PDF
Thermal Expansion in a MEMS Device
Introduction
The purpose of this model is to exemplify the use of the Material Library in COMSOL Multiphysics. This library contains more than 20,000 property functions for over 2600 materials. The larger part of these properties are mechanical and thermal properties for solid materials given as functions of temperature. You need the Material Library to build the model.
The example also shows how to set up a model of thermal expansion when the structure is constrained.
Note: This model requires the Material Library.
Thermal expansion is a common method used in the microscale to displace a part of a component, for example in an actuator.
Model Definition
The figure below shows the model geometry:
Figure 1: Geometry of the device.
The model consists of two sets of physics:
•
A thermal balance with a heat source in the device, originating from Joule heating (ohmic heating). Air cooling is applied on the boundaries except at the position where the device is attached to a circuit board, where a thermal insulation condition is set.
•
A force balance for the structural analysis with a volume load caused by thermal expansions. The device is fixed at the positions where it is attached to a circuit board (see Figure 1). The effect of possible thermal expansion for the circuit board is investigated.
The device is made of the copper-beryllium alloy UNS C17500, and the circuit board is made of FR4 material.
The thermal balance consists of a balance of flux at steady state. The heat flux is given by conduction only. The heat source is a constant heat source of 1·108 W/m3. The air cooling at the boundaries is expressed using a constant heat transfer coefficient of 10 W/m2 and an ambient temperature of 298 K.
The expression for thermal expansion requires a strain reference temperature for the copper-beryllium alloy, which in this case is 298 K.
All other thermal and mechanical properties are obtained from the Material Library.
Results and Discussion
The following figure shows the temperature distribution in the device. The heat source increases the temperature to around 323.67 K from an ambient temperature of 298 K. The temperature varies less than 1/100 of a degree in the device.
Figure 2: Temperature field in the device. The edges of the original geometry are shown in black. The deformed shape is exaggerated by a factor of 200.
The following figures show the stress field in the deformed device with fully constrained attachment boundaries (Figure 3), and with the expansion effect taken into account for the circuit board (Figure 4). The latter case leads to certain relaxation of the constraint applied to the device boundaries attached to the board. The resulting maximum von Mises stress becomes less by an order of magnitude. The stress is well within the elastic region for the material. The two latter solutions are juxtaposed in the same plot with common color range in Figure 5.
.
Figure 3: The von Mises stress in the deformed structure with fully constrained attachment boundaries. The edges of the original geometry are shown in black. The deformed shape is exaggerated by a factor of 200.
Figure 4: The von Mises stress in the deformed structure when the circuit board thermal expansion effect is modeled. The deformed shape is exaggerated by a factor of 200.
Figure 5: Comparison of the von Mises stress with and without thermal expansion effect in the circuit board modeled.
Application Library path: MEMS_Module/Sensors/thermal_expansion
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  3D.
2
In the Select Physics tree, select Structural Mechanics>Thermal-Structure Interaction>Thermal Stress, Solid.
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies>Stationary.
6
Click  Done.
Geometry 1
1
In the Model Builder window, under Component 1 (comp1) click Geometry 1.
2
In the Settings window for Geometry, locate the Units section.
3
From the Length unit list, choose µm.
Work Plane 1 (wp1)
1
In the Geometry toolbar, click  Work Plane.
2
In the Settings window for Work Plane, click  Show Work Plane.
Work Plane 1 (wp1)>Plane Geometry
In the Model Builder window, click Plane Geometry.
Work Plane 1 (wp1)>Rectangle 1 (r1)
1
In the Work Plane toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 10.
4
In the Height text field, type 80.
5
Locate the Position section. In the xw text field, type -100.
6
In the Work Plane toolbar, click  Build All.
Work Plane 1 (wp1)>Copy 1 (copy1)
1
In the Work Plane toolbar, click  Transforms and choose Copy.
2
Select the object r1 only.
3
In the Settings window for Copy, locate the Displacement section.
4
In the xw text field, type 30.
5
In the Work Plane toolbar, click  Build All.
Work Plane 1 (wp1)>Circle 1 (c1)
1
In the Work Plane toolbar, click  Circle.
2
In the Settings window for Circle, locate the Size and Shape section.
3
In the Radius text field, type 10.
4
Locate the Position section. In the xw text field, type -80.
5
In the yw text field, type 80.
6
In the Work Plane toolbar, click  Build All.
Work Plane 1 (wp1)>Circle 2 (c2)
1
In the Work Plane toolbar, click  Circle.
2
In the Settings window for Circle, locate the Size and Shape section.
3
In the Radius text field, type 20.
4
Locate the Position section. In the xw text field, type -80.
5
In the yw text field, type 80.
6
In the Work Plane toolbar, click  Build All.
Work Plane 1 (wp1)>Rectangle 2 (r2)
1
In the Work Plane toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 40.
4
In the Height text field, type 20.
5
Locate the Position section. In the xw text field, type -100.
6
In the yw text field, type 60.
7
In the Work Plane toolbar, click  Build All.
8
Click the  Zoom Extents button in the Graphics toolbar.
Work Plane 1 (wp1)>Difference 1 (dif1)
1
In the Work Plane toolbar, click  Booleans and Partitions and choose Difference.
2
Select the object c2 only.
3
In the Settings window for Difference, locate the Difference section.
4
Find the Objects to subtract subsection. Click to select the  Activate Selection toggle button.
5
Select the objects c1 and r2 only.
6
In the Work Plane toolbar, click  Build All.
