problem by using the following modifications of the aforementioned procedure: critical elements are found using Non Destructive Testing (NDT); FE models of the critical areas are created using local structure measurements; FE analysis is performed using strain gauge measurements for Boundary Conditions during the crane operation.

The main flow of the proposed approach is that the residual life could be calculated for the crane operational parameters, the measurements have been performed for. Despite the paper uses crane structure as an example, the approach is general and it could be transferred on different types of steel structures.

Introduction

In the engineering practice the mostly used approach for stress analysis is Finite Element Analysis (FEA). In order to perform the FEA for the crane structure the following information about the crane must be presented:

Crane’s line diagram, where all structure elements are represented with their center lines or point masses; in addition, the elements’ sections geometrical parameters are also given (width, height, web/flange thickness etc.).
Crane elements’ weight and the Centers of Gravities coordinates.
Material properties of the crane elements’ grades.

This information could be taken from the structural drawings of the crane. Normally the crane owner may have the drawings, but in reality, it is quite hard to find the drawings especially for the machine that has been in operation for more than 20 years. Of course, one more way to find this information is to contact the crane manufacturer. However, it could lead at least to additional expenses to buy those drawings or sometimes the company does not even exist anymore and it is impossible to enquire the documents.

In this paper the approach that allows to overcome the structural drawing absence problem is proposed. As an example, the approach is used for 38-year-old Quay Grab Unloader residual life estimation as the FEA is a basic part of such type of project.

The idea of the approach is to find several critical elements of the crane, create the FE submodels for each of them based on geometrical measurements, performed on site. And instead of taking the boundary conditions (the forces that represent the action of the rest of the crane on the submodel) for these submodels from the whole crane Finite Element Analysis, get them from the processing of strain gauge signal measured during crane operation.

The residual life assessment approach for the considered Grab Unloader consists of the following steps

Find out the crane critical elements by combining the results from the crane structural surveying and the fatigue damage check method based on coercive force measurements.
Creating FEM models of the structure critical elements using geometrical measurements.
Measure the stress fluctuation during crane operation using strain gauges.
Process the measured signal and convert it to the FE model nodal forces.
Cut the material from the most critical element and test it to find the current, degraded properties of the grade.
Calculate the residual life of the critical elements based on crack growth modelling, using the material parameters obtained from the test and the “measured” boundary conditions.

More detailed description of each step is given farther on.

Finding crane structure critical elements

The crane critical elements have been found using the following two methods separately: structural survey; crane structure accumulated fatigue damage measurement. The obtained results have been analyzed and combined.

Structural survey. During the structural surveying the fatigue cracks of significant length have been found in the sea side Trolley Girder Support Beam (TGSB), near its center, where pulleys are attached Fig. 1. Thus, the critical element based on structural survey is TGSB central part.

Crane structure accumulated fatigue damage measurement. The approach is based on measured coercive force parameter. The measured coercive force is in proportion with the fatigue damage accumulated in the element. For each grade exists the coercive force critical magnitude that shows that the further operation is dangerous and could lead to structure failure. For the simplicity the whole range of the coercive force is split into several intervals: Reliable operation, Controllable operation, Critical Operation [1, 2, 3, 4]

The method could be used for the residual life estimation for the tested grades only, where the critical value of the coercive force is found. For the Grab Unloader grade the study of changing coercive force vs number of stress cycles does not exist. That is why only comparison analysis that shows the critical elements could be done instead of finding the residual life directly for each element. The critical elements are the ones with the biggest coercive force magnitude.

Based on the measured coercive force parameter it appears that the critical elements are Boom and Girder.

Combining the surveying results the following critical elements have been taken for the further residual life assessment (see Fig. 2):

Boom, the section between Boom/Girder hinge and Boom/forestay hinge.
Girder, between Land side and Sea side legs, just above the hopper where the crane unloads its grab.
Sea side TGSB middle part, where the pulley support is fixed to it.

