Commit 8487436e authored by Jeremy BLEYER's avatar Jeremy BLEYER

Dynamic modal analysis example

parent 98142cc2
......@@ -13,6 +13,7 @@ Contents:
intro
2D_elasticity
demo/modal_analysis_dynamics/cantilever_modal.py.rst
demo/reissner_mindlin/reissner_mindlin.rst
......
......@@ -48,6 +48,13 @@ in Solid and Structural Mechanics at `Laboratoire Navier <http://navier.enpc.fr>
a joint research unit of `Ecole Nationale des Ponts et Chaussées <http://www.enpc.fr>`_,
`IFSTTAR <http://www.ifsttar.fr>`_ and `CNRS <http://www.cnrs.fr>`_ (UMR 8205).
.. image:: _static/logo_Navier.png
:scale: 8 %
:align: left
.. image:: _static/logo_tutelles.png
:scale: 20 %
:align: right
......
......@@ -72,7 +72,7 @@ def process():
if not ret == 0:
raise RuntimeError("Unable to convert rst file to a .py ({})".format(f))
png_files = [f for f in os.listdir(version_path) if os.path.splitext(f)[1] == ".png" ]
png_files = [f for f in os.listdir(version_path) if os.path.splitext(f)[1] in [".png",".gif"] ]
for f in png_files:
source = os.path.join(version_path, f)
print("Copying {} to {}".format(source, demo_dir))
......
.. _ModalAnalysis:
==========================================
Modal analysis of an elastic structure
==========================================
-------------
Introduction
-------------
This program performs a dynamic modal analysis of an elastic cantilever beam
represented by a 3D solid continuum. The eigenmodes are computed using the
**SLEPcEigensolver** and compared against an analytical solution of beam theory.
The corresponding file can be obtained from :download:`cantilever_modal.py`.
The first four eigenmodes of this demo will look as follows:
.. image:: vibration_modes.gif
:scale: 80 %
The first two fundamental modes are on top with bending along the weak axis (left) and along
the strong axis (right), the next two modes are at the bottom.
---------------
Implementation
---------------
After importing the relevant modules, the geometry of a beam of length :math:`L=20`
and rectangular section of size :math:`B\times H` with :math:`B=0.5, H=1` is first defined::
from fenics import *
import numpy as np
L, B, H = 20., 0.5, 1.
Nx = 200
Ny = int(B/L*Nx)+1
Nz = int(H/L*Nx)+1
mesh = BoxMesh(Point(0.,0.,0.),Point(L,B,H), Nx, Ny, Nz)
Material parameters and elastic constitutive relations are classical (here we
take :math:`\nu=0`) and we also introduce the material density :math:`\rho` for
later definition of the mass matrix::
E, nu = 1e5, 0.
rho = 1e-3
# Lame coefficient for constitutive relation
mu = E/2./(1+nu)
lmbda = E*nu/(1+nu)/(1-2*nu)
def eps(v):
return sym(grad(v))
def sigma(v):
dim = v.geometric_dimension()
return 2.0*mu*eps(v) + lmbda*tr(eps(v))*Identity(dim)
Standard FunctionSpace is defined and boundary conditions correspond to a
fully clamped support at :math:`x=0`::
V = VectorFunctionSpace(mesh, 'Lagrange', degree=1)
u_ = TrialFunction(V)
du = TestFunction(V)
def left(x, on_boundary):
return near(x[0],0.)
bc = DirichletBC(V, Constant((0.,0.,0.)), left)
The system stiffness matrix :math:`[K]` and mass matrix :math:`[M]` are
respectively obtained from assembling the corresponding variational forms::
k_form = inner(sigma(du),eps(u_))*dx
l_form = Constant(1.)*u_[0]*dx
K = PETScMatrix()
b = PETScVector()
assemble_system(k_form, l_form, bc, A_tensor=K, b_tensor=b)
m_form = rho*dot(du,u_)*dx
M = PETScMatrix()
assemble(m_form, tensor=M)
Matrices :math:`[K]` and :math:`[M]` are first defined as PETSc Matrix and
forms are assembled into it to ensure that they have the right type.
Note that boundary conditions have been applied to the stiffness matrix using
``assemble_system`` so as to preserve symmetry (a dummy ``l_form`` and right-hand side
vector have been introduced to call this function).
