Structural Modeling and Failure Assessment of Spar-Type Substructure for 5 MW Floating Offshore Wind Turbine under Extreme Conditions in the East Sea

: Not only the driving for offshore wind energy capacity of 12 GW by Korea’s Renewable Energy 2030 plan but also the need for the rejuvenation of existing world-class shipbuilders’ in-frastructures is drawing much attention to offshore wind energy in Korea, especially to the diverse substructures. Considering the deep-sea environment in the East Sea, this paper presents detailed modeling and analysis of spar-type substructure for a 5 MW ﬂoating offshore wind turbine (FOWT). This process uses a fully coupled integrated load analysis, which was carried out using FAST, a widely used integrated load analysis software developed by NREL, coupled with an in-house hydrodynamic code (UOU code). The environmental design loads were calculated from data recorded over three years at the Ulsan Marine buoy point according to the ABS and DNVGL standards. The total 12 maximum cases from DLC 6.1 were selected to evaluate the structural integrity of the spar-type substructure under the three co-directional conditions (45 ◦ , 135 ◦ , and 315 ◦ ) of wind and wave. A three-dimensional (3D) structural ﬁnite element (FE) model incorporating the wind turbine tower and ﬂoating structure bolted joint connection was constructed in FEGate (pre/post-structural analysis module based on MSC NASTRAN for ship and offshore structures). The FEM analysis applied the external loads such as the structural loads due to the inertial acceleration, buoyancy, and gravity, and the environmental loads due to the wind, wave, and current. The three-dimensional FE analysis results from the MSC Nastran software showed that the designed spar-type substructure had enough strength to endure the extreme limitation in the East Sea based on the von Mises criteria. The current process of this study would be applicable to the other substructures such as the submersible type.


Introduction
Among the renewable energy resources, wind energy has been growing steadily and securing the competitiveness of price through its lowering levelized cost of energy (LCOE). In particular, onshore wind has shown large cost reductions over decades with economically large-scaled wind turbine size and wind farms construction in addition to the improvement of the technologies and logistics, which lead to a preferable choice among other alternative renewable energy sources against fossil fuel energy [1][2][3][4].
But the onshore wind farms have been facing many limitations for large-scale wind turbines installation due to the visibility issue, noise emission, transportation difficulty, and other opposition aroused from residents. Moreover, due to their surrounding land conditions, onshore wind turbines are more likely to have lower capacity factors which could decrease the overall power performance [5][6][7]. To overcome these problems, wind proper design strategies according to the dynamics of substructures [34]. However, there is little research on the detailed structural modeling process and stress analysis of a spartype substructure for a FOWT utilizing the coupled load analysis and the interface between the nonlinear time-domain multi-physics models (aero-hydro-servo-elastic) and three-dimensional finite element model. Furthermore, even though there was a study on the substructures for the Southwest offshore wind farm in Korea with a water depth under 33 m, few studies were published for the FOWT in the East Sea of Korea, where six GW floating offshore wind farms were planned [35].  [24].
In this work, the design process on the structural model and analysis of a spar-type substructure for a 5 MW FOWT specially designated to the East Sea in South Korea will be presented in detail with a fully coupled integrated load analysis and three-dimensional finite element model/analysis. FAST, a widely used integrated load analysis software developed by NREL, was coupled with in-house hydrodynamic code (UOU code) [36,37]. The environmental design loads will be calculated from the data recorded for three years at the Ulsan Marine buoy point according to the ABS and DNV standards [38,39]. The three-dimensional (3D) structural finite element (FE) model of a spar-type substructure The design of a FOWT in the deep-water environment is complicated compared to conventional fixed offshore wind turbines because of the complex external load conditions caused by waves, wind, and current as well as the structural loads including the hydrostatic pressure and ballast loads [25]. Due to the highly coupled interaction of aerodynamics from wind and hydrodynamics from the ocean, it is important to understand the dynamic behavior of the floating platform related to the six degrees of freedom such as pitch, yaw, roll, surge, heave, and sway to design the optimal substructure to mount the wind turbine generator [26]. There are many studies that have been performed for the dynamic response of floating offshore wind turbines and the resulting dynamic response values are then used for the structural analysis of the substructure model in detail [27][28][29][30].
Bagbanci et al. presented a coupled dynamic analysis of spar-type floating wind turbine and validated with results obtained from OC3 Hywind and obtained the tower base motions and platform motions for wind speed 3.7 m/s with 4 m wave height and 0 degrees heading angle [31]. Han et al. found the optimal spar substructure design for a 3 MW FOWT with the maximum postural stability in 6-DOF motions using a genetic algorithm with a neural network approximation [32]. Hegseth et al. presented a linearized aero-hydroservo-elastic floating wind turbine model to find out the optimal design solution using the gradient-based optimization for a 10 MW FOWT with a spar-type substructure [33]. Valk and Paul performed the coupled simulations of FOWT to derive proper design strategies according to the dynamics of substructures [34]. However, there is little research on the detailed structural modeling process and stress analysis of a spar-type substructure for a FOWT utilizing the coupled load analysis and the interface between the nonlinear time-domain multi-physics models (aero-hydro-servo-elastic) and three-dimensional finite element model. Furthermore, even though there was a study on the substructures for the Southwest offshore wind farm in Korea with a water depth under 33 m, few studies were published for the FOWT in the East Sea of Korea, where six GW floating offshore wind farms were planned [35].

