J. Cent. South Univ. (2019) 26: 1958-1975

DOI: https://doi.org/10.1007/s11771-019-4145-0

Set-based parametric modeling, buckling and ultimate strength estimation of stiffened ship structures

LI Yi-bo(李毅波)^{1, 2}, PAN Qing(潘晴)^{1, 2}, HUANG Ming-hui(黄明辉)^{1, 2}, LI Lu(李鲁)³

1. State Key Laboratory of High Performance Complex Manufacturing, Central South University,Changsha 410083, China;

2. School of Mechanical and Electrical Engineering, Central South University, Changsha 410083, China;

3. School of Software, Central South University, Changsha 410083, China

Central South University Press and Springer-Verlag GmbH Germany, part of Springer Nature 2019

Abstract: There have been a great demand for a suitable and convenient method in the field of buckling analysis of stiffened ship structures, which is essential to structural safety assessment and is significantly time-consuming. Modeling, buckling behaviors and ultimate strength prediction of stiffened panels were investigated. The modeling specification including nonlinear finite element model and imperfections generation, and post-buckling analysis procedure of stiffened plates were demonstrated. And a software tool using set-based finite element method was developed and executed in the MSC. Marc environment. Different types of stiffen panels of marine structures have been employed to investigate the buckling behavior and assess the validity in the estimation of ultimate strength. A comparison between results of the generally accepted methods, experiments and the software tool developed was demonstrated. It is shown that the software tool can predict the ultimate capacity of stiffened panels with imperfections with a good accuracy.

Key words: buckling; ultimate strength; stiffened plates; parametric modeling; ship structure

Cite this article as: LI Yi-bo, PAN Qing, HUANG Ming-hui, LI Lu. Set-based parametric modeling, buckling and ultimate strength estimation of stiffened ship structures [J]. Journal of Central South University, 2019, 26(7): 1958-1975. DOI: https://doi.org/10.1007/s11771-019-4145-0.

1 Introduction

Stiffened panels which are reinforced in the longitudinal direction and transversely supported by widely spaced transverse structures, are widely used in all parts of the hulls, e.g., transverse bulk heads, deck beams and bottom floors. Loading capacity, buckling behavior and ultimate strength of the panels exert an important influence on the longitudinal strength of the hull girders, which has been and will always remain the crucial point for consideration in the design of ships.

Buckling analysis is essential for stiffened plates of various engineering structures, since the aim of nonlinear buckling analysis, i.e., ultimate strength prediction, of ship structures is to provide sufficient theoretical evidence for structural design and strength assessment.

Buckling and ultimate strength of stiffened structures have been extensively investigated over past decades. There are four kinds of methods to estimate buckling behaviors, i.e., analytical approaches [1-4], semi-analytical methods [5, 6],experimental tests [7-10], empirical methods [11-13] and non-linear finite element methods (FEM) [14-18]. However, the analytical approaches are restricted to idealized and simple cases, which has limited their development and application. The test method is often uneconomic though the first material can be obtained. On the other hand, the test results can hardly be applied to large ship structures because of the problem of dimension transformation. Also, the empirical method hinder the high fidelity estimation of buckling behaviors.

Structural instability analysis of stiffened panels associated with post buckling analysis has been discussed and investigated in the literature. PRZEMIENIECKI [19, 20] proposed a displace method of matrix analysis for local instability prediction of stiffened plates, based upon finite element method. PATEL et al [21, 22] examined the dynamic instability behaviors of stiffened plates that is subjected to in-plane harmonic load using finite element method. In Ref. [23], plate prismatic sub-stiffening was introduced to increase local stability and strength performance, in which a critical stress criterion for post-buckling stability were employed. They have shown that the results simulated by finite element method agree with the experimental data with a good accuracy. XU et al [24] investigated the instability behavior of stiffened panels under axial compression using a nonlinear finite element analysis model with measured initial imperfections. ALSOS et al [25, 26] studied the failure behavior of stiffened plates subjected to collision cases using finite element code LS-DYNA, in which the Bressan– Williams–Hill (BWH) instability criterion was adopted. In Ref. [27], the effects of square opening and geometrical parameters on ultimate strength and instability characteristics of stiffened plates with cutouts have been investigated using an approximate method. SU et al [28] proposed a model of titanium alloy stiffened plates under shear load and the buckling instability and failure mechanism were examined using the finite element method. In Ref. [29], different buckling modes including torsional and web buckling, and instability behaviors of stiffened plates have been investigated. FENNER et al [30] developed a model of stiffened plates with fillets and a buckling analysis have been conducted to investigate the instability modes. It is shown that the filleted line junctions contribute to the increase of structural buckling stability.

Since the buckling of ship structures is intrinsic nonlinear, the nonlinear FEM has become the most effective technique for the prediction of ultimate strength, stress status estimation and instability analysis of the ship structures [14-22, 24-26]. Among the nonlinear FEM commercial packages, MSC. Marc [31] is one of the most outstanding and powerful finite element platforms for researchers and engineers, especially in the field of dynamic and multi-physics simulations.

The first step for the procedure of bucking analysis is modeling of engineering structures. The computer aided design (CAD) models of stiffened plates are constructed by software tools like Solidworks, Pro/Engineering, UG, etc. In order to proceed the process of finite element analysis, the established models were imported into the platform of commercial software, e.g., MSC. Marc, Abaqus, and ANSYS. The commercial packages facilitate the modeling process for simple structures. While for the case of structural optimization, in which the design of geometrical parameter changes frequently and iteratively, it is complicated to reconstruct the CAD model and proceed the post-processing repeatedly. Yet, a connection between practitioners and commercial finite element tools in this regard, i.e., complicated case, is still lacking.

