Appropriate Boundary Condition for Finite Element Analysis of Structural Members Isolated from Global Model.pdf

APPROPRIATE BOUNDARY CONDITION FOR FINITE ELEMENT ANALYSIS
OF STRUCTURAL MEMBERS ISOLATED FROM GLOBAL MODEL
Aun Haider Bhutta1
1 Senior Engineer, Pakistan Air Force, Pakistan, Ph +92(0)321 6906109, Email: aunbhutta@gmail.com.
ABSTRACT
61
NED UNIVERSITY JOURNAL OF RESEARCH - STRUCTURAL MECHANICS, VOL XVIII, NO. 3, 2021
https://doi.org/10.35453/NEDJR-STMECH-2021-0001
Manuscript received on 1st March 2021, reviewed and accepted on 28th May 2021 as per publication policies
of NED University Journal of Research. All rights are reserved in favour of NED University of Engineering
and Technology, Karachi, Pakistan. Pertinent discussion including authors’ closure will be published in July
2022 issue of the Journal if the discussion is received by 31st January 2022.
The wing of a fighter aircraft has various structural members which support aerodynamic and
inertial loads, and transmit these loads to the fuselage. As a foremost step to evaluate the structural
behaviour of the wing assembly, component contribution analysis is carried out. A finite element
analysis of wing tulip of fighter aircraft isolated from the wing was performed under the design
load case. Since aircraft wing is a statically indeterminate structure, reaction forces and moments
at the supports depend upon the stiffness characteristics of the wing itself. In addition, stiffness of
wing also affects the distribution of load and resulting deformation of the wing. These require that
support structure of tulip isolated from the global wing model is represented by appropriate boundary
conditions for the analysis. A comparative study for three boundary conditions (fixed support, nodal
displacements and elastic support) was carried out to determine the representative boundary
condition for the analysis of structural members isolated from the global model. It was found that
elastic support represents the stiffness of the global model and is a more appropriate boundary
condition for the analysis of local models which are isolated from a global model.
Keywords: boundary conditions; fixed support; nodal displacement; elastic support; global model;
local model; submodelling.
1. INTRODUCTION
The wing of an aircraft generates lift which is required to balance the weight of aircraft during flight
[1]. Modern fighter aircrafts have multi-spar wet wing design where fuel is carried inside the wing
structure. Wing also has lift-producing surfaces (such as flaps and slats) and control surfaces (such
as ailerons). These surfaces affect the air flow and resultant pressure distribution over the wing.

62
A. H. Bhutta
The internal structure of the wing of a fighter aircraft is illustrated in Figure 1. Wing skin provides
an external cover to the internal structural members. It also transmits fluid forces to the stingers and
ribs by plate and membrane action. Wing spars (Figure 1) run along the span and carry the flight
loads (including bending moment, torsional moment and shearing forces) and weight of the wing
on ground. Stingers are thin longitudinal members along the span direction which (together with
the skin) resist axial and bending load along with the skin (Figure 1). The transverse members which
run along chord wise direction are called ribs (Figure 1). Ribs maintain the shape of the wing cross-
section [2]. The wing may also have external hard points or stations where external stores (such as
fuel tanks) can be carried. The external payload is attached to the wing tulips (Figure 1). The wing
tulip considered in this paper is located at a rib which (in turn) is attached to front wall of wing.
Structural analysis of wing tulip isolated from the wing under applied loads is carried out in this
paper to determine the maximum stress on the tulip. Effects of various boundary conditions on the
maximum stress have been examined. A scheme of analysis has been identified to include the
stiffness of the attached structure through application of appropriate boundary condition. This paper
identifies the most appropriate boundary condition for the analysis of structural member isolated
from the global model.
Aun Haider Bhutta is a Senior Engineer at Pakistan Air Force, Pakistan. He received his
Bachelors and Masters in Aerospace Engineering from National University of Science and
Technology, Pakistan and Air University, Pakistan, respectively. He has more than 12 years
of experience in ‘O’, ‘I’and ‘D’level maintenance of aircraft and engines. His research interests
include structural health monitoring, numerical analysis, finite element methods, aero elasticity,
fluid structure interaction and design optimisation.
Figure 1. Internal structure of aircraft wing.

