Automatic FE modeler using stiffener-based mesh generation algorithm for ship structural analysis

Transcription

1 Marine Structures 21 (2008) Automatic FE modeler using stiffener-based mesh generation algorithm for ship structural analysis Beom-Seon Jang a,, Yong-Suk Suh a, Eun-Ki Kim b, Tae-Hee Lee b a Structure Research Part, Marine Research Institute, Samsung Heavy Industries, Geoje-si, Gyeongnam , Republic of Korea b Engineering Service Division, MSC.KOREA, Sungnam-si, Kyungki-do , Republic of Korea Received 31 March 2007; received in revised form 20 August 2007; accepted 20 August 2007 Abstract Shipbuilding industries have started to employ 3D CAD systems to integrate all design and production processes by achieving seamless data transfer and data sharing. The emerging 3D CAD system brings a considerable change in FE analysis field. The availability of 3D geometry increased the recognition of the need for developing automatic FE modeling system consequently. However, general automatic mesh algorithms developed by academic research field have a limitation. The difficulty in satisfying lots of line constraints and the absence of proper idealization of 3D geometry entities defined in CAD system hinders directly employing the general mesh algorithms. In this research, an automatic FE modeling system has been developed for cargo hold FE modeling and whole ship FE modeling. The basic concept of the algorithm is to decompose surfaces using stiffener lines into subregions and generate mesh using a rule established based on FE modeling practice of ship structure. Since the decomposed subregions take simple polygon, they can be easily transformed into elements by decomposing the polygon according to the rule defined considering the shape of the polygon and mesh seed on its perimeter. The algorithm is also designed to treat appropriate geometry idealizations for bracket-type surface and stiffener connections. The idealization process is also completely customized based on FE modeling practice. The validity of the developed system is verified through illustrative examples. r 2007 Elsevier Ltd. All rights reserved. Keywords: Automatic FE mesh generation; Stiffener-based mesh generation algorithm; Geometry idealization Corresponding author. Tel.: ; fax: addresses: beomseon.jang@sasmsung.com (B.-S. Jang), yongsuk.suh@samsung.com (Y.-S. Suh), ekkim@mscsoftware.co.kr (E.-K. Kim), thlee@mscsoftware.co.kr (T.-H. Lee) /$ - see front matter r 2007 Elsevier Ltd. All rights reserved. doi: /j.marstruc

2 B.-S. Jang et al. / Marine Structures 21 (2008) Introduction Ship design work includes a wide range of design works; hull design and steel outfitting, electric outfitting, machinery outfitting, production drawings and so on. These design works have been performed in different CAD systems and there have been serious troubles in transferring the model data from one CAD system to another. The integration into a single 3D CAD system requires exhaustive work and an investment of huge amount of money and time to cover the extensive design work. This has delayed the introduction of 3D CAD system into shipbuilding industries differently from any other engineering fields. The introduction of 3D CAD system is also expected to change the situation of FE analysis field. FE modeling takes an advantage of 3D geometry model by transferring it from 3D CAD system to FE preprocessor. Moreover, in FE modeling, there is a tendency of achieving a higher accuracy by reducing the mesh size, which eventually increases FE modeling time. On the contrary, rapid growth in computer performance has reduced the solving time, which accounts for a small portion of the FEM analysis time. This changing situation has encouraged to develop automatic FE modeling algorithm, which has emerged as an important issue in today s analysis engineering environment. Since long time, analysis engineers in shipbuilding industry have constructed FE model manually while referring to only printed drawings. At most, 2D drawing data from 2D CAD system is imported to FE preprocessor and referred in manual modeling after it is reassembled as a 3D model in these days. If this manual work is replaced with automatic process, analysis and design time can be drastically reduced. In addition, a shortened analysis time gives scope for a more innovative/superior design by making it earlier, to reflect analysis results on design amid a tight ship design schedule. Automatic FE modeling system for ship structural modeling needs a sufficient consideration of ship structure s characteristics. The development includes a new algorithm, named Stiffener-Based Mesh Generation. Its basic concept is that stiffener lines are used in decomposing surface into smaller polygon-type regions and the regions are divided into elements and smaller regions according to templates established by mesh generation practice of ship FE analysis fields. The algorithm is also designed to treat geometry idealization process which is completely tailored to the practice. The system can generate whole-ship coarse mesh model and cargo hold fine mesh model for tanker, container ship, and LNG carrier. This is expected to enhance the efficiency by drastically cutting down routine and simple FE meshing work. Meanwhile, due to the increasing request of ship owners and classification societies for direct FE analysis, almost the same structural analysis has been repeatedly performed for examining cargo hold strength or whole-ship global strength. This has induced great concern in developing user-friendly environ ment for typical FE analysis to guarantee consistent result and to shorten analysis time. Samsung Heavy Industries has developed integrated systems for cargo hold analysis and whole-ship analysis. The systems include all subsystems ranging from importing geometry model to generating a final report. Figs. 1 and 2 depict the organization of two systems.

3 296 B.-S. Jang et al. / Marine Structures 21 (2008) Fig. 1. Hold analysis integrated system (HAIN System). Fig. 2. Whole ship analysis integrated system (WAIN System). The developed automatic modeler plays a role of reducing total analysis time. The system includes the following items: Hold Analysis Integrated System (HAIN System) - Interface with CADRA/GS-CAD - Automatic FE modeling for cargo hold - Automatic load generation module - FE model and load check module - Automatic reporting system Whole Ship Analysis Integrated System (WAIN System) - Interface with GS-CAD - Seakeeping analysis - Design wave decision module - Automatic FE modeling for whole ship - Load generation module from seakeeping results - FE model and load check system.