Creating FEM models of the structure critical elements

Based on the geometrical measurements performed on site (i.e. member cross section height, width, flange and web thicknesses, bulkheads’ and stiffeners’ geometry etc.) the FE models of the critical elements have been created. As the further analysis is planned to utilize the Linear Fracture Mechanics approach one or two cracks have been introduced acc. [5] to each submodel (there are several models for each critical element where the only difference is the crack length). The cracks’ positions are based on preliminary analysis of the element without crack and the cracks were introduced in the areas with the biggest stress range. Each crack is oriented to be normal to the first principal strain. The linear material behavior model is used.

Measured stress for FEM submodels’ Boundary Conditions

Concept. Firstly, we have to find out the normal and shear stress distribution in a cross section which is used for the further boundary condition application. Then we could decide about the minimum amount of the strain gauges, their axis directions and positions along the section.

Stress distribution in cross section. For the normal and shear stress distribution the thin wall section beam theory is used. In crane structures the most frequently used types of cross sections are box and I beam types. As soon as all three critical elements of the Grab Unloader have box cross section type, all further analysis is done for this particular cross section type. This approach could be easily used for another cross section type (i.e. I beam). The typical box cross section with internal forces and moments is shown in Fig. 6.

The appropriate stress type (normal and/or shear) is calculated for each load component and the resultant stress distribution is found as a stress superposition. The following rules for the stress signs are used acc. [6]:

For normal stress: tension stress is assumed to be positive; compression stress is assumed to be negative.

For shear stress: positive shear stress acts on positive faces of the material element in the positive direction of an axis. Also, positive shear stress acts on negative faces of the material element in the negative direction of an axis. A positive face has its normal vector in the positive direction of an axis, and a negative face has its normal vector in the negative direction of an axis.

Normal stress from normal to the cross section force Fx:

Normal stress distribution from My bending moment:

Shear stress distribution from Fz shear force:

Normal stress distribution from Mz bending moment:

Shear stress distribution from Fy shear force:

Stress distribution over the cross section.

Stress superposition for all forces and moments is shown on Fig. 13.

Strain gauge minimum amount and positions

On this stage we could decide about the minimum amount of strain gauges we need to reconstruct the stress distribution based on measurements. Having analyzed the stress distribution it could be concluded that:

the normal stress is represented by polynomial with the maximum order of 1;
the shear stress is represented by polynomial with the maximum order of 2.

In other words, we need to have measurements from at least two point along each edge to reconstruct the normal stress distribution and at least three points to reconstruct shear stress distribution.

Minimum amount of the strain gauges for box section type beam

Application

The stress has been measured during 26 crane operational cycles using the modern 64-channel data acquisition device, Fig. 15. The device has several position sensors that were located along the Boom and Girder to show the trolley position during the measurements.

The strain gauges have been attached from the inner side of the structure. The gauges, positioned along and transversely to the critical element axis, were used; the positions are shown in Fig. 16 by arrows that are the gauge center lines.

Strain gauges’ positions on Boom, Girder and TGSB

Strain gauge signal snippet for TGSB critical element during crane operation

The snippet of measured signals from the strain gauges vs time are shown in Fig. 17.

The calibration coefficient to convert measured signal in volts to strain has been taken from laboratory tests (for each channel) using the specially designed beam (Fig. 18) with varying width to provide constant strain all over its length.

Beam for strain gauge initial signal calibration

On the first step strain gauge signal in volts was measured for test weights of 0, 0.5 kg, 1 kg, 1.5 kg and 2 kg. Then the corresponding strain magnitudes were calculated for all applied test loads using Strength of Material approach. This allowed to plot point in strain vs voltage axes.

On the second step the calibration coefficient was calculated using linear interpolation for strain vs voltage signal plot.

Using calibration coefficient Initial signal from the strain gauge (electrical voltage) has been converted to strain (Fig. 19, a; Step 1), then to stress (Fig. 19, b; Step 2), filtered out [7] and the stress cycles were extracted using Range-Pair Counting Method algorithm [8], Fig. 19.

Measured signal conversion volt-strain-stress

Based on the stress at the points where the strain gauges are placed the stress distribution diagram along each plate edge has been reconstructed for normal (Step 3) and shear (Step 4) stresses, Fig. 20.