Modal dynamic analysis consists in solving the following generalized
eigenvalue problem :math:`[K]\{U\}=\lambda[M]\{U\}` where the eigenvalue
is related to the eigenfrequency :math:`\lambda=\omega^2`. This problem
can be solved using the ``SLEPcEigenSolver``. ::
eigensolver = SLEPcEigenSolver(K, M)
eigensolver.parameters['problem_type'] = 'gen_hermitian'
eigensolver.parameters["spectrum"] = "smallest real"
eigensolver.parameters['spectral_transform'] = 'shift-and-invert'
eigensolver.parameters['spectral_shift'] = 0.
The problem type is specified to be a generalized eigenvalue problem with
Hermitian matrices. By default, SLEPc computes the largest eigenvalues, here
we instead look for the smallest eigenvalues (they should all be real). To
improve convergence of the eigensolver for finding the smallest eigenvalues
(by default it computes the largest ones), a spectral transform is performed
using the keyword `shift-invert` i.e. the original problem is transformed into
an equivalent problem with eigenvalues given by :math:`\dfrac{1}{\lambda - \sigma}`
instead of :math:`\lambda` where :math:`\sigma` is the value of the spectral shift.
It is therefore much easier to compute eigenvalues close to :math:`\sigma` i.e.
close to :math:`\sigma = 0` in the present case. Eigenvalues are then
transformed back by SLEPc to their original value :math:`\lambda`.
We now ask SLEPc to extract the first 6 eigenvalues by calling its solve function
and extract the corresponding eigenpair (first two arguments of `get_eigenpair`
correspond to the real and complex part of the eigenvalue, the last two to the
real and complex part of the eigenvector)::
N_eig = 6 # number of eigenvalues
print "Computing %i first eigenvalues..." % N_eig
eigensolver.solve(N_eig)
# Exact solution computation
from scipy.optimize import root
from math import cos, cosh
falpha = lambda x: cos(x)*cosh(x)+1
alpha = lambda n: root(falpha, (2*n+1)*pi/2.)['x'][0]
# Set up file for exporting results
file_results = XDMFFile("modal_analysis.xdmf")
file_results.parameters["flush_output"] = True
file_results.parameters["functions_share_mesh"] = True
# Extraction
for i in range(N_eig):
# Extract eigenpair
r, c, rx, cx = eigensolver.get_eigenpair(i)
# 3D eigenfrequency
freq_3D = sqrt(r)/2/pi
# Beam eigenfrequency
if i % 2 == 0: # exact solution should correspond to weak axis bending
I_bend = H*B**3/12.
else: #exact solution should correspond to strong axis bending
I_bend = B*H**3/12.
freq_beam = alpha(i/2)**2*sqrt(E*I_bend/(rho*B*H*L**4))/2/pi
print("Solid FE: {0:8.5f} [Hz] Beam theory: {1:8.5f} [Hz]".format(freq_3D, freq_beam))
# Initialize function and assign eigenvector (renormalize by stiffness matrix)
eigenmode = Function(V,name="Eigenvector "+str(i))
eigenmode.vector()[:] = rx/omega
The beam analytical solution is obtained using the eigenfrequencies of a clamped
beam in bending given by :math:`\omega_n = \alpha_n^2\sqrt{\dfrac{EI}{\rho S L^4}}`
where :math:`S=BH` is the beam section, :math:`I` the bending inertia and
:math:`\alpha_n` is the solution of the following nonlinear equation:
.. math::
\cos(\alpha)\cosh(\alpha)+1 = 0
the solution of which can be well approximated by :math:`(2n+1)\pi/2` for :math:`n\geq 3`.
Since the beam possesses two bending axis, each solution to the previous equation is
associated to two frequencies with bending along the weak axis (:math:`I=I_{\text{weak}} = HB^3/12`)
and along the strong axis (:math:`I=I_{\text{strong}} = BH^3/12`). Since :math:`I_{\text{strong}} = 4I_{\text{weak}}`
for the considered numerical values, the strong axis bending frequency will be twice that corresponsing
to bending along the weak axis. The solution :math:`\alpha_n` are computed using the
``scipy.optimize.root`` function with initial guess given by :math:`(2n+1)\pi/2`.
With ``Nx=400``, we obtain the following comparison between the FE eigenfrequencies
and the beam theory eigenfrequencies :
===== ============= =================
Mode Eigenfrequencies
----- --------------------------------
# Solid FE [Hz] Beam theory [Hz]
===== ============= =================
1 2.04991 2.01925
2 4.04854 4.03850
3 12.81504 12.65443
4 25.12717 25.30886
5 35.74168 35.43277
6 66.94816 70.86554
===== ============= =================
Markdown is supported
0% or .
You are about to add 0 people to the discussion. Proceed with caution.
Finish editing this message first!
Please register or to comment