In the past decades, significant progresses have been made in the field of computational mechanics, and numerous codes and software tools that facilitate the engineering design and analysis process, spring up like mushrooms. For instance, PAPAZAFEIROPOULOS et al [32] developed a software platform for finite element post-processing by constructing a connection between MATLAB and Abaqus. YANG et al [33], introduced a software platform to cope with the issue of complexity of finite element model online updating in hybrid simulation. HSIEH et al [34] provided a general framework for meshless methods, which facilitates the implementations and broaden new research and developments. Also, development of software platform incorporated MSC.Marc has contributed to technological progress, includes finite element data exchange system [35], implementation using subroutine [36-41], stress formation behavior [42], thermal buckling analysis [43], etc.

In this work, in order to make the analyzing process convenient for engineers to investigate the buckling behaviors, a software tool which incorporates set-based modeling, Marc/Mentat and equation solver (kernel) was developed. Nonlinear buckling analysis for different types of stiffened panels are carried out using the proposed toolbox. The proposed toolbox has provide a parametric modeling interface between practitioners and FEM software. The modeling, buckling analysis, and post-processing procedures have been integrally incorporated into the framework of commercial software. Therefore, the efficiency of analysis and modeling for stiffened panels is increased drastically.

This research is organized as follows. Section 2 is devoted to a general description of the process of buckling analysis of stiffened plates. In Section 3, the software framework and constitution are presented. Section 4 shows the applications of the software platform in parametric modeling of complex plates and ultimate strength prediction of stiffened structures. Finally, the conclusion is given in Section 5.

2 Nonlinear buckling and methodology

In the design of engineering structures, the stage of post buckling makes it possible for the panel to continue to carry the load. Thus, it is an effective way to achieve the goal of lightweight design by taking advantage of capacity of bearing load for stiffened panels.

2.1 Modeling of stiffened panel

2.1.1 FE model of the stiffened model

The middle region of ship structures, e.g., an oil tanker, can be treated as a rectangular box structure composed of several stiffened panels with stiffeners and transverse frames.

As shown in Figure 1, a finite model of the stiffened panel with stiffeners was established. The model was constructed in a right hand Cartesian coordinate system, in which x-axis is parallel with the direction of stiffeners and y-axis is perpendicular to x-axis. In addition, z-axis is vertical to the plate.

Four corners of the rectangular stiffened panel are labeled as C1, C2, C3 and C4, respectively, as presented in Figure 2. The plate, stiffener webs and flanges are all modelled using 4-node shell elements.According to the rules of nonlinear buckling analysis of IACS common rules [44-46] and DET NORSKE VERITAS (DNV Rules), no less than six elements should be used in the transverse directions between stiffeners for the plate, and the number of elements should be properly selected in order to ensure that the elements are almost square. For the stiffener web, no less than three elements should be selected across the web height and the number of elements should be chosen so that the elements are nearly square. With respect to the stiffener flange, there should be more than one element across the stiffener flange for L-shaped profiles and two elements for T-shaped profiles. In this study, in order to determine the proper mesh density, the convergence investigation by changing the number of elements was carried out. In Figure 3, the convergence results regarding ultimate strength is illustrated. The variables, n_p, n_w and n_f denote the number of element of plates, stiffener web and flange, respectively. It is shown that a convergence can be obtained preferably when the mesh density is set as n_p≥6, n_w≥2 and n_f≥2.

Figure 1 Finite model of stiffened panel

Lines labeled as FR1, FR2 and FR3 denote the transverse frames with 1/2+1+1+1/2 spacing. The transverse frames are not modeled and are represented by multi-point constraints (MPCs), which will be discussed in the later section. The material parameters of the plates and stiffeners are chosen as bi-linear material model with elastic modulus E=205800 N/mm², Poisson ratio γ=0.3 and yield stress σ_y=315 N/mm².

Figure 2 Nodes and edges in stiffened panel model

Figure 3 Convergence investigation regarding selection of number of element

2.1.2 Boundary conditions, load cases and set based definition algorithm

All edges in the model are forced to remain straight during the analysis. Edges C1-C4 and C2-C3 are restricted from rotation around y-axis and z-axis.

According to DNV rules, boundary conditions should be imposed on the edges and lines, as indicated in Figure 2 and Table 1. To perform such complex constrains well in the software tool, dedicated modeling methods have been studies and lots of MPCs, such as RBE2’s, node ties and servo links should be used as shown in Table 1.

Figure 4 is illustrated to represent the support of adjacent panels in a larger structure. If a panel buckles the edges will normally try to pull in, the neighboring panels also will buckle and will therefore try to pull in with the same force. These forces will balance each other leaving the edge to remain straight. All edges of the FE model of stiffened panel should be keep straight during the analysis procedure in order to represent the mutual “pull-in” effects of adjacent plates in a large scale panel of ship structure. Therefore, all the nodes on edges B3 and B4 should be forced to move on a straight line, which is illustrated in Figure 5. In addition, the opposite edges of the panel should be constrained to be parallel, i.e., B1∥B2, B3∥B4, respectively.

In order to induce MPCs into the model conveniently, a set-based method is used as shown in Figure 6, sets need to be used are listed in Table 1 and Table 2. Firstly, all the nodes (corner nodes, RBE2 nodes, stiffened web nodes, transverse frame nodes, etc.) of both the retained and tied were defined. In this step, coordinates of all the nodes were obtained in order to facilitate the subsequent analysis process. Then, all the sets defined were transferred into the corresponding module of the software tool associated with the interaction between sets and Marc/Mentat.

Note that the transverse frames, FR1, FR2 and FR3 are not modeled and are expressed by constraints in z-axis direction. Four typical load cases with different combination of loads are modeled as shown in Table 2.