The stress (normal and shear) distribution reconstruction along the plate edge

Finally, knowing number of FE along each edge, plate thickness and FE edge length, the stress to the FE edge has been converted to nodal forces, Fig. 21. In order to automatize the aforementioned steps C++ based programs and ANSYS APDL language macros have been used.

Nodal forces calculation based on the reconstructed stress

Boom critical element with applied boundary conditions

Material tests

The following material tests have been performed to find out the degraded properties of the Ship Unloader grade:

Uniaxial tension in order to find the possible changes of yield stress value due to the accumulated fatigue damage.

Impact toughness test to find the possible embrittlement of the grade due to the accumulated fatigue damage

Impact toughness test machine and specimen

Fractography for all mentioned above tested specimens

Fracture features of the specimen destruction tested for impact strength (with different resolution)

It is found that

Based on yield stress and impact toughness values there is no significant degradation of plasticity of the grade during the crane operational life.
At the same time, fractography found a large number of deep laminations in the steel. The laminations appear due to weakened cohesion between grade matrix elements, nonmetallic inclusions etc. Those laminations significantly decrease the robustness of the crane element and could be a reason of the crane collapse due to uncontrolled fatigue crack propagation.

Critical elements’ residual life assessment based on crack growth FEM analysis

The residual life has been calculated acc. [9] based on linear fracture analysis, which utilizes Paris low:

The cycles with SIF amplitude which is more than 0 have been considered in analysis. Also cycles with compression stress in the crack tip have been excluded.

Having analyzed all three submodels (Boom, Girder and TGSB) it was found that the element with the lowest value of the residual life is the TGSB with the critical area of the sheave support flange connection. The residual life of the unloader after repair, based on the fatigue analysis of its critical element, is approximately 9.7 years. It has been assumed that the crane will work with the same regime (same Safe Working Load, mechanisms accelerations etc.).

Summary

Advantages of the approach

The proposed approach allows to perform the FEM analysis for the crane elements in the cases when the structural drawings are not available.
The measured stress contains all the information about forces that appear during the real operational process (i.e. skew load on the trolley wheels, forces from the grab swaying on ropes, dynamic forces during closing the grab etc.). This allows to calculate the residual life more precise for the considered crane. At the same time for FEA analysis of the whole FE model those forces are unknown and are taken according to the existing standards where certain exaggerations are used to represent the crane worst operational conditions that in real life happen seldom and for the particular crane under consideration could not happen at all.

Disadvantages of the approach

The analysis could be done only for the current operational parameters of the crane. For the case when it is needed to calculate the residual life for the case of increased SWL or mechanism accelerations, the FEA of the whole crane and as the result the full package of structural drawings is needed.

References

Starikov, Beljatinskij, Perentkovskis, & Klimenko. The use of magnetic coercivity method to diagnose crane metalware. TRANSPORT, 26 (3), (2011), 255-262.
A. Starikov, Nikiforov Yu. A. (2012). Residual life assessment for the metallic structures of hoisting machines. Strengs of Materials, 44(1), (2012), 108-113.
Starykov, M., Methodology of residual life assessment in the metallic structures of lifting machines. TRANSPORT, 28 (3), (2013), 238-243.
Practical evaluation of fatigue and stress state, and residual life of metal by non-destructive method for measuring magnetic characteristic “The coercive force” – A case study / R. Solomakha, R. D. Pittala, G. Bezlyudko, B. V. Baskaran // Asia Pacific Conference on Non-Destructive Testing (14th APCNDT), Mumbai, India, November 18–22, 2013. – P. 1–9.
Information on http://www.cae.tntech.edu/~chriswilson/FEA/ANSYS/ANSYS_LEFM02.pdf
Information on https://en.wikipedia.org/wiki/Mohr%27s_circle
Draper, Modern Metal Fatigue Analysis, Birchwood Park, Warrington : EMAS Pub, 2008.
Standard Practice for Cycle counting in Fatigue Analysis. ASTM E 1049-85 (Reapproved 1997). (n.d.).
BS 7910 Guide on methods for assessing the acceptability of flaws in metallic structures, 1999.

