Optimization and Scaling of Electron Beam Freeform Fabrication (EBF3) Panels

 

First Quarterly Report

 

Rakesh. K. Kapania, Jing Li, and H. Kapoor

Department of Aerospace and Ocean Engineering

Virginia Polytechnic Institute and State University

Blacksburg, VA 24061-0203

Email: rkapania@vt.edu

 

November, 2004

 

*     Background

Researchers in the Materials and Thermal Structures Branch at the NASA Langley Research Center in Hampton, VA, are exploring advanced metal manufacturing methods for rapid prototyping, fabrication and repair of aerospace structures. Electron beam freeform fabrication (EBF3) is a layer addition technique that produces complex, unitized, structural metallic parts with strengths comparable to that of wrought product, directly from computer-aided design (CAD) data. Since the EBF3 process is digitally controlled, EBF3 can be used to perform repairs in remote locations, and it offers the potential for reductions in part manufacturing costs and weight, and increased material processing performance to enhance mission success for aircraft, launch vehicles, and spacecraft.

However, before this vision can be realized a number of technical issues related to the computational modeling and optimization of the fabrication process, practical applications, and the relationship between an application and the selection of parameters that impact the quality of the process must be addressed. The proposed work here is a step in that direction. We propose starting a joint VT/IALR/Langley integrated analysis/design/prototyping research program of complex structures. As a first step, the team will focus on following technical challenge: (I) integrated stiffened aluminum and titanium plates for aircraft structural panels subjected to complex in-plane and out-of-plane loads, and (II) implement these designs using some of the RPT capabilities available at IALR and Danville Community College.

The team at Virginia Tech will consist of Dr. Rakesh K. Kapania, and two graduate students. Dr. Don Moffitt of the Institute of Advanced Learning and Research will act as a liaison between Virginia Tech and The Dan River Community College.

1.      Functionally Graded, Optimally Stiffened Panels

 

Stiffened panels are used in aerospace structures to reduce weight.  But most of the stiffened plates have used stiffeners in the two mutually orthogonal constant directions, available manufacturing approaches coupled with existing computational capabilities, in hardware and software, preclude any other option.  Earlier these directions used to coincide with the length and breadth of the plate.  However, there are now some examples of stiffeners being placed in geodesic fashion depending upon the loads that are applied to the panel.  An example is some of the personal basketball boards. Some recent research on composite structures has shown that fibers placed in a continuously varying orientation can further improve the performance of a composite panel or reduce the weight for the same performance.  Similar improvements in the behavior of stiffened isotropic panels are now possible, thanks to the availability of EBF3.

 

We will investigate the optimal design of stiffened panels by allowing the stiffeners to have continuously varying properties such as orientation, thickness, width, and material properties (see Fig. 1).  These are  the design variables that earlier studies have kept constant because of manufacturing constraints.  By continuously varying the stiffener orientation, we can align the stiffeners along the load paths for the static case and in a way that can drive the natural frequencies away from the resonance frequencies for a dynamic case.  The biggest difficulty in such an optimization is to how to express the orientation of a curvilinear stiffener as a design variable.

 

We have faced a similar problem in our design of a sensor for a smart bed, being designed for retirement homes, where a fiber-optic cable of a given length needs to be placed in a curved fashion so as to increase its sensitivity to a patient’s movement.  We overcame this problem, by expressing the placement of fiber-optics cable using non-uniform rational B-splines (NURBS).  The control points of the NURBS represent the design variables.  Both standard optimization algorithms and genetic algorithms are being used.  The former are faster but prone to giving results that may not be a global minimum while the latter are very slow but can yield a global minimum with a significantly greater probability.  In solving the optimization problem at hand, we need to ensure that the radius of curvature of the stiffener, at some points, may not become too small. 

 

In addition to the orientation, we will investigate the use of materials with different Young’s modulus and densities for a stiffener.  Here we envision a material with one value of Young’s modulus near the plate and another value as we go away from the plate to ensure that the natural frequencies are away from the resonance frequencies.  This is a form of a functionally graded material.  Other design variables will be height and width of the stiffeners.

 

Throughout this research, efforts will be made to develop scaling parameters that will enhance the value of the present research for panels that have arbitrary dimensions, curvatures and loads.