Table1 Constraints and boundary conditions for panel

Figure 4 Pulling in effect of buckling in large stiffened plates [46]

Figure 5 Constraints to keep model edges parallel [46]

2.1.3 Imperfection modeling

Initial imperfections of the stiffened panels play a key role in buckling characteristics [14]. It is shown that reasonable estimation of ultimate capacity can be achieved by choosing suitable initial imperfections based upon linear buckling modes results.

The imperfection is a combination of local and global deflections, which are illustrated in Figure 7. Thus, we need to modify coordinates of all the nodes before proceeding nonlinear buckling analysis.

Concerning the calculation of the local deflection, the theoretical formulations are as follows:

                (1)

                  (2)

where a is the transverse frame spacing; m and n represent the number of stiffener and transverse frame, respectively. In the local modes, as shown in Figure 7(a), the plate and stiffener webs have multi-wave buckling modes with a magnitude of w_p=b/200 for the plate, where b is the stiffener spacing, and w_p=h_w/200 for the stiffener web [47] and h_w is the stiffener height.

It is difficult to compute right coordinates of all the nodes according to Eqs. (1) and (2) in a finite element model, but we can use the first buckling mode to do such a job. As shown in Figure 8, plate deflection of the first buckling mode is a multi-wave shape, by adjusting the magnitude of all the waves, Eqs. (1) and (2) can be satisfied easily, detailed process will be presented in Section 3.

Figure 6 Flowchart of set based method

Table 2 Loads and load cases

The first buckling mode (eigenvalue) was utilized to represent the local deflection, but some researchers found that it is not enough to have a reasonable representation of the local deflection. Equation (1) indicates that the magnitude of the maximum deflection of all the stiffener web, w_wl, should be the same and equal to h_w/200.Equation (2) indicates that the magnitude of the maximum z-deflection of the plate, w_pl, should be the same and equal to b/200. However, it is shown in Figure 8 that neither the z-deflection of the plate nor the y-deflection of the stiffener web satisfies such requirements.

Then, the set-based magnification method is used to make a reasonable local deflection. Firstly, different sets of the plates and stiffener webs were created, as shown in Figure 8. nSetLong_i (i=1, 2, 3, …, ns) represent different sets of stiffener webs, while nSetTrans_j (j=1, 2, 3, …, ns+1) represent different sets of plates according to multi-half waves. Total number of the half waves is equal to ns+1 because cross nodes between the stiffener webs and plates are fixed in z direction. After getting the magnitude of different waves for different sets, amplification factors can be get from Eqs. (3) and (4):

                 (3)

                 (4)

where coeY(i) and coeZ(i) represent amplification factors, respectively; maxval(Dy(i)) and maxval(Dz(i)) represent magnitude of different waves for different sets.

Figure 7 Initial imperfection:

Figure 8 Deflection of plate for first eigenvalue for direction:

The global imperfection definition of global z-deflections:

                   (5)

This is applicable to both plate and stiffeners. The y-deflections of the stiffeners can be expressed as:

           (6)

where w_s is the global deflection of stiffener webs and w_g is the global deflection of of both plate and stiffener webs.

2.2 Nonlinear buckling analysis procedures

The procedure of nonlinear buckling analysis of stiffened panels can be divided into:

Step 1: Modeling of geometry, boundary conditions and loads, etc.

Step 2: Linear buckling analysis, which is used for extracting eigenvalue, mode and local imperfection generation.

Step 3: Nonlinear buckling analysis, which contains ultimate strength estimation, and mode extracting.

3 Software architecture & framework

The design of this software tool aims to facilitate the procedure of complex and iterative modeling of stiffened panels and buckling analysis. The software was developed in the environment of MSC.Marc/Mentat platform, and Figure 9 provides a general overview of schematic interactions between each module.

For the software platform, the interface definition (*.ms) file can be used to develop the interface of input of parameters of plates. When the parameters are defined, parameters of the stiffened plate are transferred to the command of Python subroutine by data ports. After the model is established, the Fortran user subroutine is located. Then the Fortran subroutine (*.f) file and the solution file(*.dat) of Marc are loaded to solver kernel, where the buckling problem is solved using finite element method. The main internal behaviors of the software tool are described below.

Figure 9 Architecture of software tool

3.1 System implementation and interface design

Figure 10 shows different types of stiffener which are commonly used, and it is really fussy for practitioners to construct the stiffened panel repeatedly, especially for the case of optimization design. In order to simplify the modeling process of stiffened panels, a graphical user interface (GUI) is coded by interface definition file (*.ms) of MSC. Marc/Mentat, as shown in Figure 11. The user can easily define geometry, constraints, loads and boundary conditions. In addition, the GUI can send commands to Python subroutine to proceed the process of finite element modeling by clicking the button of “Proceed The Modeling”. Furthermore, the GUI can be used to proceed the linear and nonlinear buckling analysis, respectively, by triggering the Fortran subroutine (i.e., clicking the button of “Submit: CaseN_linear” and “Submit: CaseN_nonlinear”) after the subroutine is located by Python script.

3.2 Parametric modeling module

The parametric modeling module is written in Python, which is the selected scripting language for MSC.Marc. The modeling procedure are described in Appendix A in detail.

3.3 Buckling analysis architecture

As presented in Section 2, we introduced a modified first eigenvalue to represent the local deflection, which was coded by Fortran, which is shown in Appendix B.

Firstly, the coordinates of all the nodes in the finite model were obtained and transferred into array ford and Startarry. Then, let the set name equal to plate and the eigenvalue in the direction of z-axis was obtained. Next, the maximum deflection in the direction of z-axis was found and the scale factor was computed. Thus, the scaled coordinates of all the nodes in set plate were achieved.