The influence of a Quay Crane sea transportation on its further exploitation

Maksym Starykov, Frank Van Hoorn²

¹ PhD, Mechanical Engineer, Palfinger Marine, Bergen, Norway

²MSc, Naval Architect, Argonautics Marine Engineering, Inc, Windsor, USA

Corresponding author: Maksym, Starykov, starikovmax@yahoo.com

Submitted 06.05.2016; accepted date (use style Received dates, or Alt + Ctrl + R)

Abstract. For the last decades, fully erected container cranes have been delivered to a customer site by ships. On one hand, using this method of transportation is very attractive due to its cost and time savings. But on the other hand, being exposed to cycling loads from the ship motions during the sea voyage, the crane structure accumulates fatigue damage. Using the accumulated fatigue damage parameter, the crane transportation could be associated with the amount of the working cycles the crane could have worked out during its normal operating at the customer site. In the presenting paper the research for the real case of a new crane voyage from China to Ukraine has been done.

Keywords: crane sea transportation, fatigue damage accumulation, ship motion accelerations, finite element analysis, container crane, ship-to-shore crane, STS crane.

Introduction. In general practice of lifting cranes they could be delivered from the manufacturer factory to a customer site in two different ways:

By means of railway. In this case the crane is erected on the factory, passes all the tests, then is dismantled back into major parts which are loaded onto platforms and delivered to a customer site(J.Verschoof, 2002). Main disadvantages of this method are the necessity of time and costs for the crane additional erecting, disassembling; the final erecting on the customer site takes time and quite a space, and in the case of a container terminal the terminal owner experiences certain inconvenience.
By means of sea transportation. In this case the fully erected and temporarily reinforced crane is loaded on a ship of special type, secured by lashings and some additional supports (in some cases it could be partly dismantled) and transported by sea. This method has been being used to deliver the relatively large crane to the customer site for the last 20 years. The main obvious merits are time and cost savings, the possibility to use the machine in short time after its delivery (Martin C, 2004),(Van Hoorn, Design Criteria for Self-Propelled Heavy-Lift Transports – And How Theory Theory Correlates with Reality, 1991), (Capitan, 1989).

1. Statement of research problems and the technique for their decision.
The main disadvantage of the crane delivery by means of sea transportation could be understood after a closer look at the cyclic loads, which act on the carried crane from the ship motions along the whole voyage. The loads could have quite significant magnitude and amount of cycles, which leads to fatigue damage accumulation (Murakami, 2012) in the crane elements and joints. In the other words it means that after a new crane is delivered by sea to the customer site it is not a new anymore, but has a condition which is equivalent to being in operation for some time.

Of course, each transportation case is individual and the following cases are possible:

The stress level in the crane structure could be lower than the one that creates fatigue damage. Then no fatigue damage accumulates and the crane condition at the customer side after the voyage is the same as it was at delivery from the factory.
Transportation routes could be short enough and the crane would not be undergoing significant amounts of load cycles. In this case, the accumulated fatigue damage during the voyage could be very small and neglected.

The main goal of the current research is in finding out if the delivery of the fully erected Ship to shore crane by vessel damages the crane by decreasing its service life and in the case of positive answer assess this damage in terms of working cycles. The main parameter that is checked by structural engineers on the project preparation stage is the static strength of the crane structure, lashing elements, deck of the carrying vessel and all the reinforcements. Unfortunately, investigations of the influence of a fully erected crane transportation by sea on its residual life, which involves fatigue analysis of the structure but not only static strength, have not been found. In this paper, the analysis for specific case has been done in order to assess such influence.

Thus, the novelty of the current research is in the investigation of carried crane service life decreasing due to the sea voyage based on fatigue damage accumulation assessment.

A real case of a ZPMC© quay crane delivery from China to Ukraine has been used for this analysis. The route is shown in fig.1.

