Natural Frequency Calculation Example
The analysis is performed with JuliaFEM v0.3.3
The example model is a bracket that is attached to two adapter plates via tie contacts. The adapter plates are constrained from one of their side as fixed.
The Bracket is modeled as cast iron while the Adapter plates are modeled as steel.
The material parameters are listed in the following table.
|Part||Material||E [MPa]||μ||ρ [kg/m3]|
|LDU Bracket||Cast Iron||165000||0.275||7100|
First all the packages needed in the calculation are included by typing
using package_name .
using JuliaFEM using JuliaFEM.Preprocess using JuliaFEM.Postprocess using JuliaFEM.Abaqus: create_surface_elements
The mesh needs to be read from ABAQUS input file to JuliaFEM. The function
abaqus_read_mesh(ABAQUS_input_file_name::String) will do the trick.
# read mesh mesh = abaqus_read_mesh("LDU_ld_r2.inp")
Problem(problem_type, problem_name::String, problem_dimension) function will
construct a new field problem where
problem_type is the type of the problem
(Elasticity, Dirichlet, Mortar etc.),
problem_name::String is the name of the
problem_dimension is the number of DOF:s in one node (1 in a heat
problem, 2 in a 2D problem, 3 in an elastic 3D problem, 6 in a 3D beam problem,
create_elements(mesh, Element_set_name::String) function will collect the
element sets from the ABAQUS input file. In this example the element sets are
update!(element_set_name, parameter::String, value) will update the material
parameters for the model. In this example there are two different materials for
the two different element sets.
The element sets are then added into the element list of the Problem:
# create a field problem with two different materials bracket = Problem(Elasticity, "LDU_Bracket", 3) bracket_elements = create_elements(mesh, "LDUBracket") adapterplate_elements = create_elements(mesh, "Adapterplate1", "Adapterplate2") update!(bracket_elements, "youngs modulus", 208.0E3) update!(bracket_elements, "poissons ratio", 0.30) update!(bracket_elements, "density", 7.80E-9) update!(adapterplate_elements, "youngs modulus", 165.0E3) update!(adapterplate_elements, "poissons ratio", 0.275) update!(adapterplate_elements, "density", 7.10E-9) add_elements!(bracket, bracket_elements) add_elements!(bracket, adapterplate_elements)
Boundary conditions can be created from node sets.
Problem(problem_type, problem_name::String, problem_dimension, parent_field_name::String)
function is used again to perform this. In this method the problem type is
parent_field_name is the type of the Dirichlet variable
(“temperature”, “displacement”, etc.).
Then the fixed nodal elements are collected from the input file with the
The displacements are then updated with
update!(node_set_name::String, parent_field_name direction::String, value)
direction is the direction of the displacement and
value is the
value of the nodal displacement which of course is 0.0 since our elements
# create a boundary condition from a node set fixed = Problem(Dirichlet, "fixed", 3, "displacement") fixed_elements = create_nodal_elements(mesh, "Face_constraint_1") update!(fixed_elements, "displacement 1", 0.0) update!(fixed_elements, "displacement 2", 0.0) update!(fixed_elements, "displacement 3", 0.0)
JuliaFEM allows new functions to be built with the help of other JuliaFEM functions. For example we need now a helper function to create tie contacts to our model.
Our function is called
create_interface and it has three variables: mesh,
slave and master.
mesh refers to our input file name that is defined at
the begining of this document,
slave is the name of our slave surface in
the input file and
master is the name of the master surface. The function
Problem() function with the
update! function from the JuliaFEM library.
""" A helper function to create tie contacts. """ function create_interface(mesh::Mesh, slave::String, master::String) interface = Problem(Mortar, "tie contact", 3, "displacement") interface.properties.dual_basis = false slave_elements = create_surface_elements(mesh, slave) master_elements = create_surface_elements(mesh, master) nslaves = length(slave_elements) nmasters = length(master_elements) update!(slave_elements, "master elements", master_elements) interface.elements = [slave_elements; master_elements] return interface end
Interfaces can now be applied with our own function
create_interface(mesh, slave::String, master::String) that collects necessary
information from our input file and creates a tie contact.
# call the helper function to create tie contacts tie1 = create_interface(mesh, "LDUBracketToAdapterplate1", "Adapterplate1ToLDUBracket") tie2 = create_interface(mesh, "LDUBracketToAdapterplate2", "Adapterplate2ToLDUBracket")
All problems need to be added into
solver_type is the type of the solver (Modal, Linear, Nonlinear).
In this example we are using a modal solver that solves generalized eigenvalue
problems Ku = Muλ since we are calculating natural frequencies.
The results can be imported to xdmf file format for further review. This
is performed by typing
solver_name.xdmf = Xdmf(result_file_name::String)
solver_name is the name of our solver which we defined and
result_file_name is the name we want to give our xdmf result file.
Yet we need to specify some properties for our analysis. We only want to
calculate the first six frequencies for our model. This can be done by first
solver_name.properties.nev = value where
nev refers to the number
of eigenmodes and
value is the number of eigenmodes which are to be calculated,
and then typing
bracket_freqs.properties.which = :SM where
which refers to
the type of the eigenmodes (:SM, :LM , etc.) and
:SM specifies that the eigen
modes to be calculated shall be the smallest ones.
Finally by simply typing
solver_name() we are commanding JuliaFEM to start
# add the field and the boundary problems to the solver bracket_freqs = Solver(Modal, bracket, fixed, tie1, tie2) # save results to Xdmf data format ready for ParaView visualization bracket_freqs.xdmf = Xdmf("results") # solve 6 smallest eigenvalues bracket_freqs.properties.nev = 6 bracket_freqs.properties.which = :SM bracket_freqs()
JuliaFEM gives the following calculation results for the analysis.