Accelerated Life Testing

Fatigue testing of nonlinear materials with a creep mechanism is a time consuming process. In accelerated life testing, the experiment time is greatly reduced by subjecting the material to testing conditions in excess of the operating ones. In this model an aggressive thermal load cycle is simulated and, its effect on the fatigue life of a solder joint is examined.

This example demonstrates how to evaluate fatigue driven by a specific strain or energy quantity and therefore a simple schematic representation of an electronic component is used. Moreover, only one cycle is simulated as opposed to several that are required to obtain a steady state cycle when working with nonlinear materials. This simplification is motivated by the fact that the purpose of this model is to show how to evaluate fatigue based on a user defined variable. The required strain and energy variables are defined explicitly via ordinary differential equations and calculated during the simulation of the thermal load cycle.

Model Definition

Microelectronic components consist of several materials. When subjected to temperature changes, differences in coefficients of thermal expansion introduce a stress concentration caused by the discontinuous deformation. With consecutive heating and cooling, the stress state changes back and forth until the component finally fails in fatigue.

This example uses a schematic geometry which captures the structural function of the main components rather than an accurate geometry of the microelectronic component. A symmetric model is used and half of its geometry is shown in Figure 1. The total size of the resistor and of the printed circuit board (PCB) is 4 × 0.5 mm2. The size of the solder is 0.5 × 0.25 mm2. It is assumed that the structure is in plane strain conditions.

The resistor is made of alumina, the printed circuit board is a fiberglass based laminate and the solder joint is an SnAgCu alloy that responds both linearly and nonlinearly to an applied load. The elastic and the thermal properties of the materials are given in Table 1.

Figure 1: Geometry of the electronic component. The dashed line indicates symmetry.

Table 1: Elastic and thermal properties of Materials.
Material	Young’s modulus (GPa)	Poisson’s ratio	Coefficient of thermal expansion (ppm/°C)
Fiberglass	22	0.4	21
SnAgCu	50	0.4	21
Alumina	300	0.22	8

The solder material nonlinearity is creep, which is a material behavior where deformation changes over the time although the stress remain constant. Generally materials creep with different rates in three distinct phases: primary creep, secondary creep and tertiary creep; see Figure 2.

Figure 2: Creep strain development at constant stress. Primary creep denoted with 1, secondary with 2 and tertiary with 3.

The secondary creep is also called the steady state creep since the strain rate at constant stress is constant. In the representation of the solder material the primary and tertiary creeps are disregarded while the steady state creep is represented with a double Norton law according to

where

is the creep rate, σe is the equivalent stress and AI, nI, σn, AII, and nII are the material constants given by Table 2. The first term represents a creep mechanism observed at low stresses while the second term describes the dominating creep behavior at high stresses, see Figure 3.

Table 2: Creep Material Constants.
Material constant	Value
AI	8.03·10-12 1/s
nI	3
σn	1 MPa
AII	1.96·10-23 1/s
nII	12

Figure 3: Creep model for the solder SnAgCu solder material.

Two fatigue models are evaluated. In the first, the lifetime is based on a Coffin-Manson type model. The development of the shear strain controls the fatigue according to

where ΔγII is the range of the creep shear strain of the second creep mechanism experienced in a load cycle and N is the number of cycles to fatigue.

The second fatigue evaluation depends on the energy dissipation and follows a Morrow type criterion according expressed as

where ΔWII is the dissipated creep energy of the second creep mechanism during a load cycle.

Results and Discussion

First the user defined creep strains and energies are verified. The creep strain calculated in the structural analysis is a summation of creep contributions from different mechanisms and thus

where

is the creep strain of the first mechanism and

is the creep strain contribution from the second mechanism. The individual contributions of each creep mechanism are calculated in two separate ODE interfaces. A composition of creep results is shown in Figure 4.

Figure 4: Creep strain history. The equivalent creep strain is shown.

From the figure it is clear that the creep strain calculated using the Nonlinear Structural Materials Module equals the sum of the creep strains calculated with the user defined method.

The creep energy dissipation can also be calculated using the additive decomposition since

where δ denotes an increment and Wc denotes the energy dissipation density. The results of the energy comparison in Figure 5 shows a perfect agreement between values calculated by the built-in materials and the user defined material.

Figure 5: The energy dissipation history.