PEER REVIEW
3 of 23 proper design strategies according to the dynamics of substructures [34]. However, there is little research on the detailed structural modeling process and stress analysis of a spartype substructure for a FOWT utilizing the coupled load analysis and the interface between the nonlinear time-domain multi-physics models (aero-hydro-servo-elastic) and three-dimensional finite element model. Furthermore, even though there was a study on the substructures for the Southwest offshore wind farm in Korea with a water depth under 33 m, few studies were published for the FOWT in the East Sea of Korea, where six GW floating offshore wind farms were planned [35].  In this work, the design process on the structural model and analysis of a spar-type substructure for a 5 MW FOWT specially designated to the East Sea in South Korea will be presented in detail with a fully coupled integrated load analysis and three-dimensional finite element model/analysis. FAST, a widely used integrated load analysis software developed by NREL, was coupled with in-house hydrodynamic code (UOU code) [36,37]. The environmental design loads will be calculated from the data recorded for three years at the Ulsan Marine buoy point according to the ABS and DNV standards [38,39]. The three-dimensional (3D) structural finite element (FE) model of a spar-type substructure incorporating the wind turbine tower and floating structure bolted joint was constructed under the external loads such as the structural loads due to the inertial acceleration, buoyance, and gravity, and the environmental loads due to the wind, wave, and current. The structural integrity of the spar-type substructure was investigated under extreme limitations based on the von Mises criteria.

Overall Key Specifications and Schematic Layout
The schematic layout of the wind turbine and a spar-type floating platform are shown in Figure 3. Table 1 lists the overall key specification of 5 MW FOWT, and Tables 2 and 3 lists the detailed properties of the baseline part of the 5 MW rotor nacelle assembly (RNA) and tower developed by Unison (www.unison.co.kr), and the characteristics of the structural specifications of the floating platform, respectively.

Overall Key Specifications and Schematic Layout
The schematic layout of the wind turbine and a spar-type floating platform are shown in Figure 3. Table 1 lists the overall key specification of 5 MW FOWT, and Tables  2 and 3 lists the detailed properties of the baseline part of the 5 MW rotor nacelle assembly (RNA) and tower developed by Unison (www.unison.co.kr), and the characteristics of the structural specifications of the floating platform, respectively.

Mooring System Specification
The mooring system was designed as the catenary mooring type to suit the depth of 150 m in the waters of the Korea East Sea gas field. The layout and specifications of the mooring system are shown in Figure 4 and Table 4. It was designed as a studless link chain, the length of the chain was 560 m, the diameter was 120 mm, and the dry weight per unit length was 288 kg/m. The drag anchor is located at 532.21 m from the center of the floater, and by installing two clamp weights, it is designed so that lift-up does not occur at the anchor point even if the touched down length is short [40].

