Interactive Stiffened Panel Analysis (ISPAN) modules, written in FORTRAN, were developed to provide an easy to use tool for creating finite element models of composite material stiffened panels. The modules allow the user to interactively construct, solve and post-process finite element models of four general types of structural panel configurations using only the panel dimensions and properties as input data. Linear, buckling and post-buckling solution capability is provided. This interactive input allows rapid model generation and solution by non finite element users. The results of a parametric study of a blade stiffened panel are presented to demonstrate the usefulness of the ISPAN modules. Also, a non-linear analysis of a test panel was conducted and the results compared to measured data and previous correlation analysis

Dorris, William J.

Hairr, John W.

Ingram, J. Edward

Shah, Bharat M.

English

NASA Technical Reports Server

N95- 28846
ISPAN
INTERACTIVE STIFFENED PANEL ANALYSIS
A TOOL FOR
QUICK CONCEPT EVALUATION AND DESIGN TRADE STUDIES
b
John W. Hairr, William J. Dorris, J. Edward Ingram, and Bharat M. Shah*
Lockheed Aeronautical Systems Company
Marietta, Georgia 30063 <-
ABSTRACT
Interactive Stiffened Panel Analysis (ISPAN) modules, written in FORTRAN,
were developed to provide an easy to use tool for creating finite element models of
composite material stiffened panels. The modules allow the user to interactively construct,
solve and post-process finite element models of four general types of structural panel
configurations using only the panel dimensions and properties as input data. Linear,
buckling and post-buckling solution capability is provided. This interactive input allows
rapid model generation and solution by non finite element users. The results of a
parametric study of a blade stiffened panel are presented to demonstrate the usefulness of
the ISPAN modules. Also, a non-linear analysis of a test panel was conducted and the
results compared to measured data and previous correlation analysis.
INTRODUCTION
Stiffened panel analysis computer programs have been in existence for many years.
Typically, they are based on a combination of closed form solutions and a large data base
of metallic stiffened panel test results. Developing a similar analysis capability for
composite materials would be a formidable task due to the the lack of a complete composite
stiffened panel test data base and due to the complex failure modes resulting from material
anisotropy and variations in design/fabrication techniques. Closed-form solutions for the
complex failure modes and out-of-plane response characteristics of the composite materials
933
https://ntrs.nasa.gov/search.jsp?R=19950022425 2020-06-16T07:48:16+00:00Z
are being developed; have not demonstrated sufficient applicability and
accuracy. As finite element programs, and in particular, the pre- and post-processing
programs have matured, it has become apparent that a more practical alternative to the
closed-form solutions would be a non-linear finite element-based program which is user
friendly. That alternative is envisioned here as an interactive input module which functions
as an interface between the structures engineer and the f'mite element program (see Figure
1). The modules developed jointly at Lockheed Missiles and Space Company (LMSC) and
at Lockheed Aeronautical Systems Company (LASC) are referred to as ISPAN, for
Interactive Stiffened Panel Analysis.
Four user input/interface modules were developed; one each for flat and curved
stiffened panels, truss-core panels and geodesic stiffened panels. Each module prompts the
user for panel dimensions, properties, loads, boundary conditions and solution type
(linear, buckling or post-buckling). The data supplied are then used to automatically
prepare the finite element model. No knowledge of the finite element program commands
or data format is required of the user. A typical stiffened panel geometry and solution
procedure can be generated in a few minutes; solution time will obviously depend on the