The fatigue lives predicted by the Coffin-Manson type model and the Morrow type model are shown in Figure 6 and Figure 7 respectively. The predicted life differs by approximately a factor of two, which is not uncommon when using fatigue models of different types, with some uncertainty in the model parameters. Both models indicate that the upper left corner is the critical point in the assembly.

Figure 6: Fatigue life based on the shear strain.

Figure 7: Fatigue life based on the dissipated energy.

Notes About the COMSOL Implementation

Fatigue can be evaluated using many different models. Several models share the same mathematical form. This is the case for the Coffin-Manson based and Morrow based models where the only difference is the controlling strain or energy measure. In rocks and rubbers it is commonly the elastic strain energy or the total strain energy that controls fatigue while in materials subjected to cyclic creep, the dissipated energy controls the fatigue. The Coffin-Manson model that initially related plastic strain to fatigue life has been modified by several researchers that propose a variety of different strain measures as the fatigue controlling mechanism.

In COMSOL Multiphysics, the Morrow and the Coffin-Manson relations

can be modified so that the fatigue evaluation is based on a user defined energy density, W, or strain, ε. If the variable controlling fatigue is already defined in a physics interface, it can be directly specified in the fatigue model node. The variable must be specified together with the corresponding physics interface tag (for example, solid.Ws when using the elastic strain energy density). When the variable is not defined in a physics interface, it can be calculated using an ODE Interface. This procedure is demonstrated in this model, where the fatigue is dependent on a specific creep strain and a specific dissipated energy density.

The basic form for an ODE is

(1)

where u is the field variable, t is the time, ea denotes the mass coefficient matrix, da denotes the damping coefficient matrix and f is the source term. The development of creep following the Norton’s law is defined with

(2)

where ij denotes a specific component, σe is the effective von Mises stress, sij is the deviatoric stress, and A, σref and n are material constants. Since the problem is a 2D plane stress analysis, only strains in x, y, z, and xy directions can develop. This gives 4 dependent variables: ecx, ecy, ecz, and ecxy. By comparing the first relation of Equation 2 with Equation 1 it can be identified that there is no contribution from the mass matrix, the damping matrix is an identity matrix and the source term equals the right-hand side of the first relation in Equation 2. This relation contains both the deviatoric stress tensor and the equivalent stress. Since both are already defined in the Solid Mechanics interface, it seems that they can be used in the definition of the source term. COMSOL Multiphysics requires, however, that the derivatives of all user-defined variables can be evaluated at all calculation steps of the analysis. At zero stress the numerical derivative of the equivalent stress

tries to evaluate a negative power of zero. A remedy to this challenge is to provide your own definition of the equivalent stress with a small addition of stress.

The nonzero stress ensures a finite derivative at stress free conditions. In the example a stress addition of 1Pa was chosen. This gives a negligible contribution to the equivalent stress since the resulting stresses have the order of magnitude of MPa.

In addition to the dependent variables used for the creep strain components, one additional dependent variable, ece, for the equivalent creep strain as defined by the second relation in Equation 2 is needed. The source term for this relation can be defined using the built-in derivative operator in COMSOL Multiphysics. For example a partial derivative of u with respect to x is simply defined as d(u,x). By putting all together, the time derivatives of the five dependent variables ecx, ecy, ecz, ecxy, and ece become:

•

alpha*solid.sdevx

•

alpha*solid.sdevy

•

alpha*solid.sdevz

•

alpha*solid.sdevxy

•

(2/3*(d(ecx,TIME)^2+d(ecy,TIME)^2+d(ecz,TIME)^2+2*(d(ecxy,TIME)^2))+1e-20)^0.5

where alpha=3/2*A/s_mises*(s_mises/s_ref)^n and s_mises=sqrt(solid.sx^2+solid.sy^2+solid.sz^2-solid.sx*solid.sy-solid.sy*solid.sz-solid.sz*solid.sx+3*solid.sxy^2+(1e-6[MPa])^2).

The time derivative of the dissipated creep energy density is

By using the derivative operator, the source term for the dependent variable, Wc, is simply d(ece,TIME)*s_mises.

The calculation of the strain variables and the energy density must be made in separate ODE Interfaces since the units of both variables differ.

Fatigue_Module/Strain_Life/accelerated_life_testing

Modeling Instructions

From the menu, choose .

New

In the window, click

Add Component

In the toolbar, click

and choose .