Figure 10 Stiffener types:

Figure 11 GUI of modeling and analysis

At the same time, let the set name equal to the web and the eigenvalue in the direction of y-axis was obtained. Next, the maximum deflection in the direction of y-axis was found and the scale factor was computed. Thus, the scaled coordinates of all the nodes in set web were achieved.

For the generation procedure of global imperfection, the coordinates of all the nodes in the model are extracted and transferred to the array gord. Then, the set plateall contains the nodes of plates and stiffener web, are used to modify the coordinates of all the nodes based upon Eq. (3). Then a set named stiffenerall was defined and used to modify the coordinates of stiffenerall based upon Eq. (4). Since the imperfection is a combination between local and global deflections. Therefore, the coordinates of all nodes of the stiffened panel must be updated before submitting jobs to the solver and the process are illustrated in Figure 12.

3.4 Post-processing module

After completing buckling and nonlinear ultimate strength analysis, the software provides a module for generating analysis report automatically as shown in Figure 11. The analysis report is writing in HTML format, which can be opened by any web browsers. It is coded by python language through communications with MARC/MENTAT.

The report is comprised of three parts, model description, linear buckling and ultimate strength, as shown in Figure 13. Parameters of the model, linear buckling factors and ultimate strength result can be transfer to analysis report automatically through the workflow shown in Figure 14.

4 Estimation of ultimate capacity and buckling

The software tool provides a non-intrusive connection between practitioners and onerous buckling analysis tasks. Behaviors of buckling and estimation of ultimate strength using the software tool will be demonstrated in this section.

Figure 12 Fortran code for global imperfection generation

4.1 Characteristics of buckling

The model is analyzed as an example for evaluate the effectiveness of the software. The characteristics of linear and nonlinear buckling are shown in Figures 15 and 16, respectively. As is shown in Figure 15, due to that the edge of the stiffened plate are restricted to be straight during the process and transverse frames are modeled as MPCs, buckling characteristics of the unloaded side is different compared to the other width direction. During the analysis process, the first eigenmodes were extracted and scaled to generate local imperfection, as presented in Section 3. When the plate endure load, both plate and stiffeners are almost buckled simultaneously, and inner and outer displacement occur. Both of the buckling behaviors of linear and nonlinear buckling cases can be obtained from the post-processing module (collected as an analysis report for each case).

Figure 13 Architecture of HTML analysis report generating module

4.2 Validation of estimation of ultimate capacity

There have been a number of methods to predict the ultimate capacity of stiffened plates. Among them, semi-empirical approach and finite element simulation are often utilized in practice. In this paper, two well-known formulas for estimating ultimate strength are used, i.e., Faulkner’s and Zhang’s formula. And they are expressed as:

Faulkner's formula [48]:

                            (7)

Zhang's formula [14]:

                 (8)

where σ_u denote the maximum stress when the plate collapses, and β, λ stand for plate slenderness ratio and stiffener slenderness ratio, respectively, and they are expressed as:

                              (9)

                            (10)

                                (11)

where t denotes the plate thickness; I stands for the moment of inertia and A represents the cross-sectional area of the stiffener; a is the length between two transverse frames across the x-axis direction and b is the length between two transverse frames across the y-axis direction. The above mentioned formulas have been proven to be effective for the prediction of ultimate strength under axial compression.

A comparison of ultimate capacity of stiffened plates between semi-empirical methods and software tool developed were conducted. Three types of stiffeners are chosen: FB type stiffener, L-shaped stiffener and T-shaped stiffener. Nine stiffened panels with different combinations of β and λ, are analyzed using the software tool. The geometric detains of the selected stiffened plates are shown in Table 3. The results obtained by Zhang’s formula and the software tool developed in this work are presented in Table 4, respectively. It can be seen from the comparison that the software tool agrees with the results by ZHANG et al [14], with a good accuracy, since the semi-empirical approaches have been validated by experimental investigations. For the selected stiffened panels, the relative error of all selected stiffened plates ranges within ±10% error band.

Also, the ultimate strength obtained from the experiments and the software tool were compared. The results include sixteen data which are investigated in publications and each of the stiffened plate were analyzed using the software tool, and the results are shown in Table 5. The data considered are selected from GHAVAMI et al [49], XU et al [8] and GORDO et al [50, 51]. Calculated results using Faulkner’s and Zhang’s formula are also demonstrated in Table 5. Note that the initial imperfections are applied to each of the plates considered.

Figure 14 Flowchart of generating of ultimate strength

It can be seen from Table 5 that an excellent agreement are achieved between software tool and the experiments. For all the experiments, 81.3% of the data is within the ±5% error band and 87.5% of the selected data are within the ±10% error band. In addition, it is observed from Table 5 that the agreement between experiments and Faulkner’s and Zhang’s formula is also good for most of the cases.

Note that only the experimental results that have the same or similar boundary conditions with the FE model established in the software toll, can be selected in order to guarantee the effectiveness of data.

5 Conclusions

A software tool for set-based parametric modeling, buckling and ultimate strength estimation of stiffened marine structures has been developed and validated with formulas available.

Its development stems from the burdensome modeling and analysis tasks in buckling of stiffened panels. The software platform provides a friendly link, i.e., GUI, between practitioners and onerous buckling analysis tasks, in which the model can be constructed and the analysis jobs are submitted. The software tool has been verified to be effective against ten semi-empirical results.