Figure 1. The ZPMC vessel route, which transports the quay crane from Shanghai (China) to Yuzhne (Ukraine). The small green squares contain the date when the ship passed the point

The basic crane (fig. 2) parameters are as follows:

Lifting load under the spreader – 60 tons.
Outreach, A – 55meters
Back reach, B – 16 meters,
Lifting height (above rail), C – 36 meters.

Figure 2. The quay crane general arrangement. The cross section of the container carrier with the numbers of container rows are shown at the right lower corner (#1-#20)

The cranes position on the ship during its transportation is shown in figure 3.

a)
b)	c)

Figure 3. The crane on the ship’s deck

The analysis of the crane has been split into three major stages. On the first stage the loads on the crane structure due to the ship motions have been calculated. The second stage involves finite element analysis for crane static strength under the influence of the mentioned above loads. On the last stage, based on the obtained stress data for the crane structure during the voyage and using a specially created program, fatigue damage accumulated in the crane structure has been calculated.
2. Loads from ship motion determination
Based on the limited data available, the ZHEN HUA 11 vessel was modeled based on the hull of a standard bulk carrier, converted into the crane carrier, with identical dimensions (similar to the real – full scale – conversion) (Van Hoorn, Container crane transportation option: Self-propelled ship versus towed barge, 2005), (F. van Hoorn, Wijsmuller Transport B.V. and S.D. Devoy, Matthews-Daniel Co.,, 1990). For the computer model of the resulting hull, see figure 4 the loading condition was prepared based on the crane and RTG data, estimated lightship of the vessel, and some additional weights for bunkers, ballast, and some miscellaneous. The approximate stowage plan is presented in figure 5.

Figure 5. Approximate stowage plan

The resulting loading condition is summarized in table 1.

Table 1. Loading condition ZHEN HUA 11 with 3 STSs and 5 RTGs

Displacement	60,300	T
Draft bow	6.9	M
Draft aft	8.6	M
GM’	8.3	m
Roll gyradius	13.9	m
Roll period	12.5	s

For the environmental conditions for the voyage from Shanghai, China, to Yuzhne, Ukraine, the Global Wave Statistics were used. A combined voyage scatter diagram was made by adding all scatter diagrams for the areas crossed together, each weighted with a transit time factor. The same wave data base also provides wave direction statistics for the individual areas crossed (N. Hogben et al, 1986) (Van Hoorn, Heavy-Lift Transport Ships – Overview of Existing Fleet and Future Developments, 2008). Combining these with the transit times (exposures) resulting in the following probability for each class of wave heading:

34% exposure to head and following seas;
49% exposure to bow and stern quartering seas;
17% exposure to beam seas.

With the combined total voyage scatter diagram and using the MOSES© software program, the vessel motions and point accelerations at the crane CG were calculated for each wave height – wave period combination. This resulted in double significant design acceleration scatter diagrams for each of the 3 main directions. For each direction, the linear accelerations were grouped in 0.1 g interval classes and the numbers in each class were totaled, as presented in table 2. The double or full cycle significant (mean of highest 1/3) values give a good representation of the accelerations acting on the crane CG in each of the three main directions.

The loads are represented by linear accelerations along all three axis that are considered to be applied to the crane center of gravity (table 2). Total amount of oscillations is 461 000, cycle time is 10 seconds.

Table 2. Accelerations applied at Center of Gravity of the crane structure due to the ship motions

Acceleration range in units of “g”	Longitudinal acceleration oscillations (total)*	Lateral acceleration oscillations (total)*	Vertical acceleration oscillations (total)**
0.0 – 0.1	459,324	345,259	424,125
0.1 – 0.2	1,676	77,234	33,430
0.2 – 0.3	–	26,347	3,292
0.3 – 0.4	–	7,867	148
0.4 – 0.5	–	3,443	5
0.5 – 0.6	–	549	–
0.6 – 0.7	–	209	–
0.7 – 0.8	–	59	–
0.8 – 0.9	–	32	–
0.9 – 1.0	–	1	–

* – includes static part

** – excludes static part 1g

For the crane structural analysis, its model with lashing elements has been created (fig. 6).
3. Model description
The crane model has been prepared using ANSYS© utilizing finite element approach for stress calculation (Madenci, E., Guven, I, 2006), (Arsian, 2015), (Stolarsky, T., Nakasone, Y., Yoshimoto, S., 2006). The following finite elements have been used (fig. 6):

BEAM – for modelling of crane main elements (as legs, girder, boom, A-frame, stays etc.) and reinforcement structures (as boom support and crane four corner additional supports).