4 The systems begin with an interface with CAD systems. Geometry data are transferred through typical neutral format, IGES format from 2D CAD (CADRA) and ACIS format form 3D CAD (GS-CAD). The interface with 3D CAD system includes property data transfer of the geometry model. The load generation module in HAIN system automatically generates internal or external load generation for tanker and container ship in accordance with classification rules. WAIN system takes various types of actual loads into account to realize vessel s real condition at instantaneous moment in sailing. The loads include external wave pressure, internal tank pressure, inertial force, etc. They are calculated by capturing an instantaneous motion of a vessel from linear 3D seakeeping analysis results. FE model check and load check system can reduce unwanted repetitive work caused by human error that is easily committed but difficult to find out. This module is also indispensable for confirming automatically generated FE mesh and loads. Reporting system assists users in making a typical report only by following a procedure guided by a GUI. Especially, this system automatically generates all figures and stress summary tables required to be contained in a report by operating on pre/post processor system and accessing FE analysis results. This paper will focus on the automatic modeler and describe its feature suitable to FE modeling of ship structure. In Section 2, related works regarding automatic mesh generation algorithm is introduced and the main characteristics of the proposed method are explained in Section 3. Sections 4 and 5 describe overall procedures and main features of automatic modeler for cargo hold model and whole ship model, respectively. Conclusion is laid in Section Related works B.-S. Jang et al. / Marine Structures 21 (2008) To develop general automatic mesh generation algorithm many efforts have been made in academic fields and also in practical engineering fields. Most of academic researches focus on the generation of quadrilateral mesh for an arbitrary geometry with closed boundary and line constraints. Quadrilateral mesh generators can be broadly classified into two main categories: direct and indirect approaches, according to the method employed to generate the quadrilateral elements [1]. The direct approach places the quadrilaterals on the domain directly without triangulation. It is divided into two types. First, geometry decomposition approach divides a domain into simpler, convex, or mappable regions. The geometry decomposition approach is achieved by recursive decomposition algorithm [2,3], quad-tree decomposition technique [4], medial axis method [5], and convex polygon decomposition method [6]. Second, advancing front method to form elements is known as Paving, proposed by Blacker and Stephenson [7]. These methods are not suitable for generating quadrilateral with line constraints. The direct approach can generally produce better quality meshes than the indirect approach. However, the algorithms of the direct approach are difficult to handle and implement, in general. The indirect approach generates quadrilaterals by combining or splitting the background triangle mesh. The Q-Morph algorithm, which was recently introduced by Owen et al. [8], utilizes an advancing front approach to combine triangles into

5 298 B.-S. Jang et al. / Marine Structures 21 (2008) Fig. 3. Illustrating example of the algorithm of Lee et al. [9]. quadrilaterals. This algorithm can generate better quality mesh than existing algorithms. Q-Morph algorithm can generate a quadrilateral mesh with closed boundary only. Lee et al. proposed an algorithm for generating an automatic 2D quadrilateral mesh with line constraints by appending an algorithm for handling line constraints to the Q-Morph algorithm [9]. Fig. 3 shows an example of the method to a model with one hole and six line constraints. Fig. 3(a) and (b) shows the front proceeding while forming quadrilaterals. Fig. 3(c) shows the quadrilateral mesh after generation is completed and Fig. 3(d) shows the shape of the quadrilateral mesh after smoothing. In the shipbuilding industry, Kim et al. [10] proposed an algorithm to generate mesh for shell and inner hull parts of whole ship model using hull lines and compartment information in the initial design stage when 3D geometry model is not available.

6 3. Stiffener-based mesh generation algorithm This section will give a description about stiffener-based mesh generation algorithm proposed in this paper. Since this approach is based on the features of ship structure, it is designed to be suitable for FE modeling of cargo hold and whole-ship analysis Stiffener-based surface decomposition B.-S. Jang et al. / Marine Structures 21 (2008) Ship structures have specific features that stiffeners are attached on a plate for its reinforcement. Fig. 4 depicts one of web section structure of a tanker. Stiffeners attached on a plate to resist bending moment raise bending stiffness by increasing section modulus. Others are attached to prevent buckling of the plate. The mesh size of a cargo hold FE model is about stiffener spacing, that is, no node is created between two stiffeners. In the existing mesh generation algorithms such as Q-Morph, a stiffener on a plate is regarded as a line constraint to be imposed on mesh and its straight line should be kept after mesh is created on the plate. However, stiffener line constraints are too tight for Q-Morph to meet, considering the mesh size of stiffener spacing in cargo hold model. Since almost all elements share nodes on the line constraints, all elements are affected by two or more line constraints. The Q-Morph algorithm may be more appropriate for constructing fine mesh model or fatigue mesh model where its mesh size is sufficiently small compared to the area surrounded by stiffener lines. Since line constraints influence only the surrounding elements, they are not crucial in creating elements in those model. In the cargo hold modeling, it is more reasonable to regard stiffeners as lines to decompose a surface into subregions. A stiffener is always attached on a plate and its end is connected to other stiffeners or another plate in a different plane which is also a line constraint to be maintained. Due to this feature, a region decomposed by the stiffener lines forms a closed polygon. Only properly splitting the polygon into quadrilateral elements or triangular elements can generate mesh of sufficiently good quality. This is the basic idea of the proposed approach. This approach is expected to be more effective than applying the Q-Morph algorithm imposing many line constraints. Fig. 4. Typical web section structure of a tanker: (a) geometry model of which lines represent stiffeners and (b) corresponding web section FE model.