NED UNIVERSITY JOURNAL OF RESEARCH - STRUCTURAL MECHANICS, VOL XVIII, NO. 3, 2021 63
2. BACKGROUND OF FINITE ELEMENT ANALYSIS
One of the major concerns for a finite element (FE) analyst is the time required to perform the
simulation [3]. The solution time depends upon the size of FE model vis-à-vis computational
resources available. There is always an inclination of FE analyst for the anticipated results within
hours, not in days or weeks. This disposition is driven by the time constraints to design a product
and put it in service. Various techniques have been developed to minimise the solution time without
the expanse of accuracy [4].
Idealisation of the problem domain [5] from three-dimensional (3D) model to two-dimensional (2D)
model including plane stress idealisation (such as analysis of spur gears), plane strain idealisation
(such as long pipes under constant pressure) and axis symmetry modelling (such as engine valve
stem, piston of hydraulic cylinder) can reduce the solution time enormously. Furthermore, 3D
problem domain can also be reduced significantly by using reflective symmetry (such as solid
models of pressurized tanks) and cyclic symmetry (such as blades of compressor/turbine stage).
The solution time can also be reduced by properly using lower order FEs for structural members
[6]. For example, zero order mass elements can be used to idealise the inertial effects of a body.
Mass element can represent the force with acceleration or the inertial mass attached to a structure
without affecting modal solutions. Similarly, zero order spring and damper elements can represent
the stiffness and damping effects of the support structure without adding the inertial effects.
Long slender structural members (such as those in power transmission tower) can be modelled with
first order (1D) line elements [7]. A line element can represent beams, spars, pipes, etc. Thin-walled
structural members can be modelled with second order (2D) plate and shell elements. These 2D
area elements have triangular or quadrilateral shape with or without the presence of mid-side node.
Additionally, 2D elements can be used accurately with planar symmetry, cyclic symmetry and anti-symmetry.
However, the bulky low aspect ratio potato shaped structural members cannot be modelled by the
preceding approximations which (inevitably) require 3D solid elements [8]. 3D volume element
may have wedge, tetrahedral or brick shape. Similar to the case for 1D and 2D elements, mid-side
nodes in 3D elements define the order of shape function for interpolating the displacement values
between the nodes.
Analysing the structural response of an assembly is a natural extension of the part modelling
techniques described earlier [9]. In reality, few parts exist and operate in isolation. In many cases,
the entire assembly or subassemblies must be modelled to fully understand the system. This is
readily apparent when multiple parts are joined together such that they behave as a single, continuous
load-bearing structure. Assembly modelling is also required in some cases, as the mating components
deform in a way that the final position, deformation and stress state of the part under investigation
are functions of displacement [10].
Modelling assembly is not only computationally intensive, it also challenging and arduous [11].
Furthermore, the interaction between the mating parts in an assembly introduces an uncertainty in
the structural behaviour of the assembly. Consequently, each part or rigidly connected subassembly
(local model) is isolated from the complete assembly (global model) for analysis [12]. This method
is called component contribution analysis. The following two techniques have been devised to
represent the supporting structure in the analysis of the local model.

64
A. H. Bhutta
2.1 In-Situ Modelling
In in-situ modelling approach [13], high-fidelity local model of a part is directly positioned within
the overall global model of the assembly. Using multipoint constraints (MPCs) (also called links
or rigid elements), connectivity between the local and global model is established. The advantage
of this technique is that boundary conditions are not interpolated between the local and global model.
However, connection elements are introduced between the local and global model with characteristics
assigned by the analyst based upon the perceived behaviour within the assembly.
Figure 2 shows a global model of an oil rig with beam elements. The joint is studied for local stress
concentrations. All the load transfer within the beam element model takes place at the connecting
nodes. In reality, the load transfer actually takes place through the welded intersections of the
cylinders, with resulting local stress concentrations. Beam elements cannot simulate the load path
and the resultant stress concentration at the nodal connections between two members [14].
To model the joint in detail, improved representation with a local shell model is made which is shown
in Figure 3. Rigid elements are used to connect the shell mesh and the beam mesh. The shell elements
represent the correct load transfer path in the walls between the intersecting cylinders. Therefore,
stress concentration between the connecting members can be predicted correctly. Note that the
computing resource for the improvised model is still much less compared to a full-scale solid model.
Figure 2. Global model of oil rig.
Figure 3. Rigid elements for connection of local model to global model.