Figure 15 Deformations mode for linear buckling of:

Figure 16 Nonlinear buckling behaviors under bi-axial load:

Table 3 Geometric details of stiffened panels

Table 4 Comparison between semi-empirical formula and the software tool

Table 5 Comparison between experimental results and software tool

In this investigation, the boundary conditions imposed and determination of modeling area are based upon the IACS standards. However, there are still controversial aspects regarding imposing of boundary conditions and modeling area. Although the results obtained using the finite element model configured based on the IACS standards agree with the experimental results with a good accuracy in many load conditions. In the future, more prominent modeling standards remain to be studied. And these modeling method can also be incorporated into the proposed toolbox if possible.

Appendix A: Python script of parametric modeling for Mentat

Firstly, the PyMentat module should be imported into Python script,

from py_mentat import *

if __name__ == '__main__' :

py_connect(" ", 40007)

main()

py_disc onnect()

def main():

Then, all the parameters of the stiffened panels, which are imported in the GUI, are obtain by the code below:

a=py_get_float("a") # Distance between Transverse frames

b=py_get_float("b") # Distance between Longitudinal frames

t=py_get_float("t") # Thickness of the Plate

hw=py_get_float("hw") # Height of the Stiffener web

tw=py_get_float("tw") # Thickness of the Stiffener web

bf1=py_get_float("bf1") # Left Width of Stiffener flange

bf2=py_get_float("bf2") # Right Width of Stiffener flange

tf=py_get_float("tf") # Thickness of the Stiffener flange

nfr=py_get_int("nfr") # Number of Transverse Stiffners

ns=py_get_int("ns") # Number of Stiffeners

Modulus=py_get_float("Modulus") # Define Elastic Modulus

Density=py_get_float("Density") # Density of the material

Poisson=py_get_float("Poisson") # Define Poisson

ET=py_get_float("ET") # Harding Modulus, MPa

Yield=py_get_float("Yield") # Define Yield Stress

Then, two commands were executed:

Mesh_Gen(modelname,a,b,t,hw,tw,bf1,bf2,tf,m,ns,np,nw,nf)

Assgin_Mat(Modulus,Density,Poisson,ET,Yield)

Assgin_Geo(t,tw,tf)

nnode=[0,0]

nnode=Make_MPC(a,b,t,hw,tw,bf1,bf2,tf,m,ns)

nnode_B1 = nnode[1]

nnode_B3 = nnode[0]+2

NodeSets(a,b,t,hw,tw,bf1 ,bf2,tf,nfr,ns,nw,nnode_B1,nnode_B3)

Loadcase()

Jobs()

py_send ("*save_model")

return

The subroutine Mesh_Gen is written to generate mesh and put them into correct sets, and Assgin_Mat is used to assign all the material properties to all the elements. The subroutine Assgin_Geo aims to assign all the geometry properties to all the elements, and NodeSets is used to define the node sets, of which the coordinates will be scaled for the plate and stiffener. Loadcase is used to define load cases, convergence testing parameters, and arc length parameters.

Appendix B: Modification to generation of local imperfection

A Fortran subroutine was defined to modify the generating of initial local imperfection:

subroutine impd(lnode,dd,td,xord,f,v,a,ndeg,ncrd)

c user subroutine for output of "displacements".

c lnode(1) user node number

c lnode(2)=1 structural

c dd array of incremental displacements of this node

c td array of total displacements of this node

c xord array of coordinates of this node

c f array of reaction forces/residuals

c v array of velocity (dynamics only)

c a array of acceleration (dynamics on ly)

c ndeg number of degrees of freedom per node

c ncrd number of coordinates per node

#ifdef_IMPLI CITNONE

implicit none

#else

implicit logical (a-z)

#endif

c * * Start of generated type statements **

c xord(),cord():original coordinates

c Disp():displacement of the current increment

Then, the variables used in the subroutine are defined, and parameters of the stiffened panels are obtained.

In order to obtain the name and number of the nset, of which the coordinate will be modified, the codes are expressed as:

nline =0

open(21,file='.\setnam.tmp',status='old')

do while (.true.)

read(21,*,end=10 1)

nline=nline+1

enddo

101 continue

rewind(21)

i=1

do while(i<=nline)

read(21,*) getnam(i)

i=i+1

enddo

close (21)

The coordinates of all the nodes are extracted and imported to the array of startarry, and the codes includes:

if (inc.eq.0) then

if (incsub.eq.1) then

i=1

do while(i<=numnp)

if(lnode(1).eq.i) then

     j=1

   do while(j<=3)

      startarray(i,j)=xord(j)

      ford(i,j)=xord(j)

      j=j+1

     end do

     end if

    i=i+1

  end do

    For different types of sets, the scaled factor was computed from:

nplate=((nline-2)+1)/2

nstiff=(nline-2)-nplate

i=1

do while(i<=(nline-2))

   setnam=getnam(i)

   call marc_setinf (setnam,ihav,list,ityp,inum)

   j=1

   do while(j<=inum)

    Dy(j)=0.0

    Dz(j)=0.0

    call nodvar(1,list(j),disp,nqncomp,nqdatatype)

    Dy(j)=Dy(j)+abs(disp(2))