Geometry 1

In the window for , locate the section.

From the list, choose .

Rectangle 1 (r1)

In the toolbar, click

In the window for , locate the section.

In the text field, type 2.

In the text field, type 0.5.

Rectangle 2 (r2)

In the toolbar, click

In the window for , locate the section.

In the text field, type 0.5.

In the text field, type 0.25.

Locate the section. In the text field, type 0.5.

Rectangle 3 (r3)

In the toolbar, click

In the window for , locate the section.

In the text field, type 2.

In the text field, type 0.5.

Locate the section. In the text field, type 0.75.

Point 1 (pt1)

In the toolbar, click

In the window for , locate the section.

In the text field, type 0.25.

In the text field, type 0.625.

Click

Click the

button in the toolbar.

Add Physics

In the toolbar, click

to open the window.

Go to the window.

In the tree, select .

Click in the window toolbar.

In the toolbar, click

to close the window.

Global Definitions

Parameters 1

In the window, under click .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Value	Description
A_I	8.03e-12 [1/s]	8.03E-12 1/s	Low stress creep rate coefficient
n_I	3	3	Low stress creep rate exponent
A_II	1.96e-23 [1/s]	1.96E-23 1/s	High stress creep rate coefficient
n_II	12	12	High stress creep rate exponent
s_ref	1[MPa]	1E6 Pa	Reference stress

Interpolation 1 (int1)

In the toolbar, click

and choose .

In the window for , locate the section.

In the text field, type thermLC.

In the table, enter the following settings:


t	f(t)
0	25
15	100
30	100
45	25
60	25

Locate the section. In the text field, type min.

In the text field, type degC.

Solid Mechanics (solid)

Linear Elastic Material 1

Click the

button in the toolbar.

In the dialog box, in the tree, select the check box for the node .

Click .

In the window, under click .

In the window for , click to expand the section.

Select the check box.

Thermal Expansion 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the T list, choose . In the associated text field, type thermLC(t).

Linear Elastic Material 1

In the window, click .

Creep 1

In the toolbar, click

and choose .

Select Domain 2 only.

In the window for , locate the section.

From the A list, choose . In the associated text field, type A_I.

From the σref list, choose . In the associated text field, type s_ref.

From the n list, choose . In the associated text field, type n_I.

Linear Elastic Material 1

In the window, click .

Creep 2

In the toolbar, click

and choose .

Select Domain 2 only.

In the window for , locate the section.

From the A list, choose . In the associated text field, type A_II.

From the σref list, choose . In the associated text field, type s_ref.

From the n list, choose . In the associated text field, type n_II.

Symmetry 1

In the toolbar, click

and choose .

Select Boundaries 11 and 12 only.

Fixed Constraint 1

In the toolbar, click

and choose .

Select Point 8 only.

Materials

PCB

In the window, under right-click and choose .

In the window for , type PCB in the text field.

Select Domain 1 only.

Locate the section. In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Young’s modulus	E	22[GPa]	Pa	Basic
Poisson’s ratio	nu	0.4	1	Basic
Density	rho	1	kg/m³	Basic
Coefficient of thermal expansion	alpha_iso ; alphaii = alpha_iso, alphaij = 0	21e-6	1/K	Basic

Solder

Right-click and choose .

In the window for , type Solder in the text field.

Select Domain 2 only.

Locate the section. In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Young’s modulus	E	50[GPa]	Pa	Basic
Poisson’s ratio	nu	0.4	1	Basic
Density	rho	1	kg/m³	Basic
Coefficient of thermal expansion	alpha_iso ; alphaii = alpha_iso, alphaij = 0	21e-6	1/K	Basic

Alumina

Right-click and choose .

In the window for , type Alumina in the text field.

Select Domain 3 only.

Locate the section. In the table, enter the following settings:


Property	Variable	Value	Unit	Property group
Young’s modulus	E	300[GPa]	Pa	Basic
Poisson’s ratio	nu	0.22	1	Basic
Density	rho	1	kg/m³	Basic
Coefficient of thermal expansion	alpha_iso ; alphaii = alpha_iso, alphaij = 0	8e-6	1/K	Basic

Definitions

Variables 1

In the window, under right-click and choose .

Define help variables for the user defined strains.