 

2.      USING RAPID PROTOTYPING CAPABILITIES AT DANVILLE

 

 The optimal designs arrived at in the previous two applications will be evaluated for their ability to be fabricated using the processes available at the Danville Community College (DCC)/Regional Center for Applied Technology and Training (RCATT).  The two graduate students who would work on the two application problems will spend at least three months at Danville to ensure that the CAD (Computer-Aided Design) files work adequately on the processes available at DCC before they are sent to the NASA Langley Research Center for EBF3 processing.

 

 

Interaction with Langley: 

 

We plan to have a continuous interaction with Karen Taminger and other researchers at Langley by using the communication power of the Internet.  We will have a monthly Telecon and will make a presentation over the internet.  The slides will be placed on a secured web site and will be available to NASA Engineers before the meetings.

 

  Key techniques and progress

Here is a summary for the first quarterly achievements and progress:

·        NURBS representation for both the stiffeners and plate of a panel

·        Triangulation mesh generation using DistMesh

·        Finite element analysis and structural optimization via MATLAB/NASTRAN interface

·        Size (cross-sectional dimensions) optimization for fixed orientations and curvatures of stiffeners

·        p-method via h-method investigation

1.     NURBS representation both the stiffeners and plate of a panel

NURBS (Non-uniform rational B-Splines) has already been a standard for CAGD (computer aided geometry design).  Our main reference in this topic is one of the most used textbooks, Curves and Surfaces for Computer Aided Geometric Design: A Practical Guide, by G. Farin [1] .

·        Smart bed example

We have used the NURBS to represent the placement of the fiber optic sensor, the deformed and un-deformed mattress surfaces as well as body pressure distribution for a smart bed (Fig. 2) [2]. The locations of the control points of the NURBS curve for the fiber optic sensor are design variables. The objective is to find a placement of the fiber optic sensor so as to maximize the integrated norm-2 curvature change of the fiber curve due to a patient’s movement on the bed mattress.  The constraint is placed on the length and initial curvature of the fiber optic curve.

Figure 3 shows an example of the placement optimization of the fiber optic sensor using GA, implemented as the Java Design Tool for the Fiber Optic Sensors for the Integrated Smart Bed. The cyan curve is the initial fiber curve while the white dots of the polygon are the control points of the NURBS for the initial fiber curved. The yellow curve is the deformed fiber curve, which is determined by the bilinear interpolation from the mattress surface grid points.

·        Blade stiffened panel of EBF3

While we can borrow certain ideas from the smart bed work, we decided to give up using Java language to program in current work. Instead, we are using MATLAB, which has many useful MATLAB tool boxes (e.g. Spline Toolbox and Optimization Toolbox), as the main programming language to develop the interfaces between a user and computer and between a user and other application software, such as MSC.NASTRAN or ANSYS.

Though the Spline Toolbox in MATLAB has the capability to represent NURBS, it is not in the convenient form as used by most CAGD packages.  Therefore, we choose the NURBS Toolbox by D.M. Spink [3].

As shown in Fig. 4 and 5, the axes of stiffeners (blue curves) are represented by NURBS curves, where the control points (red circles) determine the placements of the stiffeners.

While the ends of stiffeners can be arbitrary positions within and on the plate boundary, we choose to place the ends of the stiffeners on the boundary edges (Fig. 5) to avoid the undesirable stress concentration problem due to a sudden stiffness change. The green circles in the Fig. 5 are the prescribed boundary points. Both end control points and inner control points of the stiffener curves are generated randomly and automatically to demonstrate the freedom of the stiffened panel representation using NURBS.

In addition, the curvilinear mid-surface of the panel can also be represented by NURBS, as shown in Fig. 6. The surface is determined by the red control points.

Finally, the width and height distributions along the axes of the curved stiffeners are also described using NURBS, see Fig. 7.

 

 

 

 

 

 

 

 

2.     Mesh generation and 3-D thickness display

Automatic mesh generation during optimization has been one of our most important concern for this stiffened panel optimization problem, where both cross-sectional sizes and placements or orientations of the stiffeners as design variables.

For size optimization, automation in mesh generation is not a necessity because one time satisfactory meshing can be used in the whole process of the optimization.

For placement optimization of stiffeners, however, the mesh grid points keep changing, at least in grid point positions. Sometimes, re-meshing is dispensable or advisable.