The accuracy of the in-situ modelling depends on how well the connecting elements (multipoint
constraints, rigid elements, etc) represent stiffness of the structure in the transition region, which
eventually affects the load transfer path. Nevertheless, since the stresses in the transition zone are
always uncertain, the transition zone is inevitably framed away from the stress concentration region.
2.2 Submodelling
In automotive and aerospace industry, submodelling is (more often) used to carry out FE analysis
of individual parts within the assembly [15]. This technique involves solution of coarsely meshed
global model followed by a subsequent solution of using only a portion of the coarse model (local
model) with a more refined mesh. Figure 4 shows the local refined model extracted from the global
course model.
Extracting a local model from the global model necessitates the application of creative boundary
conditions on the cut boundaries. There are three different boundary conditions that can be applied
at the cut boundaries of the submodel [16].
1) Fixed constraints are used when the attached structure is rigid enough that it does not deform
under the applied loads.
2) Nodal displacements can be enforced at the cut plane when full FE model can be solved under
the applied load and displacement which are available from the solution of global FE model.
This condition assumes that the deformation in the sub model will not affect the displacement input.
3) A submodel can be isolated from the global model by using linear and rotational springs, if
elastic response of a structure under the known load is available.
Nodal displacement and elastic support are the two boundary conditions which introduce the stiffness
of the global model within the solution of isolated structural members. However, both boundary
conditions require an additional FE analysis of the global model under the applied load.
3 FINITE ELEMENT ANALYSIS OF WING TULIP
3.1 Computer Aided Design Model
Computer aided design (CAD) model of the wing tulip was developed in Ansys DesignModeler®.
The following material properties of 30CrMnSiA alloy steel were used for the tulip: modulus of
elasticity = 196 GPa (1934×103
ksi); yield strength (sy) = 835 MPa (839 ksi); and Poison ratio (m)
= 0.3. Solid model of the wing tulip is shown in Figure 5.
Figure 4. Isolation of sub model from global model.

66
A. H. Bhutta
Figure 5. Solid model of wing tulip.
Table 1. Design loads for wing tulip
Force Component
Axial force (Fx)
Lateral force (Fy)
Vertical force (Fz)
Magnitude, N (lb)
28200 (6340)
4040 (908)
37400 (8408)
Moment component
Torsion (Mx)
Bending moment (My)
Yaw moment (Mz)
Magnitude, N.m (lb.ft)
680 (499.6)
35 (25.71)
0
Figure 6. Free mesh of wing tulip.
3.2 Design Load Case
Inflight load simulation within the carriage-envelop of the aircraft provides the design load case
for the wing tulip. The design load case for the wing tulip occurs at +4.5g symmetric pullup
manoeuvre at 0.8 Mach number. Lift force at the design load is 4.5 times the instantaneous weight
of the aircraft. The design load for the wing tulip is applied in the form of force and moment vector.
Table 1 provides the design loads for the wing tulip.
3.3 Finite Element Model of Wing Tulip
Tetrahedral elements (Solid72) with mid-side nodes were used for meshing the model. Mid-side
nodes are preserved to enforce quadratic shape function. Figure 6 shows the meshed model of the
wing tulip. In order to capture stress gradients at discontinuities, areas with geometric transition and
stress concentration were finely meshed.

Mesh independence study was performed to generate numerical model which is independent of
mesh density. Figure 7 illustrates variations in stress with increase in number of elements. It is seen
in Figure 7 that the solution becomes independent of mesh size at seventy thousand elements.
The wing tulip is attached to front rib and front wall of the wing with six M6 metric bolts. Since
suitable boundary conditions are needed when a wing tulip is isolated from wing, the following
three boundary conditions were used for comparative analysis: (a) fixed support, constrained in six
degrees of freedom (DoF); (b) nodal displacements of the tulip obtained from the solution of the
wing under the design load; nodal displacements are enforced as fixed displacement in Ansys; and
(c) elastic support which represents stiffness of the global wing model.
3.4 Structural Analysis with Fixed Support
The assumption of fixed support (constrained in six DoF) as boundary condition for the tulip is
likely to result in higher stresses at the bolt holes compared to the actual scenario. As a result, the
strength of the tulip will be underestimated. This technique, however, is conservative in nature and
many researchers [9] have used this boundary condition to determine the structural integrity of the
individual components isolated from the global model.
Figure 8 presents the applied loads and fixed support boundary condition on the tulip. Figure 9
illustrates the deformation field of the tulip under the design loads. It can be observed from the
comparison of Figures 8 and 9 that boundary condition is closely simulated in the analysis. No
displacement was observed at the attachment bolt holes in this case. Maximum deformation of 0.37
mm (0.015 in.) was observed on the flange of the tulip. The equivalent von-Mises stress is shown
in Figure 10. In addition, maximum stress 1253 MPa (182 ksi) was observed on the bolt hole. Based
upon the yield criteria of material, factory of safety (FoS) is equal to 0.67, as illustrated in
Figure 11. The aircraft has experimentally demonstrated to fly at design load case without failure.
Consequently, it can be concluded that the fixed support boundary condition under predicts the
strength of the tulip and is the most conservative in nature. Application of fixed support boundary
condition erroneously recommends reduction in inertial and aerodynamic loads on the tulip due to
low FoS. Primarily, loads can be reduced either by reducing the weight of the payload or limiting
‘g’ loads within the flight envelope. However, reduction in the payload weight and limitation on
the flight envelope both affect the operational role of the fighter aircraft.
Figure 7. Mesh independence study for wing tulip.
Note: 1 MPa = 145 psi

