Docstoc

MECH Finite Element Methods

Document Sample
MECH Finite Element Methods Powered By Docstoc
					MECH3300 Finite element methods


   Lecture 10 Issues in modelling
       Solving the equations
                      Use of symmetry
• With increasing computer power, many analysts cannot be bothered
  with symmetry. However, there are always problems that are too big,
  that can be reduced in size at least 4 fold, by exploiting symmetry.

• Even if loading is unsymmetric, symmetry of geometry can be exploited
  by subdividing the loading into symmetric and antisymmetric
  components and superimposing two solutions, modelling 1/2 the
  structure, and changing restraints on the plane of symmetry..
  F                      F/2           F/2       F/2
                                                                     F/2


                           Symmetric case       Antisymmetric case
 Plane of symmetry
       Restraints for modelling symmetry
• With symmetric deformation, nodes in a plane of symmetry
  remain there.




• To make this happen, fix displacement normal to the plane and
  rotations about axes in-plane (if defined).

• Conversely, permit in-plane displacements and rotation about
  the normal to the plane of symmetry.

• Anti-symmetry is the opposite - no motion in the plane of
  symmetry.
                Meshing solid models
• For machine components, it is possible to automatically mesh a
  CAD solid model. Standard formats are needed to import
  geometry into FE packages (eg IGES - International Graphic
  Exchange Standard).

• Geometry needs to be checked, for duplicate edges, very short
  edges that would produce too fine a mesh locally, and for details
  that should be omitted, as it is not practical to mesh them.
  Geometry must be checked for free edges, or faces, to ensure it
  is connected properly.

• A surface mesh is often created first with plates, and this used to
  guide generation of a solid mesh.

• A mesh created by automatic or other meshing must be checked
  for duplicated nodes or elements, and to ensure all elements are
  connected correctly.
    Example of auto-meshing inappropriate
     geometry (Strand7 tutorial problem)
•                         Nodes cluster to attempt
                          to match 2 very short
                          side-lengths present in
                          the geometry - these
                          “slivers” need removing.
                          Some simplification of the
                          real geometry is often
                          needed to get an
                          appropriate mesh.
     Loading and restraining solid models
A solid model subject to a point load will have very high stress at the
load. This makes it impossible to see the stress elsewhere on a
contour plot, and is unrealistic.
Hence loads must be distributed realistically. This can take some
thought - eg loading due to a pin in a hole.
Distribution?
Quadratic by Hertz theory.




Restraints also need realistic distribution. For the pin in a hole case,
polar coordinates at the centre of the hole are needed so as to fix
radial displacements around the hole, but not tangential ones. Over
what angle of arc?
             Meshing arbitrary shapes
• This is something commercial packages still not not do well.

• A surface described by a stereolithography *.stl file can often be
  imported, but this can be a very fine triangulation. It may be
  possible to “unrefine” this to get a more suitable mesh (the
  command exists in NASTRAN for Windows for instance), but
  this may still take much to long to do to be practical.
                        Equation solvers
• The large set of equations in a linear elastic finite element model is
  solved either by Gauss elimination or by an iterative algorithm (eg the
  pre-conditioned conjugate gradient method).

• The iterative solvers tend to become more efficient on very large
  problems. (eg 100000 nodes). They use sparse matrix storage, that is
  they store only non-zero terms along with their row and column
  addresses.

• There are different ways of organizing how Gauss elimination is done.
• It is always 2 stages - triangular decomposition [K] = [L][U], followed
  by back-substitution F = [L]z, z = [U]u.

• (a) the equations can be written in an order that minimizes the
  bandwidth of [K], so that only terms within the bandwidth are stored on
  disk or processed by the solver.
• (b) the “wavefront” solver, implemented in ANSYS can be used.
                The wavefront solver
• In this approach to solving the equations, the elements are
  numbered so that elements connected together have similar
  numbers. Only those elements connected to a node having its
  equations processed must be assembled at any one time.