Extreme Environmental Conditions at the East Sea
The 5 MW SPAR FOWT is planned to be installed in the East depth about 58 km from the Ulsan coastline in Korea. The wind a obtained from the data recorded for three (2016-2018) years at the n

Extreme Environmental Conditions at the East Sea
The 5 MW SPAR FOWT is planned to be installed in the East Sea of 150 m water depth about 58 km from the Ulsan coastline in Korea. The wind and wave data were obtained from the data recorded for three (2016-2018) years at the nearest Ulsan Marine buoy point. The 50 years return period extreme sea state was estimated using extreme statistical analysis [41]. In the extreme sea state, the 50 years return period wind speed was applied to 39.83 m/s referring to the IEC standard [42,43]. The extreme period of significant wave height was 11.12 m with a wave period is 14.17 s. With reference to the annual tidal report, the extreme current speed was applied at 1.63 m/s [44]. Figure 5 shows the wind rose diagram with different wind speed configurations and Table 5 summarizes the extreme environmental design conditions.     Figure 6 shows the structural modeling and analysis process of the substructure for FOWT design using a fully coupled integrated load analysis. Fully coupled load analysis and integrated modeling/design were performed using NREL FAST, UOU code, FEGate, and MSC Nastran. The numerical simulation analysis was carried out using FAST representative code to analyze floating offshore wind turbines. The FAST is open-source code developed by NREL. It is primarily used to perform complex aero-elastic analysis of three-bladed horizontal axis wind turbines (HAWTs), and the HydroDyn module was added to analyze floating offshore wind turbines [36]. In the FAST simulation, the hydrodynamic forces are calculated by adding the viscous drag of the Morison equation based on traditional potential theory. The volume and center of buoyancy under the waterline for the scaled floater were confirmed by 3D modeling, and the hydrostatic restoring coefficient was determined by the shape of the floater. The UOU in-house code solves the radiation problem and diffraction problem by using the 3D panel method for the interaction of surface waves with platform geometry through frequency domain analysis. The added mass, radiation damping, and wave excitation forces were obtained from the in-house code, and these values are used input data to the FAST fully coupled analysis of FOWT [45]. The numerical simulation of mooring lines was executed using the MoorDyn module. MoorDyn is based on a lumped-mass modeling approach that is able to capture mooring stiffness, inertia, and damping forces in the axial direction, weight and buoyancy effects, seabed contact forces, and hydrodynamic loads from mooring motion using Morison's equation [46].

Integrated Design and Analysis Platform
From the dynamic analysis in FAST, the following results were used for the structural analysis of the spar structure in MSC NASTRAN (FEGate); six degrees of freedom motions at COG (surge, sway, heave, roll, pitch, yaw). FEGate requires the period value as well as acceleration values directly calculated from the FAST model. The traditional and standard equations from DNVGL were used to derive the periods as mentioned in the above answer. The associated periods corresponding to the six-degrees of motion were calculated from the equation below [47].
The angular acceleration of roll motion shall be taken as Equation (1): where, a = acceleration parameter = 1.0 for extreme sea loads design load scenario The numerical simulation analysis was carried out using FAST representative code to analyze floating offshore wind turbines. The FAST is open-source code developed by NREL. It is primarily used to perform complex aero-elastic analysis of three-bladed horizontal axis wind turbines (HAWTs), and the HydroDyn module was added to analyze floating offshore wind turbines [36]. In the FAST simulation, the hydrodynamic forces are calculated by adding the viscous drag of the Morison equation based on traditional potential theory. The volume and center of buoyancy under the waterline for the scaled floater were confirmed by 3D modeling, and the hydrostatic restoring coefficient was determined by the shape of the floater. The UOU in-house code solves the radiation problem and diffraction problem by using the 3D panel method for the interaction of surface waves with platform geometry through frequency domain analysis. The added mass, radiation damping, and wave excitation forces were obtained from the in-house code, and these values are used input data to the FAST fully coupled analysis of FOWT [45]. The numerical simulation of mooring lines was executed using the MoorDyn module. MoorDyn is based on a lumped-mass modeling approach that is able to capture mooring stiffness, inertia, and damping forces in the axial direction, weight and buoyancy effects, seabed contact forces, and hydrodynamic loads from mooring motion using Morison's equation [46].
From the dynamic analysis in FAST, the following results were used for the structural analysis of the spar structure in MSC NASTRAN (FEGate); six degrees of freedom motions at COG (surge, sway, heave, roll, pitch, yaw). FEGate requires the period value as well as acceleration values directly calculated from the FAST model. The traditional and standard equations from DNVGL were used to derive the periods as mentioned in the above answer. The associated periods corresponding to the six-degrees of motion were calculated from the equation below [47].
The angular acceleration of roll motion shall be taken as Equation (1): where, a 0 = acceleration parameter f p = 1.0 for extreme sea loads design load scenario θ = roll angle, in deg T θ = roll period, in s Inertial acceleration and period information are used as input for the FEM analysis in MSC NASTRAN (FEGate). In other words, from the FAST simulation, the dynamic response result according to the environmental load of the time varying was derived. Of these, 12 extreme value conditions were extracted for the structural analysis conditions. We used inertial acceleration directly from FAST which was input information for the FEM analysis. As a conservative approach, we also applied the direction of the environmental condition such as wind, wave, and current in which the extreme value occurs was also considered.
In the structural analysis, 3D shell elements were used for the plates and reinforcements such as stiffeners and girders. From the structural analysis, the failure assessment was performed according to the von Mises stress criteria.