68
A. H. Bhutta
Figure 8. Loads and fixed boundary condition on tulip.
Figure 9. Deformation of tulip with fixed support.
Note: 1 in. = 25.4 mm
Figure 10. Equivalent stress on tulip with fixed support.
Figure 11. Factor of safety for tulip with fixed support.

3.5 Finite Element Model of Wing
Modern fighter aircraft are built on wet wing design where fuel is carried inside the wing structure.
The wing also has external hard points or stations where external carriage such as fuel tanks or
weapons (bombs, missiles, electronic pods, etc) can be carried. Various structural members of the
wing support the aerodynamic and inertial loads acting on the wing within the flight envelop. Based
upon the structural functions of inner wing members, the following assumptions have been made
for the development of FE model of the wing [1].
1) Wing skin transfers the fluid forces to both the stringers and ribs by plate and membrane actions,
respectively. It supports the applied bending and axial loads together with the stringers. When
the structure is pressurised, skin together with the ribs also supports the hoop or circumferential
load. It is assumed that uniform shear stresses are developed in the skin to support the applied
torsional moments and shear forces. Skin was modelled with 1D Shell181 element in Ansys.
2) Spars of the wing run along the span wise direction of the wing (Figure 12). The spar has two
sections namely spar web and spar cap. Shear stress is developed in both the spar web and spar
cap under the applied torsional moments and shearing forces. Spar cap transmits fluid forces
to stringers and ribs by plate and membrane action. Spars are modelled with standard Beam188
element in Ansys.
3) Stringers are the thin longitudinal members along the span direction (Figure 12). Stringers resist
axial and bending loads along with the skin of wing. Stringers divide the skin into small panels
which increase its buckling and compressive failure limit. It is assumed that the stringers only
carry uniformly distributed axial stresses over their cross sections. Beam188 elements in Ansys
were used to model the stringers for internal load analysis, with minimal error being introduced
by the displacement incompatibilities between the beam elements and shell elements (for the skin).
4) Ribs are the transverse members which run along the chord wise direction (Figure 12). Ribs
distribute concentrated loads such as drop tanks and jettisonable ammunition into the structure
and redistribute stresses around structural discontinuities. Ribs establish the column length for
the stringers and skin panels and act as end restraint to increase buckling stress. Transverse ribs
remain rigid within their own planes to maintain the cross-sectional shape of wing. However,
Figure 12. Finite element model of inner structure of wing.

70
A. H. Bhutta
ribs do not resist any warping deformations out of their planes. Ribs are modelled with Shell181
elements in Ansys.
5) Secondary aircraft structure such as leading and trailing edge flaps, ailerons, and fuel/hydraulic
lines were not modelled.
6) Weight of fuel is represented by 0D Mass21 element in Ansys. Full fuel weight inside the wing
was applied at the centre of gravity location of wet wing. 1D line element Link180 in Ansys was
used for the connection of mass elements with the wing structure.
Figure 12 presents the detailed finite element model of inner structural members of the wing.
Figure 13 presents the subject FE model of the wing with intact skin elements.
3.6 Structural Analysis with Nodal Displacement
Nodal displacement obtained from the solution of the wing model can be used as displacement
boundary condition on the tulip instead of fixed support. Finite element analysis of the wing model
was carried out under design load to generated deformation field of the wing. Figure 14 illustrates
the deformation field of the wing under the design load.
Figure 13. Finite element model of wing with skin.
Figure 14. Deformation field of wing under design load.