Our previous work on the smart bed includes dealing with a similar problem, where an optimal placement of the fiber optic curve needed to be found. As the stiffness contribution of the fiber optic cable to the mattress model is too small, the fiber is treated as absolutely flexible. This allows us to use a very coarse rectangular mesh for the mattress, and the curve points of the fiber are not required to coincide with those of the mattress (Fig. 8a). The deformed fiber curve is determined from the deformed mattress surface by an approach similar to the bilinear interpolation from the grid points of the mattress surface.

For the stiffened panel work, however, the stiffeners are attached mainly to provide the structural support for thin and easily deformed plate so that both the load carrying capability and natural vibration frequency of the panel are increased; thus, the stiffness of the stiffeners cannot be ignored.

First, we may generate dense mesh for plate and align the grid points of stiffeners to coincide with those of the plate (Fig. 8b). This approach may not apply to the problem at hands when the eigen-problems for buckling and vibration frequency are to be solved.

Second, we may choose to align the gridlines of the plate as shown in Fig. 8c so that all of the stiffener grid points coincide with the grid points of the plate for a given stiffener meshing. This will lead to an extremely non-uniform mesh. We can release this problem by first aligning the grid points  to some prescribed mesh grids such as in Fig. 8b but with a much less density, and then move back to previous locations after generating the gridlines that pass all the grid points for stiffeners. Moving mesh grid points is a necessity to get a more uniform mesh. Some further work, including literature review, needs to be done for moving rectangular mesh.

Third, we may choose to use coarse mesh for both plate and stiffeners. A grid point of a stiffener can be either on the gridline(s) of plate mesh or within a rectangular element, as also seen in Fig. 8a. Then, special rectangular plate elements with extra mid-side grid points and inner grid points are needed. The most popular rectangular plate elements, such as 8-noded or 9-noded, will work when the grid point of the stiffeners are apart enough.  There is a limitation to use this kind of element, such as 8-noded element, because it is suggested that the mid-side node location on an edge be on middle 1/3 edge length. To remove this limitation, moving mesh is also a necessity.

Higher order or p-version of elements is one of our concerned via h-version elements. “One of the main applications of p-version elements is detailed stress analysis. The p-elements have higher-order polynomials, which provide better representation of complex stress fields. For these complex stress fields, the geometry, loads, and boundary conditions must be represented accurately. This includes modeling fillets instead of sharp corners, distributed loads and constraints instead of point loads and constraints, etc. A more detailed model leads to more detailed results. p-elements have several modeling advantages. With the higher-order polynomials, the geometry and loads can be represented more accurately. Generally, fewer p-version elements with curvature than h-version elements with straight edges are required. The accuracy of the analysis is controlled primarily by the polynomial level, not by the element size. Generally the user needs to only use the minimum number of elements necessary to adequately model the geometry, independent of expected result characteristics. Polynomials levels can then be assigned based on areas of the model in which the user is interested, and areas of the model in which the user is not. (Of course the same polynomial level can be assigned everywhere for a minimum of user involvement, but this is not as efficient.) If a more accurate answer is necessary, the polynomial levels can be increased, either manually by the user or automatically by the program, until the answers reach the specified accuracy, without changing the mesh. Adding degrees-of freedom until the error decreases to a specified level is known as adaptivity. By adding higher-order polynomials instead of refining the mesh, a faster rate of convergence, and therefore fewer iterations, can be achieved.”[5]

A comprehensive literature review on automatic mesh generation has  not been made yet as we focus on the availability of the mesh generation software. Reference 4 gives the link to a summary of different mesh generation software, their capability, and source code availability, of which the DistMesh - A Simple Mesh Generator in MATLAB developed by Gilbert Strang and Per-Olof Persson from Department of Mathematics at Massachusetts Institute of Technology is our first choice due to the following reasons:

·        Source code in MATLAB is available as free software

·        The code is short and simple and easy to be used and modified

·        The mesh quality is mostly acceptable

DistMesh generates unstructured triangular and tetrahedral meshes! It uses a special distance function to describe the relationship between a point and the boundary of the domain, Delaunay function in MATLAB to generate triangular mesh, and move the mesh by solving a truss equilibrium problem while some prescribed grid point locations can be fixed. This gives us the freedom first to generate arbitrary grid points of stiffeners’ axes, and then generate the triangular mesh for plate so that the grid points for stiffeners are part of grid points for the plate.