Dynamic Load Case (DLC)
DLC 6.1 was selected for the ultimate limit analysis of the FOWT under extreme environmental conditions [48]. Table 6 shows the summary of the simulation configuration for DLC 6.1. Dynamic simulations for leveraging structural analysis models are commonly used to calculate wind turbine loading effects. In these cases, the total duration of the loading data should be long enough to ensure statistical reliability of the estimate of the characteristic loading effect. In general, continuous 1 h periods are required for each mean, hub height wind speed, and sea condition considered in the simulation [43]. In this study, each load case consisted of three random seeds of 1 h per simulation to conservatively approach the spectral gap of the wave at low frequencies, which is the low natural frequency of the floating substructure. Moreover, a 3D Kaimal turbulence model with six turbulence fields across all simulations and the wind gradient value of 0.11 was used. Extreme sea state with irregular waves was defined using the Jonswap spectrum. The load safety factor of 1.35 was considered for the load calculation. According to the wind rose previously shown in Figure 5, the environmental loads were applied in three main directions (45 • , 135 • , and

3D Finite Element Modeling and Structural Analysis of a Spar-Type Substru
Based on the conceptual layout, the 3D finite element model of the s substructure was constructed with the aid of CATIA (CAD Modeler) and FEGa Pre/Post Processor) software and later numerically analyzed by MSC Na commercially available finite element analysis software [49][50][51]. All structural ele the substructure were checked for compliance with the requirements of equivale criteria in accordance with DNVGS-ST-0119 [24]. The individual design components and von Mises equivalent design stresses of the structure should greater than the design resistance considering the safety factors through linea analysis [52].

3D Finite Element Model
Finite element modeling was constructed as close as possible to the conceptu and basic specification of the spar-type substructure, and all structural componen floater such as the shell, decks, girders, and reinforced stiffeners are modeled elements. The mesh sizes of the rectangular and triangular shell elements are bo less than 500 mm × 500 mm. Among the upper part of the FOWT, the RNA com was modeled as the lumped mass element to the center of gravity of the RNA, tower component was modeled as shell elements for the wind load application. shows the 3D finite element model of a spar structure. This approach has been several studies available in the literature and is in accordance with the DNV-RP-C

3D Finite Element Modeling and Structural Analysis of a Spar-Type Substructure
Based on the conceptual layout, the 3D finite element model of the spar-type substructure was constructed with the aid of CATIA (CAD Modeler) and FEGate (FEM Pre/Post Processor) software and later numerically analyzed by MSC Nastran, a commercially available finite element analysis software [49][50][51]. All structural elements of the substructure were checked for compliance with the requirements of equivalent stress criteria in accordance with DNVGS-ST-0119 [24]. The individual design stress components and von Mises equivalent design stresses of the structure should not be greater than the design resistance considering the safety factors through linear elastic analysis [52].

