# Two cubes of different materials

 Title Two cubes of different materials Tags elasticity tension bending Runnng time 1 sec See also 006-cylinder-pure-compression CAEplex case https://caeplex.com/p/a2c96 Available in HTML PDF ePub

# 1 Problem description

Two cubes of 10mm \times 10mm \times 10mm each share a common face (fig. 1). One cube is “hard” and has a Young’s modulus E=100~\text{GPa} and \nu=0.25. The other one is “soft” with E=10~\text{GPa} and \nu=0.35. The free end of the hard cube is fully fixed and the free face of the soft cylinder is loaded with a tensile force F_x=-200~\text{N} in the axial direction and a bending force F_z=-10~\text{N} in the transversal direction. The objective of the case is to compare the three different inter-element averaging (or lack of) methods to compute nodal values of secondary fields (i.e. strains and stresses) that Fino provides.

Figure 1: Two cubes of different materials CAD from CAEplex https://caeplex.com/p/a2c96 (rotate and zoom it).

# 2 Geometry and mesh

The two cubes are created with the OpenCASCADE kernel and then meshed by Gmsh:

SetFactory("OpenCASCADE");

a = 10;
Box(1) = {-a,-a/2,-a/2,a,a,a};
Box(2) = {0,-a/2,-a/2,a,a,a};
Coherence;

Mesh.CharacteristicLengthMax = 10;
Mesh.CharacteristicLengthMin = 4;
Mesh.Algorithm = 1;
Mesh.ElementOrder = 2;

Physical Surface("fixed", 1) = {1};

Physical Volume("solid1") = {1};
Physical Volume("solid2") = {2};


The mesh is excessively coarse to better illustrate the point of this case. The elements are still of second order in order to obtain non-uniform derivatives of the displacements within each element.

# 3 Input file

The annotated input file two-cubes.fin should be self-explanatory. The only important detail is that it reads a command line argument from Fino’s invocation which should be either always, never or material and is passed to the FINO_SOLVER SMOOTH keyword. Sec. 5 shows what the differences between these three modes are.

DEFAULT_ARGUMENT_VALUE 1 always
FINO_SOLVER SMOOTH $1 # put Fino in either "always", "never" or "material" mode MESH FILE_PATH two-cubes.msh DIMENSIONS 3 # read mesh file # material properties MATERIAL solid1 E 100e3 nu 0.25 # the names solid1 and solid2 are the MATERIAL solid2 E 10e3 nu 0.35 # physical groups in the .geo file PHYSICAL_GROUP NAME fixed BC fixed # fix one end face PHYSICAL_GROUP NAME load BC Fz=-10 Fx=-200 # load the other face FINO_STEP # solve the problem! # write a vtk file with the mode in the name MESH_POST FILE_PATH two-cubes-$1.vtk \
dudx dudy dudz \
dvdx dvdy dvdz \
dwdx dwdy dwdz \
sigmax sigmay sigmaz \
tauxy tauyz tauzx \
sigma sigma1 sigma2 sigma3 \
E VECTOR u v w

# 4 Execution

The parameters always, never and material are successively passed to the two-cubes.fin input above:

$gmsh -v 0 -3 two-cubes.geo$ fino two-cubes.fin always
$fino two-cubes.fin never$ fino two-cubes.fin material
\$

# 5 Results

Fig. 2 illustrates the difference in the computed stresses.

Figure 2: Von Mises stresses depending on the averaging scheme chosen in Fino.. a — always-averaged, b — never-averaged, c — material-averaged