    Dz(j)=Dz(j)+abs(disp(3))

   j=j+1

   end do

   coeY(i)=ww/maxval(DY)

   coeZ(i)=wp/maxval(DZ)

i=i+1

enddo

    For different set of plates, the coordinates of all the nodes are extracted and used for computing:

i=1

do while(i<=nplate)

   setnam=getnam(i)

   call marc_setinf(setnam,ihav,list,ityp,inum)

   j=1

   do while(j<=inum)

     if(lnode(1).eq.list(j)) then

       k=list(j)

  call nodvar(1,lnode(1),disp,nqncomp,nqdatatype)

  ford(k,1)=startarray(k,1)+disp(1)*coeZ(i)

  ford(k,2)=startarray(k,2)+disp(2)*coeZ(i)

  ford(k,3)=startarray(k,3)+disp(3)*coeZ(i)

 end if

 j=j+1

 end do

i=i+1

end do

The same procedure is proceeded to the sets of StiffFlange, and in order to generate the global imperfection, the coordinates of all the nodes for nSet_PlateAl set are extracted and used for computing:

setnam=getnam(nline-1)

call marc_setinf(setnam ,ihav,list,ityp,inum)

i=1

do while(i<=inum)

if(lnode(1).eq.list(i)) then

  k=list(i)

  x0=startarray(k,1)+a0/2.0

  y0=startarray(k,2)+b0

  z0=startarray(k,3)

  zz=wg*sin((pi*x0/a0)-pi/2.0)*sin(pi*y0/B1)

  gord(k,1)=startarray(k,1)

  gord(k,2)=startarray(k,2)

  gord(k,3)=startarray(k,3)*2+zz

 end if

 i=i+1

end do

Then the coordinates are written to the corresponding file:

i=1

do while(i<=numnp)

   if(lnode(1).eq.i) then

    write(201,110) i,ford(i,1),ford(i,2),ford(i,3)

    write(202,110) i,gord(i,1),gord(i,2),gord(i,3)

    write(203,110) i,ford(i,1)+gord(i,1),

    + ford(i,2)+gord(i,2),ford(i,3)+gord(i,3)

    j=1

    do while(j<=3)

     write(204, 120) ford(i,j)+gord(i,j)

     j=j+1

    end do

   end if

   i=i+1

end do

endif

endif

110 format(1X,I9,',',es19.12,',',es19.12,',',es19.12)

120 format(1X,es19.12)

return

end

References

[1] PAIK J K, THAYAMBALLI A K, KIM D H. An analytical method for the ultimate compressive strength and effective plating of stiffened panels [J]. Journal of Constructional Steel Research, 1999, 49(1): 43-68. DOI: 10.1016/S0143-974X (98)00207-7.

[2] CUI Jin-ju, WANG De-yu, MA Ning. Elastic buckling of stiffened panels in ships under bi-axial compression [J]. Ships and Offshore Structures, 2017, 12(5): 599-609. DOI: 10.1080/17445302.2016.1189140.

[3] FUJITA Y, NOMOTO T, NIHO O. Ultimate strength of rectangular plates subjected to combined loading (1st & 3rd report)[J]. Journal of the Society of Naval Architects of Japan, 1979, 145(149): 194-202. .DOI: 10.2534/jjasnaoe 1968.1979.194.

[4] OZDEMIR M, ERGIN A, YANAGIHARA D, TANAKA S, YAO T. A new method to estimate ultimate strength of stiffened panels under longitudinal thrust based on analytical formulas [J]. Marine Structures, 2018, 59: 510-535. DOI: 10.1016/ j.marstruc.2018.01.001.

[5] BRUBAK L, ANDERSEN H, HELLESLAND J. Ultimate strength prediction by semi-analytical analysis of stiffened plates with various boundary conditions [J]. Thin-Walled Structures, 2013, 62: 28-36. DOI: 10.1016/j.tws.2012. 08.005.

[6] MANCO T, MARTINS J P, RIGUEIRO C, SILVA L S D. Semi-analytical orthotropic model for the prediction of the post-buckling behaviour of stiffened cylindrically curved steel panels under uniaxial compression [J]. Computers & Structures, 2018, 211: 27-42. DOI: 10.1016/j.compstruc. 2018.08.015.

[7] CHOI B H, HWANG M, YOON T, YOO C H. Experimental study of inelastic buckling strength and stiffness requirements for longitudinally stiffened panels [J]. Engineering Structures, 2009, 31(5): 1141-1153. DOI: 10.1016/j.engstruct.2009.01. 010.

[8] XU M C, SOARES C G. Experimental study on the collapse strength of wide stiffened panels [J]. Marine Structures, 2013, 30: 33-62. DOI: 10.1016/j.marstruc.2012.10.003.

[9] XU M C, SOARES C G. Comparisons of calculations with experiments on the ultimate strength of wide stiffened panels [J]. Marine Structures, 2013, 31: 82-101. DOI: 10.1016/ j.marstruc.2013.01.003.

[10] NOORALIZADEH A, NAGHIPOUR M, NEMATZADEH M, et al. Experimental evaluation of steel plate shear walls stiffened with folded sheets [J]. International Journal of Steel Structures, 2017, 17(1): 291-305. DOI: 10.1007/s13296- 015-0206-x.

[11] KHEDMATI M R, ZAREEI M R, RIGO P. Empirical formulations for estimation of ultimate strength of continuous stiffened aluminium plates under combined in-plane compression and lateral pressure [J]. Thin-Walled Structures, 2010, 48(3): 274-289. DOI: 10.1016/j.tws. 2009.10.001.

[12] LEHETA H W, ELHANAFI A S, BADRAN S F. Reliability analysis of novel stiffened panels using Monte Carlo simulation [J]. Ships and Offshore Structures, 2017, 12(5): 640-652. DOI: 10.1080/17445302.2016.1193984.

[13] XU Ming-cai, SONG Zhao-jun, ZHANG Wen-bo, PAN Jin. Empirical formula for predicting ultimate strength of stiffened panel of ship structure under combined longitudinal compression and lateral loads [J]. Ocean Engineering, 2018, 162: 161-175. DOI: 10.1016/j.oceaneng.2018.05.015.

[14] ZHANG Shen-ming, KHAN I. Buckling and ultimate capability of plates and stiffened panels in axial compression [J]. Marine Structures, 2009, 22(4): 791-808. DOI: 10.1016/ j.marstruc.2009.09.001.

