FEM model¶
Finite Element Modelling (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 boundaries 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.
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 (see Figure 35).
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 case of a perfect conical indenter (\(h_\text{tip} = 0\text{nm}\)), a tip defect of 1nm giving a radius of \(R = 1.6\text{nm}\) is set into 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 the conical parts of a cono-spherical indenter, is calculated from the followig equation:
(114)¶\[h_\text{trans} = R(1-sin(\alpha))\]
Find here the Matlab function to calculate the tip radius: tipRadius.m.
Find here the Matlab function to calculate the transition depth: transitionDepth.m.
Find here the Matlab function to calculate 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.
Material properties¶
For each layers 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¶
The contact is defined by default frictionless for 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.
Boundaries 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 37 and Figure 38).
Indentation process is simulated by imposing a vertical displacement to the rigid indenter along the (\(z\)) axis (see Figure 37 and Figure 38). A value of 200nm for the indentation depth is set by default.
Warning
Indentation displacement is given in nanometers and is negative.
Generation of the Python script for ABAQUS¶
After material properties are configured (Young’s moduli and Poisson’s ratios) and the model geometry is given (thickness for each thin films), a Python script for ABAQUS can be generated by pressing the ‘FEM’ button.
The python script is saved in the folder where your nanoindentation results are stored.
To generate the FEM model in ABAQUS, apply the following procedure:
start ABAQUS
select the folder containing 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.
Outlooks¶
More recently in 2022, evaluation of thin film material properties are performed using FEM analysis coupled with artificial neural network (ANN) method [6].
References¶
Other links / References¶
ABAQUS documentation
Bhattacharya A.K. and Nix W.D., “Finite element analysis of cone indentation.” (1991).
Madsen D.T. et al. “Finite Element Simulation of Indentation Behavior of thin Films.” (1991).
Chen X. and Vlassak J.J., “A Finite Element Study on the Nanoindentation of Thin Films.” (2000).
He J.L. and Veprek S., “Finite element modeling of indentation into superhard coatings.” (2003).
Charleux L., “Micromécanique de l’essai d’indentation : expériences et simulations.”, PhD thesis, Institut National Polytechnique de Grenoble (2006).
Kopernik M. and Pietrzyk M., “2d numerical simulation of elasto-plastic deformation of thin hard coating systems in deep nanoindentation test with sharp indenter.” (2007).
Guo W., “On the influence of indenter tip geometry on the identification of material parameters in indentation testing.”, PhD thesis, University of Liège (2010).
Fourcade T., “Études des propriétés mécaniques de matériaux métalliques en couches minces”, PhD thesis - Université de Toulouse (2013).
Li Y. et al., “Models for nanoindentation of compliant films on stiff substrates” (2015).
Pöhl F., “Determination of unique plastic properties from sharp indentation” (2019).