Home / Examples / Stress Analysis [Galileo] / Example 60: Warp of Substrate in the Cooling Process of Resin

Example 60: Warp of Substrate in the Cooling Process of Resin

General

Epoxy resin is coated on an alumina substrate and cured at 200℃ and then the substrate is cooled down to 25℃.
The warp caused by the difference in thermal expansion coefficient between alumina and epoxy resin in the cooling process is solved.
A resin material is used whose physical properties change greatly at the glass transition temperature of 140℃. It is generally recommended to treat such material as viscoelastic material.
In this example, the following three material models will be compared: 1) viscoelasticity, 2) elasticity, and 3) viscoelasticity (simple setting).
See [Analysis of Viscoelastic Materials] and [Viscoelasticity (Simple setting)] for more details.
The deformation, the displacement distribution and the stress distribution are solved.
Unless specified in the list below, the default conditions will be applied.

Results will vary depending on Femtet version and the PC environment.

Analysis Space

Item	Settings
Analysis Space	3D
Model Unit	mm

Analysis Conditions

The temperature is applied evenly on the model.

Select Thermal Load and set the reference temperature and the reached temperature.

There is no need to couple with the thermal analysis [Watt].

Item	Settings
Solver	Stress Analysis [Galileo]
Analysis Type	Static Analysis
Options	Select Thermal Load

For the models 1) viscoelasticity and 3) viscoelasticity (simple setting), Step/Thermal Load tab is set as follows.

Cooling speed is 1℃/s from 200℃ to 25℃. To perform analysis every 5℃, set Time to 175 and Substeps to 35.

Tab

Setting Item

Settings

Step/Thermal Load

Time Setting

Set up

Reference Temperature

200 [deg]

Step/Reached Temperature Setting

Step	Time [s]	Substeps	Reached Temperature [deg]
1	175	35	25

Options for the Nonlinear Analysis

Save the results of substeps : Select

For the model 3) elasticity, the setting is as follows.

Tab

Setting Item

Settings

Step/Thermal Load

Step Setting

Multi-step thermal load analysis

Time Setting

Set up

Reference Temperature

200 [deg]

Step/Reached Temperature Setting

Step	Time [s]	Substeps	Reached Temperature [deg]
1	175	35	25

Options for the Multi-Step Analysis

Save the results of substeps : Select

Graphical Objects

This model consists two boxes for alumina substrate and epoxy resin.

We set the symmetric boundary conditions in X and Y directions.

To solve the amount of warp, displacement of the center is fixed for reference.

Body Attributes and Materials

Body Number/Type	Body Attribute Name	Material Name
0/Solid	board	001_Alumina *
1/Solid	resin	1. Viscoelast_Mat 2. Elast_Mat 3. SimpleViscoelast_Mat

(*) Available from the material DB

Material setting is done as follows with the data of dynamic modulus.

See [Converting the Measurement Data of Viscoelastic Materials] for the measurement data of the dynamic modulus.

Material Name	Tab	Properties
Viscoelast_Mat	Coefficient of Linear Thermal Expansion	Temperature Dependency: Yes
Viscoelast_Mat	Viscoelasticity	Defined by: Dynamic Modulus [temp/freq response] Relaxation Table : Use the csv file below. Viscoelast_Mat.csv
Elsat_Mat	Coefficient of Linear Thermal Expansion	Same as Viscoelast_Mat
Elsat_Mat	Elasticity	Temperature Dependency: Yes Material Type: Elastic The file below is obtained using the storage modulus measured at 1Hz and Poisson's ratio of 0.3. Enter the data in the file into the table. Elast_Mat.csv
SimpleViscoelast_Mat	Coefficient of Linear Thermal Expansion	Same as Viscoelast_Mat
SimpleViscoelast_Mat	Elasticity	Temperature Dependency: Yes Material Type: Viscoelasticity Setting by: Table Poisson's Ratio: 0.3 Glass Transition Temperature (Tg): 140 [deg] Enter the storage modulus measured at 1Hz, which is in the csv file below, into the table. SimpleViscoelast_Mat.csv

Boundary Conditions

Displacement and face of symmetry are set as follows.

Boundary Condition Name/Topology	Tab	Boundary Condition Type	Settings
Fix_all/Vertex	Mechanical	Displacement	Select all X/Y/Z components UX=0, UY=0, UZ=0
Sym_x/Face	Symmetry/Continuity	Symmetry	Select Reflective
Sym_y/Edge	Symmetry/Continuity	Symmetry	Select Reflective

Results

At the end of the analysis of model 2), the warning message will appear as below recommending to use the model 3).

With the following field graph setting, the Z displacements at the tip of substrate are displayed.

Select Horizontal axis: Mode (frequency, time, step, etc) for Type and select Horizontal axis: Temperature.

Coordinates: (5, 5, 0.4)

Mode: 0-34

The results are shown below. The maximum value of the vertical axis is 1.2 mm to compare the three models.

1) Viscoelasticity	2) Elasticity	3) Viscoelasticity (Simple setting)

Comparing models 1) Viscoelasticity and 2) Elasticity, 2) shows larger warp of around 1.15 mm while 1) is around 0.4 mm.

Model 3) Viscoelasticity (Simple setting) shows the same value of 0.4 mm as model 1).

If time-dependency data of elasticity is used for analysis, 3) Viscoelasticity (Simple setting) will give accurate results as the warning message above indicates.