3D Finite Element Model
Finite element modeling was constructed as close as possible to the conceptual layout and basic specification of the spar-type substructure, and all structural components of the floater such as the shell, decks, girders, and reinforced stiffeners are modeled as shell elements. The mesh sizes of the rectangular and triangular shell elements are both set to less than 500 mm × 500 mm. Among the upper part of the FOWT, the RNA component was modeled as the lumped mass element to the center of gravity of the RNA, and the tower component was modeled as shell elements for the wind load application. Figure 8 shows the 3D finite element model of a spar structure. This approach has been used in several studies available in the literature and is in accordance with the DNV-RP-C208 [53]. Most shell and reinforcement plates consisting of the spar st with the mild steel of grade A and the high tensile steel AH36/D at the high-stress region such as the mooring fairleads. The properties of plates considering the safety factor were listed in ABS MODU, the safety factor of 1.43 was used for the static load The bolted connection between the tower bottom flange and mounted on the spar substructure was also constructed in the F were modeled in three different ways to check the sensitiv depending on the element types. Figure 9 shows three different the bolted connection: RBE3 elements, the combination of RBE3 Most shell and reinforcement plates consisting of the spar structure were constructed with the mild steel of grade A and the high tensile steel AH36/DH36 was especially used at the high-stress region such as the mooring fairleads. The corresponding material properties of plates considering the safety factor were listed in Table 7. According to the ABS MODU, the safety factor of 1.43 was used for the static loading analysis [54]. The bolted connection between the tower bottom flange and the TP (transition piece) mounted on the spar substructure was also constructed in the FE model, where the bolts were modeled in three different ways to check the sensitivity of bolted connection depending on the element types. Figure 9 shows three different modeling approaches for the bolted connection: RBE3 elements, the combination of RBE3 and beam elements, and solid elements. The flange was also modeled as either a shell element or solid element. The high strength bolt with the grade of 10.9 was used according to ISO 898-1 and the corresponding material property is listed in Table 8 [55].  The three-dimensional (3D) structural finite element (FE) model also incorporate the three mooring lines with the fixed boundary conditions at the end of the mooring lines The basic shape of the mooring fairlead foundation was modeled and applied to the F analysis using MPC (multi-point constraint. The external loads such as the structural load due to the inertial acceleration, buoyance, and gravity, and the environmental loads du to the wind, wave, and current will be explained in the next section.

Structural Analysis Case
Based on the dynamic responses calculated from FAST coupled with UOU code, 1 cases with the maximum values were selected for the structural analysis of the spa substructure as listed in Table 9. Each analysis cases contain all the external loadings suc as dynamic inertia loads from DLC 6.1, gravity-induced loads due to structural weights buoyance, ballast, and environmental loads from wind, wave, and current. Table 9. Structural simulation cases.

Case No. Description LC01
Max. X-dir. moment (tower base) LC02 Max. Y-dir. moment (tower base) LC03 Max. Z-dir. moment (tower base) LC04 Max. X-dir. force (tower base) LC05 Max. Y-dir. force (tower base) LC06 Max. mooring tension  The three-dimensional (3D) structural finite element (FE) model also incorporated the three mooring lines with the fixed boundary conditions at the end of the mooring lines. The basic shape of the mooring fairlead foundation was modeled and applied to the FE analysis using MPC (multi-point constraint. The external loads such as the structural loads due to the inertial acceleration, buoyance, and gravity, and the environmental loads due to the wind, wave, and current will be explained in the next section.

Structural Analysis Case
Based on the dynamic responses calculated from FAST coupled with UOU code, 12 cases with the maximum values were selected for the structural analysis of the spar substructure as listed in Table 9. Each analysis cases contain all the external loadings such as dynamic inertia loads from DLC 6.1, gravity-induced loads due to structural weights, buoyance, ballast, and environmental loads from wind, wave, and current. Table 9. Structural simulation cases.