LINK – for lashing ropes. Initial pretension (2 tones) in each rope has been modelled.

MPC – for modelling of joints with only rotational degree of freedom. In order to model the saddle pin behavior the boom-girder joint has been modelled with the rotation restrictions.

MASS – for modelling attached elements masses, as machinery, trolley rails, ladders and platforms, elevator etc.

a) the beam model with shown beam element sections

b) crane skeleton model (beam sections are turned off)

Figure 6. The crane finite element model

The linear model of a material behavior has been chosen with Young modulus of Pa and Poisson ratio of .

The model loadings have been applied during two phases: preparatory loading steps and main loading steps.

The first preparatory loading step corresponds to the quay crane situated on the ship deck just after its disposal. It means there are neither supporting nor reinforcing structures installed yet (fig. 7). The crane structure has been loaded by its self weight and prestressed lashing ropes. Under the applied forces the structure had the initial deformation. The crane support structures (boom propping frame including two lashing wire rope that connect middle of the frame with the boom; supporting tubes at all 4 corners of the gantry) have also been modelled on the first stage, but turned off using birth/death element technology.

On the second preparatory loading step, the crane support elements have been turned on (fig. 8), and started propping the initially deformed crane structure. The main point of the splitting the preparatory loading into two steps is to model real situation, when the support elements have been applied to the deformed crane structure and therefor the only stress that could appear in the reinforcement comes from ship motions and reinforcing elements self-weight.

The boundary conditions for the crane attachment to the ship deck modelling are shown in fig.9.

Figure 7. Crane structure considered on the first preparatory loading step

Figure 8. Crane reinforcement elements, turned on the second preparatory loading step

Figure 9. boundary conditions, applied to the crane structure at first and second phase

During the second phase the loading cases that represent the structure loading with acceleration (according to the table 2) due to the ship motions have been created (PADT and Jeff Strain, 2013). For each acceleration class two loading cases have been created with acceleration acting in two opposite directions. As far as the number of cycles are given for the acceleration range, in calculation the mean value of the acceleration class range has been used.

For instance, for the longitudinal acceleration class 0.2 – 0.3 g the mean value range of 0.25g has been taken and two loading cases have been created, first one with acceleration of +0.125g and the other with -0.125g. Subtracting the second loading case from the first one gives the loading case with the stress range in the crane structure.

In addition to the stress information for the further fatigue analysis, the information regarding structure elements fatigue classification (FAT class) (Draper, 2008) is needed. For this purpose the FAT class has been assigned to all elements of the crane main structure (fig.10).

Figure 10. Elements with assigned FAT classes

For the last phase of the analysis the special program has been created (Stroustrup, 2014) that uses the external information about structure elements FAT classification and the stress for loading cases for input data. The algorithm of the program is shown in fig. 11.

The program utilizes the nominal stress approach acc. (BS EN 13001-2:2014 Crane safety. General Design. Load actions, 2014), (Hobbacher) and Palmgren-Miner cumulative damage rule (Jean Lemaitre, Rodrigue Desmorat, 2005), (Chaminda, 2015).

Figure 11. Customer fatigue analysis program algorithm

The result of the program operation is the information about accumulated fatigue damage in each element.

Basic assumptions, used in the program algorithm, are as follow

FAT class is the same for all areas of the element section. The lowest FAT for the section has been used for calculation;
Tensile and compressive stresses are considered as equally dangerous ones;
The element fatigue life correction due to the element thickness has not been taken into account (for elements with thickness more than 25mm). However, for the crane structure almost all elements have plate thickness up to 25 mm. The only exception is the Trolley Girder Support sea side Beam (TGSB) with the biggest thickness of 30 mm. And the fact that it is not a fatigue critical element justifies avoiding using plate thickness correction in program.
All the accelerations due to the ship motions have been considered acting separately rather than in combination.