7 300 B.-S. Jang et al. / Marine Structures 21 (2008) Priority- and template-based mesh generation Decomposed regions of polygon shape should be split recursively until mesh generation is completed for structural analysis. The proposed approach set up the priority order and templates in splitting the decomposed region according to the shape of the region and attached mesh seeds. A surface is divided into smaller regions by stiffener lines and all regions are ranked in the number of nodes on the perimeter of the divided region. The region having the most nodes is divided into subregions again according to the predefined scheme and a region of top priority is decided again. The priority order and templates are established based on engineer s experience in FE modeling for ship structure. The basic concept of the priority order is that mesh generation begins with the most obvious element creation in which there is no difference among different engineers for maximizing the use of quadrilateral elements instead of triangular elements. A template to create a quadrilateral element of square shape is given high priority. This process is to be described in detail in Section 4.7 with illustrative examples Geometry idealization Geometry model needs an idealization process to guarantee good mesh quality. Since the mesh quality is closely related with structural analysis results, structural engineer s experience and know-how should be incorporated into the idealization process. One of objects to be idealized is the adjustment of stiffener line ends. An end point of a stiffener line frequently does not coincide with other stiffener ends on the same plane or stiffener lines on different planes like joints in the rounded rectangular in Fig. 5(a). If the stiffener lines are kept as they are during the mesh generation, triangular elements of sharp angle are unavoidable where two stiffener end points do not match with each other exactly as Fig. 5(b). Fig. 5(c) shows mesh generated after an appropriate adjustment of stiffener ends, which leads to even stress distribution in analysis results. Stiffener ends placed closely are needed to be merged to minimize the use of triangular elements. Bracket toe end composed of complex edges circled in Fig. 6(a) is another object of the idealization. Without simplifying the toe end shape, the mesh might be like that in Fig. 6(b). Small triangular elements at the end can lead to excessive stress concentration at the point. Similarly by proper simplification is needed to get uniform mesh of good quality Fig. 5. (a) Stiffener arrangement on a web section; (b) mesh generated without an idealization of the arrangement; (c) mesh generated with a proper idealization.

8 B.-S. Jang et al. / Marine Structures 21 (2008) Fig. 6. (a) Shape of bracket toe on a web section; (b) mesh generated without an idealization of the shape; (c) mesh generated with a proper idealization. as marked by the circle in Fig. 6(c). The target area of the idealization or simplification is the area which should be carefully estimated because of high stress concentration or buckling problem. Therefore, expected analysis results should be reflected on how to idealize the area in the algorithm. Without a proper simplification, mesh quality could be too low to be used without modification and manual modification might deteriorate its time saving effect considerably. 4. Automatic FE modeler for cargo hold model 4.1. Overall procedure The automatic system is divided into two main parts: preprocessing and main mesh generation process. Overall procedures are summarized in Fig. 7. Preprocessing begins with grouping a given geometry model imported from 3D CAD system into MSC.PATRAN. For a selected group, global mesh seeds are generated and intersecting lines with other surfaces in different groups are created. Geometry constructed in CAD system needs to be reformed by cutting with intersection lines and merging surfaces separated by other lines such as seam lines or block butt lines. It is enabled by disassembling surfaces into a set of edges, breaking them by intersection lines and searching new closed loops by tracing decomposed lines. The reconstructed surfaces are decomposed by internal stiffener lines again with adjusting bracket toe end and stiffener end points. The next step is to form closed polygons and assign mesh seeds to corresponding edges of the polygons. The polygons are recursively divided in accordance with a predefined scheme until all divided polygons have only three or four edges and nodes. The process ends with transforming the decomposed polygons to shell elements and mapping properties of the original geometry to the generated mesh. Among the above-mentioned processes, the following steps are explained in detail with illustrating examples: - automatic grouping; - global mesh seeds generation;

9 302 B.-S. Jang et al. / Marine Structures 21 (2008) Preprocessing of geometry Automatic grouping Generate intersection lines with other surfaces on different planes. Generate global mesh seeds. Divide surface edge lines and intersection lines at their intersection points. Search closed loops and redefine surfaces and stiffener lines. Mesh generation with idealization Divide edge lines and stiffener lines at their intersection points. Adjust bracket toe end shape and identify a point for a stiffener end to be shifted to. Search closed polygons along with global mesh seeds on their perimeter. Recursive mesh generation for the polygons Beam mesh generation on stiffener lines. Move stiffener end nodes to the identified points. Post processing Property mapping from original geometry to generated mesh Fig. 7. Overall process of automatic mesh generation. - reconstruction of surfaces and curves; - simplification of bracket toe end and stiffener connection points; - construction of a set of polygons; - recursive mesh generation.

10 B.-S. Jang et al. / Marine Structures 21 (2008) The global coordinate system is set according to the following system: The x-axis is in the longitudinal direction, positive towards forward. The y-axis is in the transverse direction, positive towards port. The z-axis is in the vertical direction, positive upwards Automatic grouping This process is to automatically group geometry model which consists of surfaces and curves to represent steel plates and stiffeners, respectively, in MSC.PATRAN. The process is summarized in Fig. 8. All surfaces are divided into four groups based on their normal vector. Surfaces on xy-plane, xz-plane, or yz-plane are grouped into a plan group, an elevation, a section group. Surfaces representing side shell or bottom shell are Automatic grouping process Check the normal vector of every surface. Collect surfaces on xy-plane, xz-plane and yz-plane to a plan group, an elevation group and a section group, respectively Check z, y, and x coordinate value of surfaces in the plan, the elevation and the section group, respectively. Classify surfaces according to their coordinate value. Name each group ship deck_oooo, ship_elev_oooo or ship_sect_oooo. Collect slanted surfaces and select surfaces to represent hopper plates in tanker. Check the directional vector and the location of every stiffener line or check the plane a curved line is on. Allocate stiffener lines to one of the existing groups Fig. 8. Automatic grouping process.