computer. Once a panel problem has been defined, the data are saved to a file, so that any
changes to geometry, mechanical properties or loads may be accomplished by updating
this database file with the data only requiting the changes. This allows the data for
successive analyses be created in a fraction of the time required for the initial problem
definition. This operational efficiency is valuable in the trade study.
The functioning of ISPAN modules, as illustrated in Figure 2, is analogous to a
command module. In addition to interactively developing DIAL compatible geometry and
materials files from the user supplied data, it also establishes procedures to communicate
with the DIAL pre-processor, the solver, and post-processor. Thus it allows the user a
direct control over the overall problem solving.
The Lockheed developed DIAL finite element code was selected for use in ISPAN
because of its versatile non-linear and collapse analyses capability. DIAL also has very
powerful pre- and post-processors requiring a relatively few number of commands. While
the model generation data needed for DIAL is very concise, it is not intuitively obvious to
an analyst not already familiar with the DIAL code which commands and which options
should be used. Thus, if the structure to be analyzed is confined to a certain type, such as a
stiffened panel, DIAL lends itself well to an interface procedure such as ISPAN. The
934
DIAL code also features a capability called syntactic input, which is a FORTRAN-like
language that allows variable names for model data, and subroutines which use these
variables to construct model generation commands. Finally, DIAL maintains a database,
which contains model data, output data (internal loads, stresses, deflections, etc) and
information generated during a post-processing session.
PROGRAM CAPABILITIES AND LIMITATIONS
The ISPAN modules are presently capable of analyzing the panel types and general
cross-sections shown in Figure 3. The following list describes the options available to the
user in the four modules
Stiffener
Skin
Loading
- cross-section type
- number of stiffeners
- spacing (may be irregular)
- flange widths, thickness
- materials, ply orientation
- width, length and thickness
- materials, ply orientations
- axial end load, N x (tension or
compression)
- lateral load perpendicular to the stiffener
direction) Ny
- in-plane edge shear, Nxy
- normal pressure
935
Boundary
Conditions
- Each of the four panel edges may be specified
separately as free, simply-supported or
clamped.
- Vertical translations and/or rotations may also
be specified across the width of the panel to
simulate the fib/frame supports.
Solutions
- linear static
- bifurcation (buckling)
- post-buckling (arc length method)
DIAL Shell Element
All components of the stiffened panel models are constructed using a modified thick
shell element as shown in Figure 4. This element is an eight node, super-parametric,
doubly-curved thick shell element. The element was modified by separating the membrane,
bending and transverse shear responses, thus allowing the adequate representation of
both the laminate and the sandwich type structures. Linear, parabolic and cubic versions
of this element are available in DIAL. The parabolic and cubic shell elements are vastly
superior to the linear elements in terms of accuracy and are generally recommended. The
parabolic elements were selected for use in ISPAN to provide optimum accuracy for a
given level of complexity. An example of a typical flat, hat-stiffened panel model generated
by ISPAN is shown in Figure 5.
Although the stiffener elements are generally distinct from the skin elements, it
should be noted that the stiffener attach flanges are assumed to be included in the skin.
Therefore, elements in the stiffener attach flange region should be given thickness and
orientations which reflect the sum of the flange and skin in this region as indicated by the
shaded area in Figure 6.
The ribs (frames) are not modeled with structural elements in this analysis.
However, they are represented by constraints on the degrees of freedom at the rib