According to the recommendations for the fatigue analysis (Hobbacher) the critical accumulated fatigue damage value is 0.5 and according (FEM 1.001. Rules for the designing of hoisting appliances. 3rd edition, 1998) it is 1.0.

The results of the fatigue damage accumulation (Lee, 2005) for the crane exposed to longitudinal, vertical and transversal accelerations are shown in fig. 12 and 13. The maximal accumulated fatigue damage D of the range from 0.1 to 0.05 has been found in the boom diagonal beam (fig.12). The fig. 13 shows the elements with the maximal accumulated fatigue damage from 0.05 to 0.025.

Figure 12. Elements with the maximal accumulated fatigue damage from 0.1 to 0.05 (boom diagonal, shown in red)

a)		b)
a)		c)

Figure 13. Elements with the accumulated fatigue damage from 0.05 to 0.025 (shown in red)

The fatigue analysis shows that during the crane transportation on the deck of the ship the crane structure has been damaged by the loading cycles, initiated by the ship’s motions. Using the accumulated damage values the crane transportation could be associated with the amount of the working cycles the crane could have worked out during its normal operating at the customer site (table 3).

Table 3. Crane transportation association with its normal operation

Critical Elements with accumulated fatigue damage and as the result decreased service life due to the transportation	Calculated Damage, accumulated during the sea transportation, Di	, Crane element’s life (maximal) lost during the crane transportation, based on critical value of fatigue damage D=1*	Crane element’s life lost (maximal) during the crane transportation, based on critical value of fatigue damage D=1, working cycles**	Crane element’s life (maximal) lost during the crane transportation, based on critical value of fatigue damage D=0.5 *	, Cran’e elements life (maximal) lost during the crane transportation, based on critical value of fatigue damage D=0.5, cycles ***
Boom diagonal beam, fig 9	0.1-0.05	10%	200,000	20%	400,000
Leg parts, portal diagonals, lower TGS beam, sill beam,	0.05-0.025	5%	100,000	10%	200,000

* the calculation is done

** assuming crane life of 2 million cycles, crane element lost life is

*** assuming crane life of 2 million cycles, crane element lost life is

Of course, not all elements that have accumulated fatigue damage are critical from the fatigue point of view for normal operation. The good example is the boom diagonal, which is almost not loaded during the crane normal exploitation.
4. Discussion of the obtained results
According to the obtained results of the fatigue damage calculation, accumulated during the crane transportation by sea, it appears that up to 20% of the crane life has been used during its transportation. The crane that came down to the customer’s port was not the new crane, but already “used”. The fact the crane had lost such significant part of its structure life could give the customer some negotiation freedom in terms of either price reduction, increasing the warranty period or the other options.

For different cases of sea transportation such discussions between the manufacturer and customer should be based on the analysis, which could be similar to the one, shown here.

The performed analysis has been done based on accelerations of the ship, obtained from the computer modelling based on Global Wave Statistics (N. Hogben et al, 1986). The computer analysis very often gives overestimated results (Van Hoorn, Container crane transportation option: Self-propelled ship versus towed barge, 2005) and for more precise fatigue damage accumulation in the crane structure the strain measurement technic during the whole voyage could be used.

For this case before the voyage, the fatigue analysis should have been done in order to find the possibilities to minimize the accumulated fatigue damage by proper transportation plan (lowering down the CG of the whole crane by partly dismantling boom, girder and/or A-frame). The best transportation scheme is the one, for which the ship accelerations induces in the crane structure stresses with amplitude less than the endurance limit and the fatigue damage does not accumulates. Instead of this the manufacturer of the crane applied to the structure some reinforcements, but their positions and amount were decided from static strength point of view and that have not prevent fatigue damage accumulation.
5. Conclusion