11 304 B.-S. Jang et al. / Marine Structures 21 (2008) distinguished by their outermost coordinate values, that is, the largest and the smallest y-coordinate value or the smallest z-coordinate value. Fig. 9 shows an example that a geometry model for midship cargo hold part is divided into four groups. Surfaces in a group are grouped by their coordinate values again. Surfaces in the plan group, the elevation group, and the section group are distinguished by their z-coordinate, y-coordinate, and x-coordinate values, respectively. For each group, a proper name is given. For example, a name of Ship_Deck_02490 is given to the group including surfaces placed on xy-plane of which z-coordinate level is 2490 mm from the bottom line. Hopper plates of tanker modeled as slanted surfaces are recognized by their normal vector and their y and z coordinate values. Every curve representing stiffener line is allocated to one of the existing groups including a surface on which the stiffener line is placed. Its directional vector and its location information are utilized. For example, a stiffener line of vector /100S can be added to one of the existing plan groups if its z-coordinate value coincides with the z-coordinate value of a plan group and its y-coordinate value is between the transverse range of the group. Otherwise, if its y-coordinate value coincides with an elevation group and z-coordinate value is between the vertical range of the group, it will be added to the elevation group. In a similar way, stiffener lines on yz-plane groups can be classified. Curved lines can be grouped by checking the plane on which it is. From the group information, a variety of information about structure can be obtained, for example, which group represents longitudinal bulkhead, upper deck or transverse bulkhead. Such information can be utilized for generating mesh seeds and intersection lines between surfaces in different groups. Fig. 9. Grouping all geometry into four groups.

12 4.3. Global mesh seed generation B.-S. Jang et al. / Marine Structures 21 (2008) Global mesh seeds are generated for plan groups and longitudinal elevation groups. For a plan group, mesh seeds are generated in longitudinal and transverse directions. An elevation group can share the longitudinal mesh seeds and needs only mesh seeds in vertical direction. A section group can share existing nodes in plan and elevation groups. Mesh seed generation on plan groups Obtain a set of transverse coordinate values referring to longitudinal stiffener lines on upper deck. Create mesh seeds on plan groups along lines intersecting with section groups. Generate three seeds between web sections along lines intersecting with elevation groups. In case of stringer plan group, get stiffener end points on brackets reaching longitudinal BHDs Redistribute the uniform longitudinal seeds considering the stiffener end points. Generate points at the intersection of free edges of surfaces which belong to section groups. for elevation groups Share the longitudinal seeds on plan group by collecting seeds of the same y-coordinate values as each elevation group. Obtain a set of z-coordinate values of mesh seeds referring to longitudinal stiffeners on side longi. BHD Generate vertical mesh seeds along lines intersecting with section groups for section groups Share all mesh seeds on plan groups by collecting seeds of the same x-coordinate values as each section group. Share vertical mesh seeds on elevation groups by collecting seeds of the same x-coordinate values as each section group. Fig. 10. Global mesh seed generation procedure.

13 306 B.-S. Jang et al. / Marine Structures 21 (2008) This seed information plays a role of supplementing the required information for splitting regions surrounded by stiffener lines into smaller polygons. It also assists the geometry idealization of bracket toe end or stiffener end points. Overall procedure is summarized in Fig. 10. Basically, in longitudinal direction, three mesh seeds are distributed between two adjacent web sections. That is, basic mesh size in longitudinal direction is one-fourth of web section spacing. However, stiffener end points on a bracket in stringer should be taken into account in generating mesh seeds as shown in Fig. 11. Since free-edge part of the bracket and toe-end part are weak against plate buckling, it is preferred to maintain stiffener lines on the bracket and avoid triangular elements as much as possible around the bracket toe. This enables accurate panel buckling check by forming correct buckling panel shape and ensures exact stress value. In transverse direction for a plan group, y-coordinate values of global mesh seeds are obtained from those of longitudinal stiffeners on upper deck. Mesh seeds on a plan group are created along intersection lines with section groups. In addition to the uniformly distributed mesh seeds in transverse direction, there are additional mesh seeds to be created. Mesh generation is done in the order of plan groups, elevation groups and section groups; therefore, nodes to be created in the mesh generation of section groups should be incorporated into the preceded mesh generation of plan groups in advance. For this purpose, mesh seeds are also created at the intersection points between deck plan surfaces and free edge of surfaces in section groups because the free edge should be maintained straight as it is during the mesh generation of the surface. Fig. 12 depicts an example of global mesh seed generation for a plan group a stringer group. The z-coordinate values of vertical directional mesh seeds for an elevation group are obtained from longitudinal stiffeners on side longitudinal bulkhead and distributed along the intersection lines with all section groups. For a section group, mesh seeds in other groups can be shared by adding all mesh seeds of which x-coordinate value is the same as the section group. Fig. 11. Global mesh seed generation in longitudinal direction for a plan group considering the stiffener lines on bracket in stringer.