locations. The details of this are discussed in the sub-section on boundary conditions.
936
Loads
In-plane axial ( N x ), lateral ( Ny ) and shear loads (Nxy, Ny x ) as well as normal
pressure (P) may be applied to the model. Figure 7 shows the definition and sign
convention of these load components.
The axial loads on the panel ends (N x ) are applied in such a way as to produce
uniform strain, (ex). That is, the total applied load is effectively distributed to the base
panel and the stiffeners according to their relative stiffnesses. This is accomplished in
DIAL by forcing a set of edge "slave" nodes to displace as the weighted average of the
displacements of the two "master" nodes at the panel comers as shown in Figure 8. The
weights used are inversely proportional to the distances of the slave nodes to the master
nodes. This method of applying axial loads simulates the loading produced by the
surrounding wing or fuselage structure as well as in most stiffened panel test set-ups.
Boundary Conditions
Each edge (boundary) of the panel may be independently specified to be free,
simply-supported or clamped. The simple supports are simulated constraining only the
out-of-plane ( normal to panel ) degree of freedom at each node. Clamped conditions are
simulated by constraining both normal translations and rotations along the edge. In
addition to the constraints used to simulate the structural support provided by the adjacent
structure, kinematic constraints are specified to prevent rigid body motions as shown in
Figure 9. These kinematic constraints are generated automatically by the ISPAN modules
Under normal circumstances, the kinematic constraints will produce no internal loading in
the panel. If a pressure load were inadvertently specified without the balancing normal or
hoop loads on the panel edges, then the kinematic constraints would provide the balancing
loads. This undesirable condition would become obvious to the user once the deflected
shape and/or stress contours are examined.
937
Theoptionexistsin ISPANmodules to provide out-of-plane support at specified
locations on the stiffened panel in such a way as to simulate a fib or circumferential frame.
The support is modeled by constraining the out-of-plane displacement normal to the panel
at user specified locations. The inherent assumption in this modeling technique is that the
fib or frame has sufficient stiffness to enforce a node in the buckled mode shape of the
panel. The rotations about the y-axis at the fib locations may also be constrained in order
to simulate a very rigid support such as a main frame. In most applications (intermediate
frames or fibs), constraining these rotations will be unconservative.
Solutions
Three solution procedures, linear static, bifurcation ( initial buckling ) and post-
buckling, are presently available in ISPAN. The linear static solution is straightforward
and needs no explanation.
The initial buckling solution is an analysis to determine the multiplier on the applied
load (eigenvalue) at which any part of the structure first becomes unstable. No knockdown
factors nor initial imperfections are accounted for in this bifurcation analysis.
A post-buckling solution allows the user to determine the ultimate load capability of
a structure. Some flight vehicle structures are permitted to buckle locally at load levels
below ultimate, provided they retain the capability to carry the ultimate load without
complete collapse. This loading condition can be analyzed using the post-buckling
solution in DIAL, which enables an investigation of the integrity of the structure after initial
buckling, to establish the ultimate allowable load based on strain cutoff, strain interaction or
general instability/total collapse. The DIAL program uses the Arc-Length method,
described in reference 2, to perform the non-linear analysis. This method requires the user
to select a target point in the form of either load factor or a maximum displacement at a
certain location (grid point). Since strength, rather than displacement is the criterion most
