exs_beambar2¶

Purpose:

Analysis of a combined beam and bar structure.

Description:

Consider a structure consisting of a beam with \(A_1=4.0 \times 10^{-3}\) m² and \(I_1=5.4 \times 10^{-5}\) m⁴ supported by two bars with \(A_2=1.0 \times 10^{-3}\) m². The beam as well as the bars have \(E=200\) GPa. The structure is loaded by a distributed load \(q=10\) kN/m. The corresponding finite element model consists of three beam elements and two bar elements and has 14 degrees of freedom.

Example:

The computation is initialized by importing CALFEM and NumPy. The topology matrices are defined separately for beam and bar elements, containing only the degrees of freedom:

import numpy as np
import calfem.core as cfc
import calfem.utils as cfu
import calfem.vis_mpl as cfv
edof1 = np.array([
    [1,  2,  3,  4,  5,  6],
    [4,  5,  6,  7,  8,  9],
    [7,  8,  9, 10, 11, 12]
])

edof2 = np.array([
    [13, 14,  4,  5],
    [13, 14,  7,  8]
])

K = np.array(np.zeros((14, 14)))
f = np.array(np.zeros((14, 1)))

The material and geometric properties are defined for beam and bar elements:

E = 200.e9
A1 = 4.e-3
I1 = 5.4e-5
A2 = 1.e-3

ep1 = [E, A1, I1]
ep4 = [E, A2]

eq1 = [0, 0]
eq2 = [0, -10e+3]

ex1 = np.array([0, 2])
ex2 = np.array([2, 4])
ex3 = np.array([4, 6])
ex4 = np.array([0, 2])
ex5 = np.array([0, 4])
ey1 = np.array([2, 2])
ey2 = np.array([2, 2])
ey3 = np.array([2, 2])
ey4 = np.array([0, 2])
ey5 = np.array([0, 2])

The element stiffness matrices are computed using beam2e() for beam elements and bar2e() for bar elements. Element load vectors from distributed loads are also computed:

Ke1 = cfc.beam2e(ex1, ey1, ep1)
Ke2, fe2 = cfc.beam2e(ex2, ey2, ep1, eq2)
Ke3, fe3 = cfc.beam2e(ex3, ey3, ep1, eq2)

Ke4 = cfc.bar2e(ex4, ey4, ep4)
Ke5 = cfc.bar2e(ex5, ey5, ep4)

The global stiffness matrix and load vector are assembled using assem():

K = cfc.assem(edof1[0, :], K, Ke1)
K, f = cfc.assem(edof1[1, :], K, Ke2, f, fe2)
K, f = cfc.assem(edof1[2, :], K, Ke3, f, fe3)
K = cfc.assem(edof2[0, :], K, Ke4)
K = cfc.assem(edof2[1, :], K, Ke5)

The system of equations is solved by specifying boundary conditions and using solveq(). The vertical displacement at the end of the beam is 13.0 mm:

CodeOutput

bc_dofs = np.array([1, 2, 3, 13, 14])
bc_vals = np.array([0.0, 0.0, 0.0, 0.0, 0.0])

a, r = cfc.solveq(K, f, bc_dofs, bc_vals)
cfu.disp_h2("Displacements a:")
cfu.disp_array(a)

cfu.disp_h2("Reaction forces r:")
cfu.disp_array(r)

Maximum vertical displacement: 0.009 m = 9.5 mm

The section forces are calculated using beam2s() and bar2s() from element displacements. This yields normal forces of -35.4 kN and -152.5 kN in the bars and maximum moment of 20.0 kNm in the beam:

CodeOutput

ed1 = cfc.extract_ed(edof1, a)
ed2 = cfc.extract_ed(edof2, a)

es1, _, _ = cfc.beam2s(ex1, ey1, ep1, ed1[0, :], eq1, nep=11)
es2, _, _ = cfc.beam2s(ex2, ey2, ep1, ed1[1, :], eq2, nep=11)
es3, _, _ = cfc.beam2s(ex3, ey3, ep1, ed1[2, :], eq2, nep=11)
es4 = cfc.bar2s(ex4, ey4, ep4, ed2[0, :])
es5 = cfc.bar2s(ex5, ey5, ep4, ed2[1, :])

cfu.disp_h2("es1 = ")
cfu.disp_array(es1, headers=["N", "Q", "M"])
cfu.disp_h2("es2 = ")
cfu.disp_array(es2, headers=["N", "Q", "M"])
cfu.disp_h2("es3 = ")
cfu.disp_array(es3, headers=["N", "Q", "M"])
cfu.disp_h2("es4 = ")
cfu.disp_array(es4, headers=["N"])
cfu.disp_h2("es5 = ")
cfu.disp_array(es5, headers=["N"])