The main merits of a crane transportation by sea, as time and cost savings, are well known and it is the main reason why this type of delivery is widely used nowadays. However, at the same time, nobody pays attention what happens with the crane during its sea voyage from the fatigue point of view, when it could be exposed to forces from the ship motions, and those forces, having both big magnitude and significant amount of cycles, could cause the crane structure fatigue damage accumulation.
In order to assess the significance of the fatigue damage for such crane delivery the analysis of the real case of a quay crane transportation from China to Ukraine has been carried out. It shows that during the transportation basic crane elements, as legs, portal pipe strut frame, sill beams, lower TGS beams, boom forestays of the crane structure accumulate up to 5% or 10% of the critical fatigue damage value (depends on the using critical value).
Using the parameter of the fatigue damage, the loading cycles, which acted on the crane during its sea voyage from the ship motions, could be associated with the crane working cycles that it could have worked off in normal operation. For this particular case the sea transportation is equivalent to wasting maximum 100 000 or 200 000 (depends on the using critical vale) crane operational cycles for such crane element, as legs, portal pipe strut frame, sill beams, lower TGS beams, boom forestays.
Using either proper designed crane structure support or partial dismantling of the crane elements could decrease significantly or in some cases even totally eliminate the fatigue damage accumulation during the crane transportation. For this, the additional fatigue crane structure analysis is needed, but the expenses for it will be fully covered by decreased costs for the further crane structural repair and downtime costs.

6. References
Arsian, M. (2015). Hands on Applied Finite Element Analysis Application with ANSYS.

BS EN 13001-2:2014 Crane safety. General Design. Load actions. (2014).

Capitan, A. B. (1989). Use of Metereological Information for Warranty Surveying Purposes. The Nautical Institute, London.

Chaminda, B. (2015). Fatigue Damage Assessment of Steel Structures and Components. Lambert Academic Publishing.

Draper, J. (2008). Modern Metal Fatigue Analysis. EMAS Publishing.

van Hoorn, Wijsmuller Transport B.V. and S.D. Devoy, Matthews-Daniel Co.,. (1990). The Dry Transport of the Green Canyon Tension Leg Wellhead Platform by a Semisubmersible Heavy-Lift Ship. , . 22nd Offshore Technology Conference . Houston.

FEM 1.001. Rules for the designing of hoisting appliances. 3rd edition. (1998).

Hobbacher, A. (n.d.). Fatigue design of welded joints and components XIII-1539-96/XV-845-96.

J.Verschoof, I. (2002). Cranes – Design, Practise and Maintenence. Proffesional Engineering Publishing.

Jean Lemaitre, Rodrigue Desmorat. (2005). Engineering Damage Mechanics: Ductile, Creep, Fatigue and Brittle Failures. Springer.

Lee, Y.-L. J. (2005). Fatigue testing and analysis. Theory and practice. Elsevier.

Madenci, E., Guven, I. (2006). The Finite Element Method and Application in Engineering using ANSYS. Springer.

Martin C, P. (2004, July). West Coast Gantry Cranes: The Path of Paceco and ZPMC. Pacific Maritime.

Murakami, S. (2012). Damage Mechanics. A continuum Mechanics Approach to the Analysis of the Damage and Fracture. Springer.

Hogben et al. (1986). Global Wave Statistics, British Maritime Technology Ltd. Feltham.

PADT and Jeff Strain. (2013). Introduction to the ANSYS Parameter Design Language (APDL).

Stolarsky, T., Nakasone, Y., Yoshimoto, S. (2006). Engineering Analysis with ANSYS software. Elsevier.

Stroustrup, B. (2014). Principles and Practice Using C++. Second Edition. Eddison-Wesley.

Van Hoorn, F. (1991). Design Criteria for Self-Propelled Heavy-Lift Transports – And How Theory Theory Correlates with Reality. Second Offshore Symposium on Design Criteria and Codes. Huston, TX.

Van Hoorn, F. (2005). Container crane transportation option: Self-propelled ship versus towed barge. Rina Conference on Marine Heavy Transport & Lift. London.

Van Hoorn, F. (2008). Heavy-Lift Transport Ships – Overview of Existing Fleet and Future Developments. MOSS 2008 conference. Singapore: MOSS.