often used for structural design, the load factor option is recommended for this type of
analysis.
The solution procedure for conducting the non-linear analysis performs an initial
buckling calculation first, and uses the resulting load and mode shape as the starting point
for the non-linear post-buckling analysis. ISPAN multiplies the first eigenvector by 2%
938
(.02) to establishtheshapeof theimperfectpanelatthezeroloadstate.Thisprocedurenot
only facilitatesthenon-linearsolutionprocedure,butprovidesamorerealisticanalysisof
actualstructures;afeaturein thisanalysisthatis normallyhandledbyknock-downfactors
in othersolutiontechniques.
ANALYSIS-TESTCOMPARISONOFPOST-BUCKLEDRESPONSE
TheISPAN modulewasusedto analyzeacompositeflat stiffenedpanelfor which
testandpreviousanalysiswork alreadyexists(ref 1). Thepurposeof thisanalysiswasto
verify theaccuracyof the post-buckledanalysissolutionin DIAL. Thepanelin thiscaseis
an 'T' stiffenedpanel81.3cmlong (parallelto stiffeners)and61.0cm widewith four
stiffenersspacedat 17.8cm. Thepanelwasloadedin purecompression.
Themodelgeometrygeneratedby ISPANis shownin Figure10. As in all ISPAN
modules,modifiedthick shellelementswereusedfor all components.The deflectedshape
of thepanelat a loadof 92.7kips is shownin Figure 11. This shape,which consistsof
five half-waves,is identicalto thatobservedin thetestpanelandin theSTAGSanalysisof
ref. 1.
The comparisons of the DIAL analysis with the results from ref. 1 in terms of load
vs. end shortening and load vs. strain curves are presented in Figures 12 and 13
respectively, and show reasonably good agreement. ISPAN presently does not include the
capability to generate tapered elements such as the attach flanges in the test panel. This
difference is thought to be responsible for the disagreement between test results and the
ISPAN-generated DIAL model results. Plans for future enhancements to the ISPAN
program may include incorporation of the interface element, which can be used to simulate
the bond between the stiffener and the skin panel. This interface element allows the
determination of the longitudinal and transverse shear and normal stresses (and strains) at
each load step in the non-linear solution; and thus can be used to predict stiffener interface
failure such as the one observed in the ref. 1 test.
939
PARAMETRIC STUDY
A trade study was conducted to illustrate one of the uses of ISPAN. A 24 in. by 24
in. blade-stiffened panel was analyzed with varying stiffener heights and spacings. The
loading for the study was uniform compression and the boundaries were simply supported.
Figure 14 shows an example of one of the blade stiffened panel model geometries
generated with ISPAN, in which the stiffener height was 2.0 in., and the spacing was 4.0
in. The combinations of height and spacing considered in this study are shown in Figure
15 along with the critical loads resulting from the linear and non-linear solutions. Both the
applied load at the strain cutoff value and the critical or collapse load are included in Figure
15 These results are presented in graphical form in Figure 16, in which it may be seen that
for a given load, there is an optimum combination of height and spacing. In this limited
study, the skin and stiffener thickness and laminate descriptions were not allowed to vary;
and obviously a comprehensive analysis to determine the optimum panel for a given
application would involve not only variations in thickness and properties, but panel length,
stiffener type and many other variables.
CONCLUSION
The ISPAN interface modules allow both experts and non-users of finite element
codes access to a powerful non-linear analysis procedure to enhance their efficiency and
analysis accuracy. The interface module procedure fills a void in the available methods of
analysis for anisotropic stiffened panel analysis. The expected benefit from this program is
the ability to consider a broad range of stiffened panel geometries and materials for multi-
axial loads application during the trade study phase of a new design also accounting for the
critical failure modes.
The analysis of an I-stiffened test panel shows that the accuracy of the ISPAN non-