LC01
Max. X-dir. moment (tower base) LC02 Max. Y-dir. moment (tower base) LC03 Max. Z-dir. moment (tower base) LC04 Max. X-dir. force (tower base)  Figure 10 shows the typical dynamic response with six degrees of freedom (surge, sway, heave, roll, pitch, and yaw). Calculated from the fully coupled integrated load analysis.

LC08
Max. sway LC09 Max. heav LC10 Max. roll LC11 Max. pitch LC12 Max. yaw Figure 10 shows the typical dynamic response with sway, heave, roll, pitch, and yaw). Calculated from th analysis. A one-hour simulation for the LC06 case, for exam shown in Figure 11, all dynamic response results from listed in Table 10, which were then applied to the FE m converted inertial acceleration values based on the perio A one-hour simulation for the LC06 case, for example, is shown in Figure 11. As shown in Figure 11, all dynamic response results from the integrated load analysis are listed in Table 10, which were then applied to the FE model of the spar structure as the converted inertial acceleration values based on the periods.

Structural Loads
The structural mass information applied to the finite element model is listed in Table 11. The structure weight corresponding to 2316 tons was properly distributed to the entire elements through FE modeling and a buoyancy of 9338 tons is applied as a hydrostatic pressure load to the FE modeling. Moreover, the concrete ballasts were modeled as beam elements with masses and added to the center of gravity of the permanent ballast tank. Figure 12 shows the hydrostatic pressure as a buoyance loading of 9338.12 tons and pressure loading due to the water ballast loading of 3558.10 tons applied to the substructure.

Structural Loads
The structural mass information applied to the finite element model is listed in Table  11. The structure weight corresponding to 2316 tons was properly distributed to the entire elements through FE modeling and a buoyancy of 9338 tons is applied as a hydrostatic pressure load to the FE modeling. Moreover, the concrete ballasts were modeled as beam elements with masses and added to the center of gravity of the permanent ballast tank. Figure 12 shows the hydrostatic pressure as a buoyance loading of 9338.12 tons and pressure loading due to the water ballast loading of 3558.10 tons applied to the substructure.

Wind Force
The wind force was calculated from the Equation (2) according to the standards of ABS-MODU.
where, f = 0.611 V k = wind velocity (m/s) C h = height coefficient (according to th height, 1.48) C s = shape coefficeint (cylindrical shapes, 0.5) The design load is listed in Table 12. In the calculation of wind pressure (P), the shape and vertical height are to be subdivided approximately in accordance with the values of references. A total wind force of 27.77 tons is applied to the FE model, according to the shapes and vertical height of FOWT.

Wave Load
The wave load was calculated from the Equation (3) based on DNV-RP-H103 [57].
where, ρ w = density of sea water (1025 kg/m 3 ) g = gravity acceleration (9.81 m/s 2 ) H s = significant wave height (m) B = breath of towed object (m) The calculated design load was summarized in Table 13. A wave force of 159.41 tons was applied to the FE model at a determined angle notated in each load case.

Current Load
The current force was calculated from Equation (4) according to the ABS-MODU standards.
where, The drag coefficient is taken 0.62 as references recommended. The current velocity was calculated of average value as the vertical height of the floater. A current force of 23.366 tons is applied to the FE model; it would be drag force for the structure as listed in Table 14.  Figure 13 shows the visualization of the load distribution applied to the FE model of the spar structure from the environmental loads such as wind, wave, and current.

Failure Assessment
The structural strength of the spar-type substructure was numerically analyz considering all external loadings such as inertia due to dynamic motions, gravi forces due to weights, wind force, wave force, and current force under extreme cond in the East Sea in Korea. The linear static analyses of about 12 cases were performed MSC Nastran, a commercially available finite element analysis software, and calculated design stress components of the structure were investigated according von Mises criteria. Figures 14-16 show that the maximum equivalent stress of 218.08 MPa occur the mooring fairlead point from the analysis case 6, which was the reason to app high tensile steel AH36/DH36 grade specifically to the fairlead parts. In addition, structures can be seen where all stresses of shell element mesh of structure are less the allowable stress of the mild steel A grade. Because all the maximum equiv stresses (von Mises stresses) from 12 load cases are less than the allowable stress, it c