• The effect of solving equations one node at a time is that the
  mesh is divided into 3 regions - nodes yet to be processed,
  nodes being processed, and nodes having been processed.

• The boundaries between these regions sweep across the mesh,
  hence the “wavefront” name.

• This approach may be more efficient than a bandwidth -
  minimizing solver.
                      Explicit Solvers
One approach to highly nonlinear problems is to integrate in
time using Newton’s law ie
FEXT + FINT = Ma
FEXT = external forces (applied loads) at some time.
FINT = internal forces (due to elastic or plastic deformation etc.)
M = mass matrix
a = accelerations - solve for these. If M is diagonal, then
these are found “explicitly” from the forces.
The new accelerations give new velocities and displacements
(central difference method). These are used to find new
internal forces, and to again to find new accelerations, and so
on. Timestep size must be very small (eg microseconds).
           Substructures or superelements
• Traditionally, very large models of ships, cars bodies etc. were solved by
  a divide and conquer approach of separating the mesh into different
  regions called either substructures or superelements.

• The equations for each region are “statically condensed” to give many
  fewer equations just relating forces/displacements on the interfaces
  between regions.

• These are solved, and the interface displacements provide boundary
  conditions to solve the equations for each substructure separately.

• A typical substructure would be the wing of an aircraft - the rear fuselage
  may be another, and the tail a third etc.

• These methods are still used where a model of part of a system is
  prepared by a sub-contractor - eg a payload for the space shuttle.
                      Eigenvalue problems
• Finding critical loads for buckling, or finding natural frequencies for
  vibration leads to matrix eigenvalue problems.

• For undamped natural frequencies [K]u = l[M]u must be solved, where
  [M] is a mass matrix and the eigenvalue l is the angular natural
  frequency squared w2 - more next semester in dynamics.

• For buckling [K]u = l[Kg]u where [Kg] is a geometric stiffness matrix
  describing the change in stiffness due to finite deformation, worked out
  for the loading used previously in a linear static analysis.

• The eigenvalue l this time is a factor on the loading that will scale it up
  to that causing buckling.

• This approach is as accurate as hand calculation of a critical load, but
  not a true finite deformation analysis that keeps updating coordinates
  of nodes - it is just a perturbation of a linear analysis.
          Solving eigenvalue problems
• We usually only want to know the lowest natural frequencies of a
  vibrating structure, as they are most easily excited.
• Similarly, only the lowest buckling eigenvalue is meaningful, as it
  takes less work to make the structure collapse at this load, than at
  the others predicted, which could only occur if buckling were
  prevented at the lowest critical load.

• Hence the most appropriate solvers are algorithms that iteratively
  refine estimates of u to find the lowest modes of deformation.
  These can however, potentially miss a solution in an ill-conditioned
  problem. An algorithm which counts how many eigenvalues exist in
  a particular range of values can be used to check if solutions are
  missing (a Sturm sequence check).

• The user can typically select how many modes of deformation to
  estimate. The results are usually animated to see the motion more
  clearly.
            Solving non-linear problems
• Non-linear problems take much more computation to solve than
  static problems, as the solvers work by successive linearization,
  that is, the solution keeps going off on a tangent and is then
  corrected.

• A static finite deformation analysis, for instance, is typically done
  by incrementing the loading a number of times. Within each
  load increment, “equilibrium iterations” are performed to correct
  the error between the external loads and the predictions of
  internal loads, found from the latest linearized solution.

• The number of iterations, to predict a substantial change of
  shape can be many hundreds, and the equivalent of a linear
  static analysis is done every iteration.

• A solution for the post-buckled state of a structure can be quite
  hard to obtain.
        History of load-deflection in some element
    • The progress of a non-linear solution can be pictured by the
      history of loading in a particular element versus its deflection.

                 Equilibrium
Load             iterations
                                                          True load-deflection
(eg tension in
                                                          graph
a particular
bar)
                                   First load increment




                       Deflection magnitude

				
DOCUMENT INFO
Shared By:
Categories:
Tags:
Stats:
views:5
posted:11/24/2011
language:English
pages:15