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Unit	Description
s_mises	sqrt(solid.sx^2+solid.sy^2+solid.sz^2-solid.sxsolid.sy-solid.sysolid.sz-solid.szsolid.sx+3solid.sxy^2+3solid.syz^2+3solid.sxz^2+(1e-6[MPa])^2)	N/m²
alpha_I	3/2A_I/s_mises(s_mises/s_ref)^n_I	m·s/kg
alpha_II	3/2A_II/s_mises(s_mises/s_ref)^n_II	m·s/kg

Add Physics

In the toolbar, click

to open the window.

Go to the window.

In the tree, select .

Click in the window toolbar.

In the tree, select .

Click in the window toolbar.

In the tree, select .

Click in the window toolbar.

In the toolbar, click

to close the window.

Domain ODEs and DAEs (dode)

In the window, under click .

Select Domain 2 only.

In the window for , locate the section.

In the table, enter the following settings:


Source term quantity	Unit
Custom unit	1/s

Click to expand the section. In the text field, type ec_I.

In the text field, type 5.

In the table, enter the following settings:


ecx_I
ecy_I
ecz_I
ecxy_I
ece_I

Set the same Gauss point integration order as in the built-in Norton material.

Click to expand the section. From the list, choose .

From the list, choose .

Distributed ODE 1

In the window, under click .

In the window for , locate the section.

In the f text-field array, type alpha_I*solid.sdevx on the first row.

In the f text-field array, type alpha_I*solid.sdevy on the second row.

In the f text-field array, type alpha_I*solid.sdevz on the third row.

In the f text-field array, type alpha_I*solid.sdevxy on the fourth row.

In the f text-field array, type

2/3*(d(ecx_I,TIME)^2+d(ecy_I,TIME)^2+d(ecz_I,TIME)^2+

2*(d(ecxy_I,TIME)^2))+(1e-20))^0.5

on the 5th row.

Domain ODEs and DAEs 2 (dode2)

In the window, under click .

Select Domain 2 only.

In the window for , locate the section.

In the table, enter the following settings:


Source term quantity	Unit
Custom unit	1/s

Locate the section. In the text field, type ec_II.

In the text field, type 5.

In the table, enter the following settings:


ecx_II
ecy_II
ecz_II
ecxy_II
ece_II

Locate the section. From the list, choose .

From the list, choose .

Distributed ODE 1

In the window, click .

In the window for , locate the section.

In the f text-field array, type alpha_II*solid.sdevx on the first row.

In the f text-field array, type alpha_II*solid.sdevy on the second row.

In the f text-field array, type alpha_II*solid.sdevz on the third row.

In the f text-field array, type alpha_II*solid.sdevxy on the fourth row.

In the f text-field array, type

2/3*(d(ecx_II,TIME)^2+d(ecy_II,TIME)^2+d(ecz_II,TIME)^2+

2*(d(ecxy_II,TIME)^2))+(1e-20))^0.5

on the 5th row.

Domain ODEs and DAEs 3 (dode3)

In the window, under click .

Select Domain 2 only.

In the window for , locate the section.

Click

In the dialog box, type energydensity in the text field.

Click

In the tree, select .

Click .

In the window for , locate the section.

In the table, enter the following settings:


Source term quantity	Unit
Custom unit	J/(s*m^3)

Locate the section. In the text field, type Wc.

In the text field, type 2.

In the table, enter the following settings:


Wc_I
Wc_II

Locate the section. From the list, choose .

From the list, choose .

Distributed ODE 1

In the window, click .

In the window for , locate the section.

In the f text-field array, type d(ece_I,TIME)*s_mises on the first row.

In the f text-field array, type d(ece_II,TIME)*s_mises on the second row.

Mesh 1

Free Triangular 1

In the toolbar, click

Size 1

Right-click and choose .

In the window for , locate the section.

From the list, choose .

Select Domain 2 only.

Locate the section. From the list, choose .

Click

Add Study

In the toolbar, click

to open the window.

Go to the window.

Find the subsection. In the tree, select .

Click in the window toolbar.

In the toolbar, click

to close the window.

Study 1

Step 1: Time Dependent

In the window for , locate the section.

From the list, choose .

In the text field, type range(0,0.5,14.5) range(14.6,0.1,15.4) range(15.5,0.5,29.5) range(29.6,0.1,30.4) range(30.5,0.5,44.5) range(44.6,0.1,45.4) range(45.5,0.5,60).

Solution 1 (sol1)

In the toolbar, click