linear analysis procedure compares favorably with test data and with other finite element
analyses.
Plans for future enhancements to ISPAN include incorporation of the existing DIAL
skin-stiffener interface element into the automatic mesh generation. The interface element
940
is used to represent the stiffness of the bond between the stiffener (s) and the skin. The
output stresses and strains for the interface element will allow bond failure modes to be
included in the analysis.
ACKNOWLEDGMENT
The authors wish to thank Messrs. Wayne Brown, Tony Wei and Dr. Norm Cyr,
of Lockheed Missiles and Space Company for their work in the development of the ISPAN
program(s). The authors also thank Dr. Randall Davis (NASA/LaRC) for his review and
comments.
REFERENCES
° Starnes, James H., Jr., Knight, Norman F., Jr., and Rouse, Marshall
"Postbuckling Behavior of Selected Flat Stiffened Graphite-Epoxy Panels
Loaded in Compression," AIAA Paper No. 81-0543, 1982.
° Anon., "DIAL Structural Analysis System User's Manual", Version L3D3,
August 1,1991, Lockheed Missiles and Space Company, Sunnyvale California.
941
DIAL IFINITE ELEMENTCODE
I FLAT CURVED TUBULAR GEODESICSTIFFENED STIFFENED FLAT SANDWICH CURVEDPANEL PANEL PANEL PANEL ISPAN
Figure 1 ISPAN - The Interface Between the Non-Finite Element Users and DIAL
ISPAN
GEOMETRYFIL__E
MATERIALFILE_
INTERACTIVE
FORTRAN PROGRAM
& VAX COM FILE
I DIAL )ATA BASE
PRE-PROCESSOR
DIAL
]ExistingDiALCode rl SOLVER
DIAL
POST-PROCESSOR
Figure 2 ISPAN Module Functional Flow
942
MODULES1 & 2:,_=,.-
(FLAT AND CURVED
STIFFENEDPANELS)
_L___T..__..E_ -L_J-
MODULE3:
(TRUSS CORE)
MODULE4: _ _ II _
(GEODESIC)
Figure 3 Sdffener Cross Sections Available in ISPAN
• SUPER-PARAMETRIC,
DOUBLYCURVEDTHICK
SHELLELEMENT
• MEMBRANE,BENDINGAND
SHEARRESPONSESARE
SEPARATED (TO SIMULATE
LAMINATE CONSTRUCTION)
Figure 4 Shell Element Type Used in ISPAN
943
Figure 5 Hat Stiffened Panel Model Generated by ISPAN
TOTAL THICKNESS MODELED
AS ONE SHELL ELEMENT
J
w
Figure 6 Attach Flanges of Stiffeners and Skin Elements are Modeled
as One Shell Element
944
\
Ny
7
\
\
Figure 7 Applied Loads Definition
.. • Master Nodes
. -" "" _- .,. 0 Slave Nodes
-" j_ 0
Figure 8 Master and Slave Nodes in CONODE Command
945
KINEMATIC CONSTRAINTS
SIMPLE SUPPORT CONSTRAINTS
z
.F
Figure 9 Typical Constraint Vectors for Flat Panel
Figure 10 DIAL Model Geometry of Test Panel From Reference 1.
946
JFigure
Figure 11 Deflected Shape of DIAL Test Panel Model at Final Load Step
Load (lbs)
120000
100000
00000
60000
40000
20000
/ •
.r:
/
//' 0 •
// 0
///0///
(
g • Starnes, et al.
0 DIAL Nonlinear Soln
0.00 0.05
I
0.10 ).15
End Shortening (in)
12 Comparison of Load-Displacement Results from DIAL and from Ref. 1 Test
and Analysis
947
100000
00000
60000
Load (lbs)
40000
20000
• Test. Data - Starnes, el. al.
0 DIAl, Nonlinear So]n ^
0 ' l ' f ' I r ' ', ' ! '
-2500 -2000 --1500 -1000 -5C3 0 500 1000 1500
Strain (10 -s in/in}
Figure 13 Comparison of Load-Strain Results from DIAL with Test Data (ref. 1)
Figure 14 Typical Blade Stiffened Panel Model Geometry from Parametric Study
948
Number of
Stiffeners
5
5
SPACING
b (in)
4.0
4.0
4.0
5 4.0
5 4.0
HEIGHT
h (in)
t bar (in) N x co (lb/in) N x cr (lb/in)
0.75 .0988 -3019.8 -2789.4
1.00 .1050 -3357.7 -3340.5
1.50 .1175 -4033.3 -5475.0
2.00 .1300 -4708.9 -3897.9
2.25 .1362 -5046.7 -3871.8
3 6.0 0.75 .0913 -2614.5
3 6.0 1.00 .0950 -2817.2
3 6.0 1.50 .1025 -3222.5
3 6.0 1.75 .1063 -3425.2
6.0 2.25 .1138 -3830.6
2 8.0
2 8.0
8.0 1.50 .0950 -2817.2
2.00 .1000 -3087.4
-1616.7
-2175.0
-3015.3
-3174.0
-2417.1
-1146.7
-2827.1
2.25 .1025 -3222.5 -2982.3
Figure 15 Stiffened Panel Paramewic Study Dimensions And Results
ts - X,, t:} 1,
k
.14 m
.13 -
_.12.c__- _7
_.11 --
i_-,
•I0-- ""---/b6''_'
.09 - --
h
.08 -
b
I I I I
t-= t sk + t Stb* h 1 2 3 4
NXc r (K/in)
Figure 16 Results of Parametric Analysis of Blade Stiffened Panel
949



ISPAN (Interactive Stiffened Panel Analysis): A tool for quick concept evaluation and design trade studies

Abstract

Similar works

Full text

Available Versions

NASA Technical Reports Server