Figure 9a shows an example of triangulation meshing using DistMesh, modified to curry our current requirements. The mesh does not look very nice as it is a very coarse mesh with unevenly distributed grid points of the four curved stiffeners for mesh distortion testing.  The mesh with high quality can be obtained when the mesh density is increased and relatively uniformly distributed grid points for stiffeners are given.

For convenience, the consistence or continuity between stiffeners and plate are enforced only by the connection of grid points. Therefore, we allow two consecutive or adjacent grid points of a stiffener to jump over several plate elements. For the same reason, the intersections among stiffeners or a stiffener itself are not calculated or connected by grid points. That is, stiffeners can overlap or penetrate with each other.

The finite element mesh for a curvilinear stiffened panel, as seen from Fig. 1, can be simply mapped or deformed from a reference flat stiffened panel with similar geometric mid-surface dimensions. This is easily implemented using NURBS representation for both flat and curved plate.

It is noticeable that Figs. 1, 6 and 7 display both plate and stiffeners with thickness. MATLAB provides a good graphical interface and rendering implementation. Its patch function provides a means for solid body display. We implement the thickness display using mid-surface, its boundary and normal, and thickness information to build up big patches for top surface, bottom surface, and side surface (s) of the solid body, either plate or stiffeners. Each of the big patches is composed of many small triangular or rectangular patches. We wrote a small package of about a dozen of MATLAB functions to implement the 3-D thickness display. It will be very helpful and pleasant to visualize the stiffener placements and cross-sectional size variations.

3.     Finite element analysis and structural optimization

MSC.NASTRAN and/or ANSYS are used for response analysis, design sensitivity analysis, and optimization, in the first stage. The Optimization Toolbox in MATLAB will be used for placement optimization while response and design sensitivity analyses are performed using MSC.NASTRAN and/or ANSYS. Working on a finite element software in MATLAB is also an option, which can speed-up the over all procedure. Repeatedly calling external software, such as NASTRAN, may be time consuming.

A MATLAB/MSC.NASTRAN interface is being developed for the stiffened panel optimization. We decided to create this interface for the following reasons:

·        MATLAB is not only an easy to learn programming language, but also has included most useful tool boxes for numerical simulation and graphical displaying

·        Application software (including NASTRAN, ANSYS, etc.) in other popular languages, such as, FORTRAN, C, JAVA, etc., can be executed as external functions in MATLAB environment

·        The NURBS tool is freely available in MATLAB version and easily implemented

·        Automatic mesh generator, such as DistMesh, is freely available in MATLAB

·        NASTRAN and/or ANSYS have been standards for structural analysis and optimization, but lacking or weak on NURBS representation and flexible programming

With the MATLAB/MSC.NASTRAN interface, a user can easily define the design problems and create Bulk Data file for MSC.NASTRAN to perform response analysis, and optimization. It also takes NASTRAN itself as external function, invokes it, and read the results from NASTRAN output to display and further process in the MATLAB environment.

The elements considered for NASTRAN will include CTRIA, CQUAD, for 2-D component modeling (e.g. plate and thin-walled stiffeners), CBAR and CBEAM for 1-D component modeling (thick and thin-walled stiffeners when warping is not an issue).

Similarly, MATLAB/ANSYS interface will be developed, when it is deemed necessary.

The following are some selective examples we have run through to illustrate and test our current capability and understand the problems at hands.

3.1  Response analysis examples

 

3.1.1        Elastic stability of a plate

This example is adopted from http://www.mscsoftware.com/support/online_ex/Nastran/Nas101/AppendixH.pdf, used for

       1) Testing of NASTRAN data created

       2) Testing of mesh distortion as shown in Fig. 9a, due to introduction of the four stiffeners.

The model is described as follows:

       1) Find the unit critical compressive stress of a flat rectangular plate. (The elements of stiffeners are not included.)

       2) Equal uniform compression of 6.89E+5 Pa on two opposite (short) edges.                                

       3) All edges are simply supported.

 4) Model properties are given in Table 1. 

The result in Fig. 9b and many other testing results show that for buckling load, the mesh distortion due to the introduction of the stiffeners is trivial. The mesh generator DistMesh works fine.

3.1.2        Natural frequency of a plate

3.1.3        Stress analysis of a plate

3.2  Structural optimization examples

In the examples that follow, the typical material properties will be refereed from Table 2.

The geometrical dimensions, boundary loading and support conditions are denoted in Fig. 10 for a planar panel.

a and b is the lengths of the panel in X and Y-directions, respectively; t is the thickness of the plate, w and h are the width and height of a stiffener’s cross-section.