14 B.-S. Jang et al. / Marine Structures 21 (2008) Fig. 12. An example of global mesh seed generation for a plan group (stringer) Reconstruction of surfaces and curves Surfaces arbitrarily created in 3D CAD system should be reconstructed considering the relations with other intersecting surfaces. An intersection line with another surface on different plane is also one of line constraints to be met in mesh generation algorithm. This system enables the intersection line constraints to be satisfied by replacing all surface boundaries with intersection lines or free-edge lines. That is, a surface which an intersection line cut across should be split into two surfaces. Two surfaces separated at a line except the intersection line should be merged, that is, surfaces split at a seam line or a block butt line should be combined to prevent nodes from being created at the seam line a seam line is a welding line created when connecting two steel plates of different thickness and usually neglected in FE modeling. Even if the reconstruction process is made for satisfying restrictions in mesh generation, the original surface information is maintained internally to transfer property information to mesh to be generated on the reconstructed geometry at the last stage. This process is summarized in Fig. 13. The detailed explanation is laid step by step as follows with an illustrating example of typical web section of tanker shown in Fig. 14: Step 1: Preprocessing of surface data. A surface is redefined as a collection of surface edges and vertexes. A curved edge is represented as a set of 20 short straight lines for an easy manipulation. The relationship between edges and vertexes are also stored by referring to each other. While redefining surface data, false surfaces are to be deleted, for example, a surface whose number of edges is below three, i.e., its area is zero. Two vertexes of a surface within given tolerance are merged. A duplicate surface is detected by comparing all vertexes of two surfaces and one of them is removed. Step 2: Group intersection lines and edge lines into a set. Intersection lines and edge lines are collected into a set but distinguished internally. Fig. 14(a) shows an original configuration of a typical web section of tanker. Dotted thick lines represent interaction lines with surfaces in other groups and solid thin lines

15 308 B.-S. Jang et al. / Marine Structures 21 (2008) Reconstruction of surfaces and curves Redefine surface data. Group intersection lines and edge lines to a set. Divide all lines in the set at their intersection points. Classify intersection lines into shared edges and free edges. Delete divided unnecessary lines. Delete overlapping edges and edges shared by two surfaces. From every vertex, search all closed loops by tracing a line of the smallest angle. Remove duplicate loops. Remove incorrect loops. Merge straight edges Redefine surfaces in a group Cut stiffener lines with loop edges and reassign to a surface to be included. END Fig. 13. Surface and curve reconstruction process. represent surface edge lines or stiffener lines on plate. Fig. 14(b) shows only surface edge lines and intersection lines along with vertexes of surface. Step 3: Divide all lines in the set at their intersection points. For every two lines in the set, their intersection is checked and divided at the intersection point. Fig. 14(c) illustrates the status of lines after this step. Step 4: Classify intersection lines shared edges and free edges.

16 B.-S. Jang et al. / Marine Structures 21 (2008) Fig. 14. An illustrative example of the reconstruction of surfaces and curves: (a) original geometry and intersection lines with other groups; (b) intersection lines and edge lines at Step 2; (c) lines cut at their intersection points at Step 3; (d) after unnecessary intersection lines are removed and shared edges are removed at Steps 5 and 6; (e) all loops found at Step 7; (f) Merged straight edges at Step 10; (g) reconstructed curves at Step 12. For each intersection line, overlapping surface edges are counted and the number is assigned to the intersection line. The number of overlapping edges indicates the number of surfaces sharing the intersection line. If the overlapping surface is one, the intersection line is classified to a free edge and if two or more, a shared edge. If there is no overlapping edge with an intersection line, the intersection line is used for breaking a

17 310 B.-S. Jang et al. / Marine Structures 21 (2008) surface. Therefore, it can be regarded as a new edge to be shared by the two broken surfaces. Eventually, all intersection lines can be classified into shared edge and free edge. The information is to be used for judging whether a closed loop to be found in the next step is correct or not. Step 5: Delete divided unnecessary lines. If an intersection line satisfies one of the following conditions, it remains. Otherwise, it is removed: - Its center point is inside of one of original surfaces or perimeter. - There exists an edge line exactly overlapping with it. An intersection line which does not satisfy any of the above conditions is one placed outside of all surfaces. It should be removed from the set. Except those intersection lines, intersection lines smaller than narrow tolerance or duplicate intersection lines are basically removed. Eventually, only edge lines or intersection lines to form new surfaces are left in the set. In the illustrating example, four intersection lines are removed as shown in Fig. 14(c) and (d). Step 6: Delete overlapping edges and edges shared by two surfaces. First, delete edges overlapping the intersection lines since those edges are to be replaced by newly defined intersection line. Next, among the remaining edges, an edge shared by two surfaces that does not duplicate any intersection line is also removed at this step. Such edges are seam lines to distinguish two plates of different thickness. It is generally neglected to avoid elements smaller than basic mesh size. Instead, to compensate the loss of property information, average thickness of two plates is assigned to elements on the seam line at the property mapping stage. It is a common recommendation of classification regulation regarding FE modeling. Eventually, only free surface edges and intersection lines shared by two surfaces are left in the set. In Fig. 14(b), two lines in the circles are removed and other shared edges are replaced by intersection lines. Step 7: From every vertex, search all closed loops by tracing a line of the smallest angle. This step begins with collecting all lines connected to a vertex to a linked list. This is for accelerating loop searching process. Next, for every vertex, search all closed loops staring from all edge lines connected to the vertex one by one. A closed loop can be found by tracing a line of the smallest angle at the next vertex until returning to the Fig. 15. An illustrative example of loop searching process.