Nodal displacements at the bolt holes of the tulip were used as boundary condition. These nodal
displacements were applied as fixed displacement in Ansys. Loads and boundary conditions for the
tulip are shown in Figure 15. Maximum deformation of the tulip under the design load (Figure 16)
is 0.32 mm (0.013 in.) on its flange. Equivalent stress on the tulip under the design load is presented
in Figure 17. Maximum stress of 782 MPa (113 ksi) occurs at bolt holes of the tulip. FoS for the
tulip is 1.07 as illustrated in Figure 18.
Figure 15. Load and displacement boundary condition on tulip.
Figure 16. Deformation of tulip with nodal displacements.
Figure 17. Equivalent stress on tulip with nodal displacements.
Note: 1 in. = 25.4 mm

72
A. H. Bhutta
Figure 18. Factor of safety for tulip with nodal displacements.
3.7 Structural Analysis with Elastic Support
The local sub model can be isolated from the global model by using linear and rotational springs if
elastic response of the global model under the known load is available. The deformation field of the
wing model under the applied load was generated. Based upon translational and rotational displacements
at the attachment bolts under the applied force and the moment, respectively, the stiffness of the
global wing model was calculated and was applied at the bolt holes. Linear and rotational stiffness
of the wing at the attachment bolts was calculated by using Eqs. (1) and (2), respectively
where K linear stiffness of the elastic support; F is the applied force on the tulip attachments; u is
the displacement at the attachment of the tulips; K is the torsional stiffness; T is the torque or moment
applied on the body; w is the twist angle; L is the length of the beam section; and q is the rotation
of the free end of the beam
Linear and rotational stiffness of the wing were applied as elastic support, which were 242 kN/m
(1658.2 lbf/ft) while rotational stiffness is 11.1 kN.m/rad (8186.5 ft.lbf/rad), respectively.
Applied loads and elastic boundary condition are shown in Figure 19. Elastic support with the wing
stiffness characteristics was used as boundary condition for the analysis. The deformation field of
the tulip under the applied loads is shown in Figure 20. Maximum deformation 0.13 mm (0.005
in.) was observed on the flange of the tulip. Maximum stress value of 674 MPa (98 ksi) was observed
on the bolt holes of the tulip as shown in Figure 21. FoS of the tulip under the design load was 1.23
which is shown in Figure 22.
4. DISCUSSION ON RESULTS
Three different boundary conditions have been enforced for structural analysis of wing tulip which
is isolated from the global wing model under the design load. These conditions include fixed support,
nodal displacement and elastic support. In all the cases, maximum deformation was observed on
the flange of the tulip while maximum equivalent stress was observed at the bolt holes. For fixed
k = F/u (1)
K = IP (1/L) = (T/q)(1/L) = T/w (2)

Figure 20. Deformation of tulip with elastic support.
Figure 19. Loads and elastic support on tulip.
Figure 22. Factor of safety of tulip with elastic support.
Figure 21. Equivalent stress on tulip with elastic support.
Note: 1 in. = 25.4 mm