Nx and Ny are the in-plane normal load densities in X and Y -directions, respectively; Qxy is the shear load density. The in-plane load density is in the term of load per unit length. The out-plane load can also be added though it is not denoted in the figure.

Though it is not very noticeable in Fig. 10, along boundary of the mid-surface of the plate are prescribed boundary fixed points. The number of boundary fixed grid points can be prescribed for each of the four numbered edges. The ends of every stiffener are connected to those boundary points. Therefore, the meshes for both plate and stiffeners are generated based on those prescribed boundary information. By default, the grid points are set to be uniformly distributed on each edge, but it is not a necessity.

Internally, the boundary fixed points are numbered along edge 1 from the corner between edges 4 and 1 to the corner between edges 1 and 2, then along edge 2 to the corner between edges 2 and 3, then along edge 3 to the corner between edges 3 and 4, finally along edge 4 to the corner between edges 3 and 1. That is, the counting order follows the right-hand screw rule, with the thumb pointing in the direction of the normal of the mid surface of the plate, but starting from the corner between edges 4 and 1.

Externally, however, it is convenient to give a location of a boundary fixed point by a number pair for each edge.  For edge 1, count the fixed points from edge 2; for edge 2, count from edge 1; for edge 3, count from edge 2; and for edge 4, and count from edge 1. Note that does not follow the right-hand screw rule this time but in positive X or Y direction!

For documentation purpose and also for better understanding the examples that follow, we take Fig. 9a as an example to illustrate an approach how we can handle placement/orientation optimization for stiffened panels.

Let Nbfix1, Nbfix2, Nbfix3, and Nbfix4 be numbers of fixed points on edge 1, 2, 3, and 4, respectively. Let Nbfix be the total number of boundary fixed points.

·        Nbfix1 = 10; Nbfix2 = 15; Nbfix3 = 10; Nbfix4 = 15;

·        Nbfix = Nbfix1 + Nbfix2 + Nbfix3 + Nbfix4 - 4;

Let EID be edge ID and i be ith fixed point on edge EID. Then, the connection between (EID, i) and internal ID I is,

·        For EID = 1, i = 1 to Nbfix1, I(EID, i)  = Nbfix1 – i +1 ;

·        For EID = 2, i = 1 to Nbfix2, I(EID, i)  = Nbfix1 + i – 1;

·        For EID = 3, i = 1 to Nbfix3, I(EID, i)  = Nbfix1 + Nbfix2 – 1 + i - 1;

·        For EID = 4, i = 2 to Nbfix4, I(EID, i)  = Nbfix1 + Nbfix2 – 1 + Nbfix3 – 1 + Nbfix4 -2  - i + 2;

·        For EID = 4, i = 1, I(EID, i)  =1.

Now, we illustrate how to represent the stiffeners’ boundary layout by its end points’ locations on the boundary edges.

Let (EID1 i1; EID2 i2;)st denote the edge location of the first (EID1 , i1) and second (EID2 , i2) end points, respectively on the boundary edges, for stiffener st, and put all edge locations of the stiffeners (four of them, for example,) in a column, we get a stiffener layout representation like

Edgelocation = [(EID1 i1; EID2 i2;)1

  (EID1 i1; EID2 i2;)2

  (EID1 i1; EID2 i2;)3

  (EID1 i1; EID2 i2;)4]

Therefore, the stiffeners’ boundary layout for Fig. 9a is

Edgelocation = [ 1    5;   4  12;

   1    7;   3    5;

   2    6;   2  12;

   2  13;   3  10;]

To summarize, the boundary layout for any stiffened panel as described in Fig. 10 can be determined by the numbers of fixed points on four edges [Nbfix1 Nbfix2 Nbfix3 Nbfix4] and the stiffeners’ boundary edge location Edgelocation. Note that when the boundary fixed points are dense enough, we have got a layout representation for any placement/orientation of (straight) stiffeners for any stiffened panel. When mid control points are added for stiffeners, curved stiffeners with any placement/orientation are also represented.

