FEM model

Finite element modeling (FEM) of conical indentation

The present model is a simulation of the conical nanoindentation process, using the FEM software ABAQUS.

The Matlab function used to generate a Python script for ABAQUS is : python_abaqus

The model is axisymmetric, with a geometry-dependent mesh and restricted boundary conditions.

Geometry of the (multilayer) sample

Each layer of the sample is characterized by its thickness (\(t_\text{i}\)).

The thickness of the substrate (\(t_\text{sub}\)) is set as 2 times the highest thin film thickness.

The width (\(w\)) of the sample is calculated as a function of the substrate thickness or the indenter tip defect.

No delamination is allowed between thin films or between thin film and substrate.

Note

Dimensions are in nm.

_images/fem_model_geometry.png

Figure 33 Geometry of the sample in the FEM model.

Geometry of the indenter

The indenter is defined as a rigid cono-spherical indenter. A spherical part is defined at the apex of the conical indenter, as shown below.

_images/conospherical_indenter.png

Figure 34 Scheme of a cono-spherical indenter.

The radius \(R\) of the spherical part is calculated from the tip defect \(h_\text{tip}\) and the cone angle \(\alpha\), using the following equation. For Berkovich, Vickers, and cube-corner indenters, the equivalent cone angle is used to set the cone angle.

(113)\[R = \frac{h_\text{tip}}{\frac{1}{sin(\alpha)} - 1}\]

In the case of a perfect conical indenter (\(h_\text{tip} = 0\text{nm}\)), a tip defect of 1 nm, corresponding to a radius of \(R = 1.6\text{nm}\), is set in the Python file. Defining a cono-spherical tip avoids the geometrical singularity at the apex of the perfect conical indenter, which would imply an infinite stress at the contact interface. But, any non-zero positive value for the tip radius can be set into the GUI.

The transition depth \(h_\text{trans}\) between the spherical and conical parts of a cono-spherical indenter is calculated from the following equation:

(114)\[h_\text{trans} = R(1-sin(\alpha))\]

See the Matlab function for calculating the tip radius: tipRadius.m.

See the Matlab function for calculating the transition depth: transitionDepth.m.

See the Matlab function for calculating the tip defect: tipDefect.m.

Mesh

The multilayer sample is divided by default into solid elements with eight nodes and axisymmetric deformation element CAX8R is adopted.

It is possible to divide the sample into solid elements with four nodes and with axisymmetric deformation element CAX4R, by changing the value of the variable “linear_elements” in the Matlab function python4abaqus from 0 (quadratic elements) to 1 (linear elements).

Note

  • CAX4R: A 4-node bilinear axisymmetric quadrilateral, reduced integration, hourglass control.

  • CAX3: A 3-node linear axisymmetric triangle.

  • CAX8R: An 8-node biquadratic axisymmetric quadrilateral, reduced integration.

  • CAX6M: A 6-node modified quadratic axisymmetric triangle.

_images/fem_model_mesh.png

Figure 35 Screenshot in Abaqus of the mesh example used in the FE model.

Material properties

For each layer of the multilayer sample, the material properties (Young’s modulus and Poisson’s ratio) are defined using the inputs given by the user from the GUI. Material properties are considered by default to be isotropic. The density is set by default to 1.0.

Note

Young’s moduli are in GPa.

Contact definition

By default, the contact is defined as frictionless in the tangential behavior and hard for the normal behavior.

The external surface of the indenter is defined as the “master” region and the top surface of the (multilayer) sample is defined as the “slave” region.

Note

Usually, the effect of friction may be neglected when indenter tips with half-angle larger than 60◦ are used (e.g.: Berkovich, Vickers) [1], [4], [2], [3] and [5].

Boundary conditions

Nodes are constrained along the rotation axis from moving in the radial direction (\(x\)). The nodes on the bottom surface of the sample are constrained along the radial axis from moving in the radial (\(x\)) and vertical (\(z\)) directions (see Figure 36 and Figure 37).

Indentation process is simulated by imposing a vertical displacement to the rigid indenter along the (\(z\)) axis (see Figure 36 and Figure 37). A value of 200nm for the indentation depth is set by default.

_images/fem_model_bc.png

Figure 36 Schematic of the boundary conditions used in the FE model.

_images/fem_model_parts_bc.png

Figure 37 Screenshot of the FE model with BCs in Abaqus.

Warning

Indentation displacement is given in nanometers and is negative.

Generation of the Python script for ABAQUS

After configuring the material properties (Young’s moduli and Poisson’s ratios) and specifying the model geometry (the thickness of each thin film), generate a Python script for ABAQUS by pressing the ‘FEM’ button.

The Python script is saved in the folder containing your nanoindentation results.

To generate the FEM model in ABAQUS, apply the following procedure:

  • start ABAQUS

  • Select the folder containing the input files: ‘File’ ==> ‘Set Work Directory…’

  • Select and run the Python file containing the FEM model (*.py): ‘File’ ==> ‘Run Script’

Note

Dimensions are in nm and Young’s moduli are in GPa, implying that load is in nN.

Results of the FEM simulation

The following pictures were obtained for a multilayer Au/Ti/SiO2/Si.

_images/fem_result_S_Mises.png

Figure 38 Screenshot of the Von Mises stress distribution at maximum load.

_images/fem_result_S_Mises_zoom.png

Figure 39 Screenshot (with a zoom in on the contact area) of the Von Mises stress distribution at maximum load.

_images/fem_result_U_magnitude.png

Figure 40 Screenshot (with a zoom in on the contact area) of the magnitude of the displacement at maximum load.

Future developments

More recently, thin-film material properties have been evaluated using FEM analysis coupled with an artificial neural network (ANN) [6].

References