18 B.-S. Jang et al. / Marine Structures 21 (2008) starting vertex. For a clear understating, another example is taken shown in Fig. 15. Four loops to define four surfaces marked shaded can be detected. Edges of e7 and e15 are classified as shared edges and other edges as free edges including e10 and e9 (here, e10 and e9 are assumed free edges). Table 1 summarizes all loops that can be found at every vertex. Step 8: Remove duplicate loops. Since all loops starting from at all vertexes are found out, it is needed to remove duplicate loops. In the example of Fig. 15, total 12 loops are to be deleted as identified in Table 1. Table 1 All closed loops that can be searched for an example of Fig. 14 Stating point ID Path Type V1 1 V14V24V54V44V1 Selected 2 V14V44V74V104V114V124V94V64V34V24V1 Incorrect loop V2 3 V24V34V64V54V2 Selected 4 V24V54V44V14V2 Same as no. 1 5 V24V14V44V74V104V114V124V94V64V34V2 Incorrect loop V3 6 V34V64V54V24V3 Same as no. 3 7 V34V24V14V44V74V104V114V124V94V64V3 Incorrect loop V4 8 V44V14V24V54V4 Same as no. 1 9 V44V54V64V94V84V74V4 Incorrect loop 10 V44V74V104V114V124V94V64V34V24V14V4 Incorrect loop V5 11 V54V44V14V24V5 Same as no V54V24V34V64V5 Same as no V54V64V94V84V74V44V5 Incorrect loop V6 14 V64V54V24V34V6 Same as no V64V94V84V74V44V54V6 Incorrect loop 16 V64V34V24V14V44V74V104V114V124V94V6 Incorrect loop V7 17 V74V84V114V104V7 Selected 18 V74V44V54V64V94V84V7 Incorrect loop 19 V74V104V114V124V94V64V34V24V14V44V7 Incorrect loop V8 20 V84V94V124V114V8 Selected 21 V84V114V104 V74V8 Same as no V84V74V44V54V64V94V8 Incorrect loop V9 23 V94V124V114V84V9 Same as no V94V84V74V44V54V64V9 Incorrect loop 25 V94V64V34V24V14V44V74V104V114V124V9 Incorrect loop V10 26 V104V74V84V114V10 Same as no V104V114V124V94V64V34V24V14V44V74V10 Incorrect loop V11 28 V114V84V94V124V11 Same as no V114V104V74V84V11 Same as no V114V124V94V64V34V24V14V44V74V104V11 Incorrect loop V12 31 V124V114V84V94V12 Same as no V124V94V64V34V24V14V44V74V104V114V12 Incorrect loop

19 312 B.-S. Jang et al. / Marine Structures 21 (2008) Step 9: Remove incorrect loops. A loop that meets one of the following conditions is regarded as a false loop and to be removed: - A loop that consists of only free edges without any shared edge. - A loop that has any intersection between its own lines in the middle of the loop. - A loop whose area is zero. In Fig. 15, two loops (V44V54V64V94V84V74V4 and V14V44V74V104 V114V124V94V64V34V24V1) are judged to be incorrect loop since they consist of only free edges. One is internal hole and the other is outer perimeter. In the example of Fig. 14, total 13 loops are left after removing duplicate loops as Fig. 14(e) and nos. 1, 2 and 13 should be deleted since they are judged false loops according to the rule defined above. Step 10: Merge straight edges. Fig. 14(f) depicts the status after some straight edges are merged. Step 11: Redefine surfaces in a group. New surfaces are defined using the lines and vertexes forming the final closed loops. Step 12: Cut stiffener lines by loop edges and reassign to included surface. Stiffener lines should also be cut by the intersection lines and two straight lines broken at the seam line should be merged into one line. Reconstructed lines are associated with a surface on which they are laid. Fig. 14(g) represents surface boundaries after the reconstruction process is completed. The surfaces are virtually drawn for an easy understanding and actually expressed as a loop defined with a collection of lines and vertexes internally Split edge lines and stiffener lines with idealization process This stage focuses on properly simplifying geometric details after breaking the reconstructed surfaces to pieces of lines. The edge lines and stiffener lines on the surface are cut at their intersection points. A curved edge line is also broken to several straight lines considering global mesh size and its curvature. Some idealization processes are needed for bracket toe end and stiffener end points. Those processes are made before or after the cutting process depending on its feature. These processes lead to more use of quadrilateral elements of uniform mesh size. The two main processes are to be introduced Bracket toe end Bracket toe of tanker web section or stringer always does not match stiffener lines of the plate whose toe end lands on vertically. It needs to be extended or cut out in the FE model whose mesh size is about the longitudinal stiffener spacing. Fig. 16 illustrates two examples of adjusting the bracket toe end of a tanker web section. If the extruded length over the closest global mesh seed on the base line is over half mesh size, it is extended to the next mesh seed. Otherwise, it is cut out at the closest mesh seed by a line normal to the base line. The global mesh seeds indicate longitudinal stiffener lines on longitudinal bulkhead or inner bottom plate. This modification is made after the cutting process in which all edge lines and stiffener lines are divided at their intersection points.

20 B.-S. Jang et al. / Marine Structures 21 (2008) Fig. 16. Two examples of the idealization of bracket toe ends: (a) an extending case and (b) a cutting out case (here, LS: longitudinal stiffener spacing). Fig. 17. An example of the idealization of stiffener end points: (a) original stiffener arrangement; (b) adjusted stiffener lines prior to mesh generation for type B; (c) mesh generation result; (d) adjusted mesh for type A.

21 314 B.-S. Jang et al. / Marine Structures 21 (2008) Stiffener end points The treatment of stiffener end point is strongly related to a panel surrounded by stiffener lines. The basic principle is to minimize the change of the panel shape and area since it can affect buckling check result. The process can be divided into two types. One type is to shift stiffener end point directly if the deviation from global mesh seed or another stiffener end point is sufficiently small. Even if all nodes on the stiffener line are to be slightly shifted after mesh generation is made for the adjusted line, the change in overall panel shape is negligible. The adjustment is made prior to the cutting process. It is illustrated in Fig. 17 as marked Type A. The other case is that the deviation is not negligible and if the end point is shifted as Type A, the original panel shape can be considerably distorted. The nodes on the middle of a stiffener line are kept at their original locations and only the node at the stiffener end point is shifted to the nearest mesh seed or other stiffener end point. This can minimize the change in the panel area. This process is enabled by shifting a node only after mesh is generated on the surface. For the shift of the node, it needs to identify which point a stiffener end point is shifted to before generating mesh on the surface. After mesh is generated, the node corresponding to the stiffener end point is shifted to the identified point. The process is marked as Type B in Fig. 17. The rule of the shift of stiffener end point is as follows: - If a stiffener line ends near a global mesh seed, it is bent. - If two stiffener lines meet at adjacent location, long stiffener line is maintained and short line is bent like Fig. 18(a). - If a vertical stiffener line on web section does not coincide with the horizontal stiffener line on deck plan (side stringer), vertical stiffener is bent as Fig. 18(b). Eventually, a reconstructed surface with stiffener lines is disassembled to a set of lines and connecting points. The next step is to construct closed loops forming the divided lines Construct polygons for mesh generation Once edge lines and stiffener lines are split, the decomposed regions take the shape of polygon which can be regarded as an elementary shape of element. Internally, a new Fig. 18. The shift of stiffener ends for idealized FE model: (a) stiffener end part is bent to longer stiffener end and (b) vertical stiffener on web section is bent.