3.2.1        Size optimization of a blade stiffened plate

A general design description for a given stiffened panel layout, planar dimensions of the plate, a and b, and the materials of the plate and stiffeners:

1.      Find the uniform thickness t of the plate, and the width and height distributions of a stiffener st, (w h)st along the stiffener’s axis,

2.      to minimize the weight of the blade stiffened panel,

Objective = weight

3.      subjected to the minimum buckling load factor constraint,

λ   λa (llowable),

and von-mises stress constraint on plate,

σvon-mises σa (llowable),

and side constraints on size design variables,

tminttmax,

wstminwstwstmax,

hstminhsthstmax

 

At this time, the size optimization with variable cross-sections is implemented element-wisely by taking the width and height of the cross-section independent from those of rest of the elements for stiffeners while assuming a uniform cross-section within an element. The optimization results at grid points will be smoothed by taking the average of values of the adjacent elements. The variable linking is not considered. The number of design variables will be very large and the convergence may be hard and slowed down. This limitation may be removed using NURBS representation for the cross-sections and using CBEAM or CQUAD element, instead of CBAR. It will be implemented when the optimization is performed within MATLAB environment.

Example 1.  Regular grid fashion – larger spacing of stiffeners. Uniform via variable cross-section of a stiffener is studied.

Planar dimensions and materials of a stiffened panel are given in Table 3. Layout (201) and edge locations of stiffeners' ends are given in Table 4. Initial sizes and bounds of cross-sectional dimensions are given in Table 5.

For a/b=1, simply supported on four edges, the material properties in Table 2, the critical stress due to buckling, with the compression on edges 1 and 3, is [6]

σcr = k π2E(t/b)2/(1 – υ2)

     = 4 π2 70 GPa (0.005/2.54)2/(1 – 0.332)

      =1.0014 MPa;

The unit pressure load density is chosen

            P0 = [Nx0; Ny0; Qxy0]; Nx0 = σcr t = 5.0072e+003 N/m; Ny0 = 0; Qxy0 = 0;

The actual load is obtained by multiplication of a load factor λ

P = λ P0

The allowable minimum buckling loads considered are included in the following array

λa = [0.5 1. 5. 10. 15. 20. 25. 30. 35. 40. 45. 50.];

The design optimization parameters used in NASTRAN is normally

$---1---|---2---|---3---|---4---|---5---|---6---|---7---|---8---|---9---|--10---|

$       Design Optimization Parameters

$DOPTPRM PARAM1 VAL1 PARAM2 VAL2 PARAM3 VAL3 PARAM4 VAL4

$

DOPTPRM       P2      15  DESMAX     25    DELP     0.5    GMAX   0.005

          CONVDV  0.0005  CONVPR  0.0005      P1       1

If there is a convergence is not achieved, DELP is set to 0.5. The maximum allowed design cycles DESMAX is extended to 50 in some cases.

This set of parameters is used thru all the examples that follow.

The scale of the design problem is as follows:

NUMBER OF GRID POINTS = 375

NUMBER OF CBAR ELEMENTS = 64

NUMBER OF CTRIA3 ELEMENTS = 688

NUMBER OF DESIGN VARIABLES = 129 (9 for uniform case)

RUN TERMINATED DUE TO HARD CONVERGENCE TO AN OPTIMUM AT CYCLE NUMBER =   21.

The 3-D display with thickness in Fig. 11b gives much better vision than in Fig. 11c.

By examination of NASTRAN f06 file, we find that only buckling load constraint is active in all buckling constraint levels. Also see Fig.  11d.

A little benefit can be observed for the larger spacing of stiffeners from Fig. 11e using variable cross-sections of stiffeners. The minimum weight under buckling load constraint level 10 seems much lower than the expected from other part of the results. It might be due to the hard convergence of the problem itself. Different initial values of design variables should be used for a stable result.

 

 

 

Example 2.  Regular grid fashion – smaller spacing of stiffeners. Uniform via variable cross-section of a stiffener is studied.

Planar dimensions and materials of a stiffened panel are given in Table 3. Layout (207) and edge locations of stiffeners' ends are given in Table 6. Initial sizes and bounds of cross-sectional dimensions are given in Table 5.

The loading is chosen as the same as in Example 1. It is a longitudinal load.

The allowable minimum buckling loads considered are included in the following array

λa = [1.  10. 20. 30. 40. 50.];

The scale of the design problem is as follows:

NUMBER OF GRID     POINTS = 425

NUMBER OF CBAR ELEMENTS = 80

NUMBER OF CTRIA3 ELEMENTS = 786

NUMBER OF DESIGN VARIABLES = 161 (11 for uniform case)

RUN TERMINATED DUE TO HARD CONVERGENCE TO AN OPTIMUM AT CYCLE NUMBER = 17.