Failure Assessment
The structural strength of the spar-type substructure was numerically analyzed by considering all external loadings such as inertia due to dynamic motions, gravitation forces due to weights, wind force, wave force, and current force under extreme conditions in the East Sea in Korea. The linear static analyses of about 12 cases were performed with MSC Nastran, a commercially available finite element analysis software, and the calculated design stress components of the structure were investigated according to the von Mises criteria. Figures 14-16 show that the maximum equivalent stress of 218.08 MPa occurred at the mooring fairlead point from the analysis case 6, which was the reason to apply the high tensile steel AH36/DH36 grade specifically to the fairlead parts. In addition, other structures can be seen where all stresses of shell element mesh of structure are less than the allowable stress of the mild steel A grade. Because all the maximum equivalent stresses (von Mises stresses) from 12 load cases are less than the allowable stress, it can be addressed that the spar-type substructure for the 5 MW floating offshore wind turbine has enough  Table 15.

Stresses from the Bolted Joint Connection
Three types of bolt elements and two types of flange elements were studied for the bolted connection joints between TP and the upper part of the substructure, and it was found that the solid element applied to the flange was conservative in the analysis as listed in Table 16. Based on the investigation of bolt and shell element types, the solid elements were applied to bolted joint connections of a spar structure FE model. Figures 17 and 18 show the stress distribution of the bolted connection in the simulation case of LC06. Three types of bolt elements and two types of flange elements were studied for the bolted connection joints between TP and the upper part of the substructure, and it was found that the solid element applied to the flange was conservative in the analysis as listed in Table 16. Based on the investigation of bolt and shell element types, the solid elements were applied to bolted joint connections of a spar structure FE model. Figures 17 and 18 show the stress distribution of the bolted connection in the simulation case of LC06.   The results showed that the von Mises stresses of bolts on the 12 anal under the allowable stress (830 MPa) of the bolt as shown in Table 17.

Conclusions
In this paper, the finite element model of the spar-type substructu FOWT planned in the East Sea was constructed in detail for structural integ under extreme environmental conditions. The extreme environmental co sea with 150 m water depth about 58 km away from the coastline of U investigated. Based on the data recorded for three years (2016-2018) at the Marine buoy point, the 50 years return period extreme sea state was ca resulted in extreme wind load, wave load, and current load to be use coupled integrated load analysis with FAST, a widely used load ana developed by NREL, coupled with the in-house hydrodynamic code deve The results showed that the von Mises stresses of bolts on the 12 analysis cases were under the allowable stress (830 MPa) of the bolt as shown in Table 17.

Conclusions
In this paper, the finite element model of the spar-type substructure for a 5 MW FOWT planned in the East Sea was constructed in detail for structural integrity evaluation under extreme environmental conditions. The extreme environmental conditions in the sea with 150 m water depth about 58 km away from the coastline of Ulsan were also investigated. Based on the data recorded for three years (2016-2018) at the nearest Ulsan Marine buoy point, the 50 years return period extreme sea state was calculated which resulted in extreme wind load, wave load, and current load to be used for the fully coupled integrated load analysis with FAST, a widely used load analysis software developed by NREL, coupled with the in-house hydrodynamic code developed by UOU. From the integrated load analysis, the dynamic responses with six degrees of freedom motions of the floating offshore wind turbine were applied to the FE model of the spar-type substructure under three co-directional conditions (45 • , 135 • , and 315 • ) of wind and wave. The threedimensional (3D) structural finite element (FE) model incorporating the mooring lines and bolted joint connection was constructed in FEGate with the fixed boundary conditions at the end of the mooring lines and the external loads such as the structural loads due to the inertial acceleration, buoyancy, and gravity, and the environmental loads due to the wind, wave, and current. The three-dimensional FE analysis in MSC Nastran software showed that the designed spar-type substructure had enough strength to endure the extreme limitation in the East Sea based on the von Mises criteria. For future work, the fatigue life calculation and damage tolerance design using the current process will be executed with high fidelity. The performed structural modeling and analysis process based on the fully coupled integrated analysis will also be beneficial to the modeling and analysis of the other FOWT substructures, such as submersible type.

Conflicts of Interest:
The authors declare no conflict of interest.