[15] KIM J H, JEON J H, PARK J S, SEO H D, AHN H J, LEE J M. Effect of reinforcement on buckling and ultimate strength of perforated plates [J]. International Journal of Mechanical Sciences, 2015, 92: 194-205. DOI: 10.1016/j.ijmecsci.2014. 12.016.

[16] KHEDMATI M R, BAYATFAR A, RIGO P. Post-buckling behaviour and strength of multi-stiffened aluminium panels under combined axial compression and lateral pressure [J]. Marine Structures, 2010, 23(1): 39-66. DOI: 10.1016/ j.marstruc.2009.10.003.

[17] LI Chen-feng, ZHU Zhi-yao, REN Hui-long, SOARES C G. Finite element analysis of the ultimate strength of aluminum- stiffened panels with fixed and floating transverse frames [J]. Journal of Offshore Mechanics and Arctic Engineering, 2017, 139(4): 041401. DOI: 10.1115/1.4036111.

[18] LI Chen-feng, REN Hui-long, ZHU Zhi-yao, SOARES C G. Numerical investigation on the ultimate strength of aluminium integrally stiffened panels subjected to uniaxial compressive load [J]. Thin-Walled Structures, 2018, 127: 221-234. DOI: 10.1016/j.tws.2018.01.003.

[19] PRZEMIENIECKI J S. Matrix analysis of local instability in plates, stiffened panels and columns [J]. International Journal for Numerical Methods in Engineering, 1972, 5(2): 209-216. DOI: 10.1002/nme.1620050207.

[20] PRZEMIENIECKI J S. Finite element structural analysis of local instability [J]. AIAA Journal, 1973, 11(1): 33-39. DOI: 10.2514/3.50433.

[21] PATEL S N, DATTA P K, SHEIKH A H. Buckling and dynamic instability analysis of stiffened shell panels [J]. Thin-Walled Structures, 2006, 44(3): 321-333. DOI: 10.1016/j.tws.2006.03.004.

[22] PATEL S N, DATTA P K, SHEIKH A H. Dynamic instability analysis of stiffened shell panels subjected to partial edge loading along the edges [J]. International Journal of Mechanical Sciences, 2007, 49(12): 1309-1324. DOI: 10.1016/j.ijmecsci.2007.04.006.

[23] QUINN D, MURPHY A, MCEWAN W, LEMAITRE F. Stiffened panel stability behaviour and performance gains with plate prismatic sub-stiffening [J]. Thin-Walled Structures, 2009, 47(12): 1457-1468. DOI: 10.1016/j.tws. 2009.07.004.

[24] XU M C, SOARES C G. Comparisons of calculations with experiments on the ultimate strength of wide stiffened panels [J]. Marine structures, 2013, 31: 82-101. DOI: 10.1016/ j.marstruc.2013.01.003.

[25] ALSOS H S, AMDAHL J, HOPPERSTAD O S. On the resistance to penetration of stiffened plates, Part II: Numerical analysis [J]. International Journal of Impact Engineering, 2009, 36(7): 875-887. DOI: 10.1016/j.ijimpeng. 2008.11.004.

[26] STORHEIM M, ALSOS H S, HOPPERSTAD O S, AMDAHL J. A damage-based failure model for coarsely meshed shell structures [J]. International Journal of Impact Engineering, 2015, 83: 59-75. DOI: 10.1016/j.ijimpeng. 2015.04.009.

[27] ALAGUSUNDARAMOORTHY P, SUNDARAVADIVELU R, GANAPATHY C. Ultimate strength of stiffened panels with cutouts under uniaxial compression [J]. Marine Structures, 1995, 8(3): 279-308. DOI: 10.1016/0951- 8339(94)00006-E.

[28] SU Yu-ru, GUAN Zhi-dong, WANG Xin, LI Zeng-shan, GUO Jun, HUANG Yong-jie. Buckling and post-buckling behavior of titanium alloy stiffened panels under shear load [J]. Chinese Journal of Aeronautics, 2019, 32(3): 619-626. DOI: 10.1016/j.cja.2018.09.007.

[29] RANJI A R. Comparative study of elastic buckling of plates stiffened with angle bar stiffeners [J]. Journal of Failure Analysis and Prevention, 2017, 17(3): 554-562. DOI: 10.1007/s11668-017-0282-7.

[30] FENNER P E, Watson A. Finite element buckling analysis of stiffened plates with filleted junctions [J]. Thin-Walled Structures, 2012, 59: 171-180. DOI: 10.1016/j.tws.2012.05. 011.

[31] MSC. MARC corp. Marc documentation, Volume A-D [R]. MSC. MARC. corp.

[32] PAPAZAFEIROPOULOS G, MUNIZ-CALVENTE M, MARTINEZ-PANEDA E. Abaqus2Matlab: a suitable tool for finite element post-processing [J]. Advances in Engineering Software, 2017, 105: 9-16. DOI: 10.1016/j.advengsoft.2017. 01.006.

[33] YANG Ge, WU Bin, OU Ge, WANG Zhen, DYKE S. HyTest: platform for structural hybrid simulations with finite element model updating [J]. Advances in Engineering Software, 2017, 112: 200-210. DOI: 10.1016/j.advengsoft.2017.05.007.

[34] HSIEH Y M, PAN M S. ESFM: An essential software framework for meshfree methods [J]. Advances in Engineering Software, 2014, 76: 133-147. DOI: 10.1016/ j.advengsoft.2014.06.006.