74
A. H. Bhutta
support, maximum deformation is 0.37 mm (0.015 in.) while maximum equivalent stress is 1253 MPa
(182 ksi) which yields FoS of 0.67. Negative safety margin suggests that the tulip will fail under
the design load. Contrary, the aircraft has demonstrated successful flight under the design load.
Therefore, it can be concluded that the fixed support is a conservative boundary condition which
underestimates the maximum load carrying capacity of the wing tulip.
Nodal displacements obtained from the static structural analysis of the wing under the design load
are enforced as fixed displacement boundary condition at the bolt holes of the tulip. With this
boundary condition, maximum deformation is 0.32 mm (0.013 in.) while the maximum equivalent
stress is 782 MPa (113 ksi). FoS comes out to be 1.07 which suggests that the tulip does not fail
under the design load.
To include the stiffness effects of the wing in the analysis of the isolated tulip, the elastic support
was used as boundary condition. Elastic support affects the stiffness matrix by introducing translational
and rotational stiffness of the wing. With this boundary condition, maximum deformation is 0.13
mm (0.005 in.) while maximum equivalent stress is 674 MPa (98 ksi). Using yield criteria, FoS
comes out to be 1.23. Positive value of FoS suggests further load carrying capacity of the wing
station for the given flight load case or more severe ‘g’ loads can be endured with the given payload.
5. CONCLUSIONS AND RECOMMENDATIONS
1. Application of fixed support used as boundary condition for finite element analysis of isolated
structural member assumes infinite stiffness of the associated global model.
2. Nodal displacement and elastic support are the two boundary conditions which introduce finite
stiffness of the global model within the solution of isolated structural members. Additionally,
both these boundary conditions require finite element analysis of global model under the applied load.
3. Nodal displacement can be enforced at the cut plane of the isolated member when the displacement
(both the translation and rotation) of the global model under the given load at the cut plane is
known. However, the application of nodal displacement as the boundary condition is based upon
the assumption that deformation of the isolated structural member under the applied load does
not significantly affect the displacement input.
4. Elastic support is most appropriate boundary condition for the analysis of local model isolated
from the global model. Therefore, elastic support is the recommended boundary condition for
the analysis of structural members isolated from the global model. The stiffness of the global
model is introduced within the finite element model of isolated members through application
of linear and rotational springs. The stiffness of these springs is calculated from the translation
and rotation of the global model at the cut plane under the applied force and the moment,
respectively.
5. Fixed support is the most conservative boundary condition which provides lower factor of safety
for structural analysis of isolated members without any information of the global model. Compared
to fixed support, factor of safety of the isolated structural member is improved when nodal
displacement and elastic support are applied as boundary conditions.

REFERENCES
[1] Peery DJ. Aircraft structures. Courier Corporation, New York, USA, 2011. p. 138-141.
[2] Wright JR, Cooper JE. Introduction to aircraft aeroelasticity and loads. John Wiley & Sons,
England, 2008. p. 211-214.
[3] Dill EH. The finite element method for mechanics of solids with ANSYS applications. CRC
press, New York, USA, 2011. p. 61-67.
[4] Jang JH, Ahn SH. FE Modeling Methodology for Load Analysis and Preliminary Sizing of
Aircraft Wing Structure. Int J Avia Aeronaut Aerospa 2019;6(2):1-8.
[5] Larson MG, Bengzon F. The finite element method: theory, implementation, and applications.
Springer Science & Business Media, London, 2013. p. 174-177.
[6] Lee H-H. Finite element simulations with ANSYS Workbench 18. SDC publications, Kansas,
USA, 2018. p. 147-148.
[7] Madenci E, Guven I. The finite element method and applications in engineering using ANSYS
Springer, London, 2015. p. 61-62.
[8] Zienkiewicz OC, Taylor RL. The finite element method for solid and structural mechanics.
Elsevier, Burlington, Vermont, USA, 2005. p. 218-220.
[9] Muscolino G, Sofi A, Giunta F. Dynamics of Structures with Uncertain-but-bounded Parameters
via Pseudo-static Sensitivity Analysis. Mech Sys Sig Process 2018;111:1-22.
[10] Peruru SP, Abbisetti SB. Design and Finite Element Analysis of Aircraft Wing Using Ribs and
Spars. Int Res J Eng Tech 2017:4(6):2133-2139.
[11] Ranjbaran A. Bench Mark Equations for Determination of the Main Parameters of Fracture
Mechanics. NED Uni J Res 2014:XI(3):29-38.
[12] RanjbaranA, Ranjbaran M. State Based Damage Mechanics. NED Uni J Res 2017; XIV(1):13-26.
[13] Rao SS. The finite element method in engineering. Butterworth-heinemann, Oxford, England,
2017. p. 271-272.
[14] Ranjbaran A, Rousta H. Finite Element Analysis of Cracked Beams Innovative Weak form
Equations. NED Uni J Res 2013;X(1):39-47.
[15] Moaveni S. Finite element analysis theory and application withANSYS, 3/e. Pearson Education,
India, 2011. p. 471-475.
[16] Hughes TJ. The finite element method: linear static and dynamic finite element analysis.
Courier Corporation, New York, USA, 2012. p. 94-95.

76
BLANK PAGE

Appropriate Boundary Condition for Finite Element Analysis of Structural Members Isolated from Global Model.pdf

More Related Content

Similar to Appropriate Boundary Condition for Finite Element Analysis of Structural Members Isolated from Global Model.pdf (20)

More from Aun Haider (14)

Recently uploaded (20)

Appropriate Boundary Condition for Finite Element Analysis of Structural Members Isolated from Global Model.pdf