The 3-D display with thickness in Fig. 12b gives much better vision than in Fig. 12c.

By examination of NASTRAN f06 file, we find that only buckling load constraint is active in all buckling constraint levels. Also see Fig.  12d.

A little more benefit can be observed for smaller spacing of stiffeners from Fig. 12e using variable cross-sections of stiffeners. The minimum weights under buckling load constraint level 40 and 50 seem much lower than the expected from other part of the results. It might be due to the hard convergence of the problem itself. Different initial values of design variables should be used for a stable result.

 

Example 3. Geodesic fashion – larger spacing of stiffeners. Uniform cross-section of a stiffener is considered.

Planar dimensions and materials of a stiffened panel are given in Table 3. Layout (212) and edge locations of stiffeners' ends are given in Table 7. Initial sizes and bounds of cross-sectional dimensions are given in Table 5.

The loading is chosen as the same as in Example 1. It is a longitudinal load.

The allowable minimum buckling loads considered are included in the following array

λa = [1.  10. 20. 30. 40. 50.];

The scale of the design problem is as follows:

NUMBER OF GRID POINTS   = 379

NUMBER OF CBAR ELEMENTS = 68

NUMBER OF CTRIA3 ELEMENTS = 696

NUMBER OF DESIGN VARIABLES = 9

RUN TERMINATED DUE TO HARD CONVERGENCE TO AN OPTIMUM AT CYCLE NUMBER = 24.

The 3-D display with thickness in Fig. 13b gives much better vision than in Fig. 13c.

By examination of NASTRAN f06 file, we find that only buckling load constraint is active in all buckling constraint levels. Also see Fig.  13d.

The minimum weight under buckling load constraint level 10 seems much lower than the expected from other part of the results. It might be due to the hard convergence of the problem itself. Different initial values of design variables should be used for a stable result.  See Fig. 13e.

A little higher weight can be observed for geodesic stiffeners than regular grid ones as in Fig. 11e of example 1, due to the longitudinal loading condition.

 

 

 

Example 4.  Geodesic fashion – smaller spacing of stiffeners. Uniform cross-section of a stiffener is considered.

Planar dimensions and materials of a stiffened panel are given in Table 3. Layout (211) and edge locations of stiffeners' ends are given in Table 8. Initial sizes and bounds of cross-sectional dimensions are given in Table 5.

The loading is chosen as the same as in Example 1. It is a longitudinal load.

The allowable minimum buckling loads considered are included in the following array

λa = [1.  10. 20. 30. 40. 50.];

The scale of the design problem is as follows:

NUMBER OF GRID     POINTS = 436

NUMBER OF CBAR ELEMENTS = 90

NUMBER OF CTRIA3   ELEMENTS = 806

NUMBER OF DESIGN VARIABLES = 13

RUN TERMINATED DUE TO HARD CONVERGENCE TO AN OPTIMUM AT CYCLE NUMBER = 33.

The 3-D display with thickness in Fig. 14b gives much better vision than in Fig. 14c.

By examination of NASTRAN f06 file, we find that only buckling load constraint is active in all buckling constraint levels. Also see Fig.  14d.

The minimum weights under different buckling load constraint levels seem much smoother than previous examples.  See Fig. 14e. A little lower weight can be observed for smaller spacing of stiffeners than in Fig. 13e of example 3.

 

Example 5. Geodesic fashion – large spacing of curved stiffeners. Uniform cross-section of a stiffener is considered.

Planar dimensions and materials of a stiffened panel are given in Table 3. Layout (2120) and edge locations of stiffeners' ends are given in Table 9 the same as (Table 7).  There is one middle control point for each NURBS curve of the stiffeners’. The four middle points are generated randomly. Initial sizes and bounds of cross-sectional dimensions are given in Table 5.

The loading is chosen as the same as in Example 1. It is a longitudinal load.

The allowable minimum buckling loads considered are included in the following array

λa = [1.  10. 20. 30. 40. 50.];

The scale of the design problem is as follows:

NUMBER OF GRID POINTS = 379

NUMBER OF CBAR ELEMENTS = 68

NUMBER OF CTRIA3 ELEMENTS = 696

NUMBER OF DESIGN VARIABLES = 9

RUN TERMINATED DUE TO HARD CONVERGENCE TO AN OPTIMUM AT CYCLE NUMBER = 12.