22 B.-S. Jang et al. / Marine Structures 21 (2008) definition of the polygon is required. The polygon can be defined by surrounding lines and points between the lines. The definition is enabled by searching a closed loop in the similar manner with the surface reconstruction process described in Section 4.4. The process starts from a corner point having only two connected lines. The process is summarized in Fig. 19. Two loops are searched: one by tracing lines of the smallest angle and one by lines of the largest angle. For each of the found loops, its correctness is examined according to the rule described in Section 4.4. Fig. 20 illustrates an example is which a long loop is a wrong one, i.e. a perimeter of an empty hole since they consist of only free edges. Once a polygon is found out, free edges of the polygon are removed from the original set of lines as illustrated by Fig. 21. This is repeated until the line set becomes empty. START Select a group containing a set of lines and a set of nodes Select a node shared by only two lines. Search a closed loop by tracing linked lines of the smallest angle Search a closed loop by tracing linked lines of the largest angle Select a correct loop of the two loops Remove free edges of the found loop from the set of lines Remove nodes in the middle of the free edges from the set of nodes Is the set of lines empty? No END Yes Fig. 19. The procedure of searching closed polygons.

23 316 B.-S. Jang et al. / Marine Structures 21 (2008) Fig. 20. An illustrative example of searching polygons. Fig. 21. An illustrative example of the process to remove free edges of found polygons Recursive mesh generation for the polygons The next step is to generate mesh from the polygons included in a reconstructed surface. A polygon having more nodes than four nodes should be decomposed. The decomposition should be repeated until all polygons are divided into sub-polygons having three or four

24 B.-S. Jang et al. / Marine Structures 21 (2008) nodes which can be directly transformed to a triangular element or a quadrilateral element. The procedure is explained in Fig. 22. The decomposition process begins with a polygon having the most nodes. Such a polygon can lead to the largest effects on the total polygon set and can accelerate the division most. The selected polygon is divided into two new closed polygons by adding a new edge. The divided polygons substitute for the previous polygon and adjoined polygons are updated. This procedure is repeated by restarting a selection of a polygon having the most nodes again. The decomposition scheme and priority are established to follow FE modeling practice of ship structure. They are summarized as a set of templates as listed in Table 2. The concept of the priority order is that a division to create a square-shaped quadrilateral element in self-evident way should be preceded. If the polygon has a rectangular shaped corner with mesh seeds, the decomposition of the part is to be done first. As adding a new node or an edge, adjoined polygons can change to a form that matches with one of templates of high priorities. Eventually, most of decompositions can be done in a definite way. For example, a node newly created according to no. 2 template can change a polygon bordering below into a form that corresponds to no. 2 or no. 1 template. The decomposition according no. 3 template can create two polygons taking the shape of no. 7 template. Mesh results are not so sensitive to a slight change in the priority order; however, the approach to decompose from more obvious part is definitely effective to good mesh quality. This can lead to maximizing the use of square-shaped quadrilateral elements instead of triangular elements. Fig. 23 shows a mesh generation example of a bracket on which many buckling stiffeners are attached. Some mesh seeds are on the perimeter of the bracket, but there are few on Recursive mesh generation for the regions Select a polygon having the most nodes on its edges Divide the polygon according to the priority defined in mesh template Update total polygon data set. Do all l polygon shave 4 or 3 edges? No Yes Create quad or tri elements. END Fig. 22. Overall procedure of mesh generation for split lines.

25 318 B.-S. Jang et al. / Marine Structures 21 (2008) Table 2 Mesh generation templates and the priority order Priority Shape of polygon Mesh generation 1 Rectangular corner with two opposite nodes 2 Rectangular corner with one node on one edge 3 L-type corner 4 Rectangular corner with no node 5 Triangular corner with two nodes 6 Pentagon 7 Rectangular corner and triangular corner Fig. 23. An illustrative example of recursive mesh generation for decomposed polygons.