[35] AFAZOV S M, BECKER A A, HYDE T H. Development of a finite element data exchange system for chain simulation of manufacturing processes [J]. Advances in Engineering Software, 2012, 47(1): 104-113. DOI: 10.1016/j.advengsoft. 2011.12.011.

[36] BANAS K. Implementation of the nonlinear imperfect transmission conditions between dissimilar materials into commercial FEM software MSC. Marc using Fortran user subroutine: Plane strain case [J]. Composite Interfaces, 2015, 22(6): 447-471. DOI: 10.1080/09276440.2015.1048649.

[37] DOBREA D V, BIRSAN D, FETECAU C, PALADE L I, BIRSAN I G. Experimental and numerical analysis with MSC Marc Software for the characterization of two-component moulded parts [J]. Materiale Plastice, 2012, 49(4): 242-248.

[38] IMSIR C, GUR C H. A FEM based framework for simulation of thermal treatments: Application to steel quenching [J]. Computational Materials Science, 2008, 44(2): 588-600. DOI: 10.1016/j.commatsci.2008.04.021.

[39] LANDKAMMER P, STEINMANN P. A non-invasive heuristic approach to shape optimization in forming [J]. Computational Mechanics, 2016, 57(2): 169-191. DOI: 10.1007/s00466-015-1226-2.

[40] QUAN Guo-zheng, ZOU Zhen-yu, ZHANG Zhi-hua, PAN Jia. A study on formation process of secondary upsetting defect in electric upsetting and optimization of processing parameters based on multi-field coupling FEM [J]. Materials Research, 2016, 19(4): 856-864. DOI: 10.1590/1980-5373-MR-2015-0678.

[41] LI Ju-qiang, LIU Juan, CUI Zhenshan. Characterization of hot deformation behavior of extruded ZK60 magnesium alloy using 3D processing maps [J]. Materials & Design, 2014, 56: 889-897. DOI: 10.1016/j.matdes.2013.11.037.

[42] WU C, KIM J W. Analysis of welding residual stress formation behavior during circumferential TIG welding of a pipe [J]. Thin-Walled Structures, 2018, 132: 421-430. DOI: 10.1016/j.tws.2018.09.020.

[43] PANTOUSA D, TZAROS K, KEFAKI M A. Thermal buckling behaviour of unstiffened and stiffened fixed-roof tanks under non-uniform heating [J]. Journal of Constructional Steel Research, 2018, 143: 162-179. DOI: 10.1016/j.jcsr.2017.12.018.

[44] IACS. Common structural rules for double hull oil tankers. International Association of Classification Societies [S]. 2010.

[45] IACS. Common structural rules for bulk carriers. International Association of Classification Societies [S]. 2010.

[46] IACS, Harmonization Project Team 2. Non-linear finite element collapse analyses of stiffened panels procedure description [S]. International Association of Classification Societies; 2009.

[47] PAIK J K, KIM B J, SEO J K. Methods for ultimate limit state assessment of ships and ship-shaped offshore structures: Part II stiffened panels [J]. Ocean Engineering, 2008, 35(2): 271-280. DOI: 10.1016/j.oceaneng.2007.08.007.

[48] FAULKNER D. Review of effective plating for use in the analysis of stiffened plating in bending and compression [J]. J Ship Research, 1975, 19: 1-17.

[49] GHAVAMI K, KHEDMATI M R. Numerical and experimental investigations on the compression behaviour of stiffened plates [J]. Journal of Constructional Steel Research, 2006, 62(11): 1087-1100. DOI: 10.1016/j.jcsr.2006.06.026.

[50] GORDO J M, SOARES C G. Compressive tests on short continuous panels [J]. Marine Structures, 2008, 21(2, 3): 113-137. DOI: 10.1016/j.marstruc.2007.12.005.

[51] GORDO J M, SOARES C G. Compressive tests on long continuous stiffened panels [J]. Journal of Offshore Mechanics and Arctic Engineering, 2012, 134(2): 021403. DOI: 10.1115/1.4004517.

(Edited by HE Yun-bin)

中文导读

基于集合的船舶加筋结构参数化建模、屈曲和极限强度预测

摘要：船体结构屈曲分析是其安全性评估的重要环节但步骤繁杂耗时，船舶结构设计领域迫切需要一种准确而简便的分析方法或工具。本文采用非线性有限元方法对加筋壁板的物理建模、屈曲分析和极限强度预测进行研究。考虑壁板初始缺陷，建立了整体加筋壁板的非线性有限元分析模型，提出了一种壁板后屈曲问题求解的建模和分析规范。基于MSC.Marc软件平台，开发了一种基于集合的壁板参数化建模和屈曲分析的软件系统。采用不同类型的船体结构加筋壁板，研究了壁板线性屈曲及后屈曲行为，并对非线性有限元求解屈曲问题的有效性进行了评估。将解析法、实验测试法以及本文所提出方法进行后屈曲分析所获得的结果对比表明，本文提出的壁板屈曲分析方法和开发的船舶结构屈曲分析软件系统，能够较准确地预测带有初始缺陷的壁板的极限强度。

关键词：屈曲；极限强度；加筋壁板；参数化建模；船舶结构

Foundation item: Projects(51575535, 51805551) supported by the National Natural Science Foundation of China; Project (ZZYJKT2018-15) supported by the of State Key Laboratory of High Performance Complex Manufacturing, China; Project (2015CX002) supported by the Innovation-driven Plan in Central South University, China; Project(2018BB30501) supported by the Key R&D Program of Liuzhou City, China

Received date: 2018-06-17; Accepted date: 2019-03-01

Corresponding author: PAN Qing, PhD; Tel: +86-731-888876164; E-mail: panqing0905@csu.edu.cn; ORCID: 0000-0002-3445-3281