The 3-D display with thickness in Fig. 15b gives much better vision than in Fig. 15c.

By examination of NASTRAN f06 file, we find that only buckling load constraint is active in all buckling constraint levels. Also see Fig.  15d.

The minimum weights under different buckling load constraint levels seem smooth.  See Fig. 15e. A little higher weight can be observed for curved stiffeners than straight ones as in Fig. 13e of example 3, possibly due to the uniform load density along boundary edges.

 

4.     Conclusions

We have initially achieved the following at this time:

·        Successfully represent the planar and curvilinear stiffened panel using NURBS.

·        Finite element mesh generation is initially investigated and a mesh generator DistMesh - A Simple Mesh Generator in MATLAB is obtained and modified for triangulation meshing that can include arbitrarily curved stiffeners.

·        A MATLAB/NASTRAN interface, along with a thickness display package, is developed and still under development for the panel definitions, automatic mesh generation, NASTRAN data generation, NASTRAN invoking, and for reading and displaying response analysis and optimization results from NASTRAN output files.

·        Sizing optimization for a planar stiffened panel is tested for different given layouts (orientations and curvatures) of stiffeners under longitudinal compression load.

·        pmethod (via h – method) is being studied, which will be very important useful  to keep the model small even when stress gradient is large and stress constraint is active. The implementation environments are investigated under ANSYS and NASTRAN. It is found that p-method is not yet implemented for eigen-problems in ANSYS. On the other hand, NASTRAN has implemented the p-method at least for solution sequence 101 and 103, that is, both static and normal modes. Among the elements we are concerned here for NASTRAN, CTRIA, CQUAD, and CBEAM have p-method versions. Design sensitivities and optimization with p-method in NASTRAN is available for stress constraints, not implemented for buckling constraint yet.

1.     Future work

Our current success in above is only initial one in every aspect, and subjected to testing and modification, and improvement so that it can be user-friendly, efficient, and robust.

Specifically, we will address the following in the next quarters.

·        Further modify the DistMesh so that it can both generate fine mesh and be robust.

·        Further review literature about finite element meshing, especially for quadrilateral elements for p-methods.

·        Customize the thickness display package so that is can be used for p-methods and implanted to other applications.

·        Increase the capability of the MATLAB/NASTRAN interface so that it can handle more elements (CQUAD, CBEAM, etc.), responses (displacements, stresses, and design sensitivities) and user-friendly (easily to be used by anyone rather than programmer himself). Especially, it needs to be able to handle multiple cases, and read the results from any design cycles. It will also be extended to p-version elements.

·        Testing examples will include different boundary conditions, and loading cases, as well as materials. Size optimization for curvilinear panel will be performed. Optimization considering natural frequency will also be tested.

·        The placement/orientation optimization methods and implementation will be further investigated.

·        The p-method, relevant meshing, implementation environment will be further tested, and investigated.

·        The necessity of creating a MATLAB/ANSYS interface will be studied.

·        The necessity and possibility to implement the structural analysis and optimization uniquely in MATLAB without using other external software will be considered.

*     References

 

1.      G. Farin: “Curves and Surfaces for Computer Aided Geometric Design: A Practical Guide”. 2nd Ed. Academic Press, Inc., 1990.

2.      J. Li, R.K. Kapania, W.B. Spillman, Jr.: “Placement Optimization of Fiber Optic Sensors for a Smart Bed Using Genetic Algorithms”. Paper AIAA-2004-4334, 10th AIAA/ISSMO Multidisciplinary Analysis and Optimization Conference, August 30–-September 1, 2004/Albany, NY USA.

3.      http://www.aria.uklinux.net/nurbs.php3

4.      http://www-users.informatik.rwth-aachen.de/~roberts/software.html

5.      MSC.NASTRAN 2004 Reference Manual

6.      http://www-math.mit.edu/~persson/mesh/

7.      N.W. Murray: “Introduction to the theory of thin-walled structures”. Clarendon Press – Oxford, 1984.

8.      MSC.NASTRAN 2004 Quick Reference Guide

9.      http://www.aoe.vt.edu/~jing/EBF3/

10.  http://www.mscsoftware.com/support/online_ex/Nastran/Nas101/AppendixH.pdf