26 inside stiffener lines except the crossing points between stiffener lines. The number indicates the order of decomposing polygons by adding breaking lines according to the mesh templates after selecting a polygon having the most nodes. There are two polygons having the most nodes, six nodes. One of them is selected first and split as the first figure in Fig. 23. After they are updated, one of polygons having five nodes is to be selected next. Lines marked the same number means that they can be selected in arbitrary order since they have the same number of nodes. The final mesh is depicted in the last figure in Fig. 23 and the generated mesh is sufficient to be used without any modification. 5. Automatic FE modeler for whole-ship structural/vibration analysis 5.1. Overall procedure B.-S. Jang et al. / Marine Structures 21 (2008) The procedure for whole ship model is almost the same as that for cargo hold model except for a few processes. A process to increase mesh size to about two or four times of cargo hold model is needed. More complex idealization or simplification process for a bracket of complicated shape in fore/aft parts is also added. This section describes those different features of whole-ship automatic modeler Selection of longitudinal stiffeners to take part in stiffener-based mesh generation The mesh size of whole-ship structural analysis model is about two times of that of cargo hold model and that of vibration analysis model is four times. The purpose of whole-ship model is to examine global behavior of a vessel. Smaller mesh size like longitudinal stiffener spacing increases the number of elements to about 500,000, which is still a big burden to both FE preprocessor and FE solver in spite of enhanced computational capability. In vibration analysis, the smaller mesh size also induces many negligible local vibration modes. For these reasons, whole-ship model employs mesh size several times larger than that of cargo hold model, which cannot consider all stiffener lines in the stiffener-based cutting process. Only stiffeners to resist bending moment are chosen for the cutting process, that is, most of buckling stiffeners on web sections are neglected. Even the bending stiffeners are also partly chosen. The detailed procedure is laid in Fig. 24. Stiffeners to take part in the mesh generation are selected prior to global mesh seed generation. Stiffeners on tank boundary such as upper deck, inner bottom deck, transverse BHD, and longitudinal BHD are the objects of the selection. For decks or transverse BHD, stiffeners between two longitudinal main members such as longitudinal BHD or longitudinal girders are enumerated from center side. In vertical direction, stiffeners on longitudinal BHD between two adjacent plan groups like stringers or decks are to be selected and enumerated from the bottom side. Basic mesh size of FE model for structural analysis is two times of longitudinal stiffener spacing and is four times for vibration. In case of structural analysis model, if the number of stiffeners between two longitudinal main structures is odd, the mesh size in transverse direction can be equally two times of longitudinal stiffener spacing; however, if even, the last mesh size should be three times to prevent the last mesh size just one time of the spacing. The rule is explained in Fig. 24.

27 320 B.-S. Jang et al. / Marine Structures 21 (2008) Automatic grouping Find out intersection lines with other surfaces on different planes. Selection of longitudinal stiffener Count number of longi. stiffeners (n) on upper deck and transverse BHD between two neighboring longi. BHDs. Count number of longi. stiffeners (n) on longi. BHD between two neighboring plan groups. Enumerate longi. stiffeners on deck from center side and stiffeners on an elevation group from bottom side. For structural analysis model If n is even and n > 3, select 2 nd, 4 th, n-2 th longi.stiffener. If n is odd and n > 3, select 2 nd, 4 th, n-1 th longi. stiffener. For vibration analysis model If n is 4k and n 8, select 4 th, 8 th, 4(k-1) th longi. stiffener. If n is 4k+1 and n 5, select 4 th, 8 th,, (4k-1) th longi. stiffener. If n is 4k+2 or 4k+3 and n 6 select 4 th, 8 th,..., 4k th longi. Remove all other stiffeners except the selected stiffeners. Global mesh seeds generation. Fig. 24. Selection of stiffeners to be referred for global mesh seed generation. A similar rule for vibration analysis model enables basic mesh size to be about four times. It allows also three times or five times of the longitudinal stiffener spacing. According to the number of stiffeners between two main structural members, the mesh size array can be generated as follows. Here, the array starts from the center side or bottom side and the digit in the array means the times of longitudinal stiffener spacing: meshsizearray ¼f4; 4;...; 5g for n ¼ 4k, ¼f4; 4;...; 3; 3g for n ¼ 4k þ 1, ¼f4; 4;...; 4; 3g for n ¼ 4k þ 2, ¼f4; 4;...; 4; 4g for n ¼ 4k þ 3. In the next step, global mesh seed generation is made using only the selected stiffeners. The other main procedure is nearly same as hold mesh generation procedure

28 B.-S. Jang et al. / Marine Structures 21 (2008) Fig. 25. Coarse mesh generated on inner bottom plate: (a) given geometry; (b) mesh for structural analysis; (c) mesh for vibration analysis. Fig. 26. An example of simplifying a complex surface through a series of steps. except tolerances in the algorithm are doubled or tripled considering the basic mesh size. Fig. 25 shows coarse mesh for structural analysis and vibration analysis. The mesh size of the former is two times that of stiffener spacing and the latter four times Simplification of complex surface and slender surface Due to the coarse mesh of whole-ship model, all of the stiffener lines cannot be used for splitting surfaces. Especially for web sections, only surface edges and vertex data are available for creating mesh because most of buckling stiffeners are removed as addressed in Section 5.2. However, some brackets on web section in fore part or aft end parts have complex shape as shown in Fig. 26. It is indispensable to simplify such a surface for coarse mesh of uniform size. The proposed algorithm is also designed to treat this simplification. Basically, an arc of small length and small radius is removed. If the angle at the circumference is small, it is removed and two straight edges connected to the arc are extended to their intersection point. Otherwise, if the angle is close to 1801, the arc is replaced by a straight line connecting two vertexes of the arc. Short straight edge is also deleted and two connected edges are directly connected. In addition, a slender surface is modeled as beam elements to get even mesh distribution around the surface. If a surface partly takes a slender shape, only the part is replaced by a curve and the other part remains a surface with an extension of one edge to the replaced curve. These simplification processes are illustrated in Fig. 26 one by one. Fig. 27 shows another example of idealizing surfaces of complex shape illustrating the conversion of slender surfaces into beam elements. What shape a surface takes is judged by checking all edges and all inside angles. Typical shapes are defined by its features of edges and angles in advance,

29 322 B.-S. Jang et al. / Marine Structures 21 (2008) Fig. 27. An example of modeling a slender surface as beam elements. Fig. 28. Mesh generation results for cargo hold model of tanker: (a) a plan group; (b) a section group; (c) a stringer created manually; (d) a web section created manually. and used as criteria to classify a surface. This simplification is made before the process of Search closed polygons along with global mesh seeds on their perimeter in Fig. 7.