Work Plane 1 (wp1)>Array 1 (arr1)
1
In the Work Plane toolbar, click  Transforms and choose Array.
2
Click in the Graphics window and then press Ctrl+A to select all objects.
3
In the Settings window for Array, locate the Size section.
4
In the xw size text field, type 4.
5
Locate the Displacement section. In the xw text field, type 50.
6
In the Work Plane toolbar, click  Build All.
7
Click the  Zoom Extents button in the Graphics toolbar.
Work Plane 1 (wp1)>Rectangle 3 (r3)
1
In the Work Plane toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 30.
4
In the Height text field, type 10.
5
Locate the Position section. In the xw text field, type -70.
6
In the Work Plane toolbar, click  Build All.
Work Plane 1 (wp1)>Array 2 (arr2)
1
In the Work Plane toolbar, click  Transforms and choose Array.
2
Select the object r3 only.
3
In the Settings window for Array, locate the Size section.
4
In the xw size text field, type 3.
5
Locate the Displacement section. In the xw text field, type 50.
6
In the Work Plane toolbar, click  Build All.
Extrude 1 (ext1)
1
In the Model Builder window, under Component 1 (comp1)>Geometry 1 right-click Work Plane 1 (wp1) and choose Extrude.
2
In the Settings window for Extrude, locate the Distances section.
3
In the table, enter the following settings:
Distances (µm)
10
4
Click  Build All Objects.
Form Union (fin)
1
In the Model Builder window, click Form Union (fin).
2
In the Settings window for Form Union/Assembly, click  Build Selected.
3
Click the  Zoom Extents button in the Graphics toolbar.
Next, create selections for use when defining the boundary conditions.
Definitions
Fixed
1
In the Definitions toolbar, click  Box.
2
In the Settings window for Box, type Fixed in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Boundary.
4
Locate the Box Limits section. In the y maximum text field, type 1[um].
5
Locate the Output Entities section. From the Include entity if list, choose Entity inside box.
Heat Flux
1
In the Definitions toolbar, click  Complement.
2
In the Settings window for Complement, type Heat Flux in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Boundary.
4
Locate the Input Entities section. Under Selections to invert, click  Add.
5
In the Add dialog box, select Fixed in the Selections to invert list.
6
Click OK.
Top
1
In the Definitions toolbar, click  Box.
2
In the Settings window for Box, type Top in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Boundary.
4
Locate the Box Limits section. In the z minimum text field, type 1[um].
5
Locate the Output Entities section. From the Include entity if list, choose Entity inside box.
Add Material
1
In the Home toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Material Library>Copper Alloys>UNS C17500>UNS C17500 [solid].
4
Click Add to Component in the window toolbar.
5
In the Home toolbar, click  Add Material to close the Add Material window.
Materials
UNS C17500 [solid] (mat1)
1
In the Settings window for Material, locate the Material Contents section.
2
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Poisson’s ratio
nu
0.34
1
Young’s modulus and Poisson’s ratio
Multiphysics
Thermal Expansion 1 (te1)
1
In the Model Builder window, under Component 1 (comp1)>Multiphysics click Thermal Expansion 1 (te1).
2
In the Settings window for Thermal Expansion, locate the Model Input section.
3
Click  Go to Source for Volume reference temperature.
Global Definitions
Default Model Inputs
1
In the Model Builder window, under Global Definitions click Default Model Inputs.
2
In the Settings window for Default Model Inputs, locate the Browse Model Inputs section.
3
Find the Expression for remaining selection subsection. In the Volume reference temperature text field, type 298[K].
Solid Mechanics (solid)
Fixed Constraint 1
1
In the Model Builder window, under Component 1 (comp1) right-click Solid Mechanics (solid) and choose Fixed Constraint.
2
In the Settings window for Fixed Constraint, locate the Boundary Selection section.
3
From the Selection list, choose Fixed.
Heat Transfer in Solids (ht)
In the Model Builder window, under Component 1 (comp1) click Heat Transfer in Solids (ht).
Heat Source 1
1
In the Physics toolbar, click  Domains and choose Heat Source.
2
In the Settings window for Heat Source, locate the Domain Selection section.
3
From the Selection list, choose All domains.
4
Locate the Heat Source section. In the Q0 text field, type 1e8.
Heat Flux 1
1
In the Physics toolbar, click  Boundaries and choose Heat Flux.
2
In the Settings window for Heat Flux, locate the Boundary Selection section.
3
From the Selection list, choose Heat Flux.
4
Locate the Heat Flux section. From the Flux type list, choose Convective heat flux.
5
In the h text field, type 10.
6
In the Text text field, type 298.
Mesh 1
Mapped 1
1
In the Mesh toolbar, click  Boundary and choose Mapped.
2
In the Settings window for Mapped, locate the Boundary Selection section.
3
From the Selection list, choose Top.
Size 1
1
Right-click Mapped 1 and choose Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Extremely fine.
4
Click  Build All.
Swept 1
In the Mesh toolbar, click  Swept.
Distribution 1
1
Right-click Swept 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Distribution section.
3
In the Number of elements text field, type 3.
4
Click  Build All.
5
Click the  Zoom Extents button in the Graphics toolbar.
Fixed Board
1
In the Model Builder window, click Study 1.
2
In the Settings window for Study, type Fixed Board in the Label text field.
3
In the Home toolbar, click  Compute.
Results
Stress (solid)
The first default plot shows the von Mises stress in the deformed material. Add markers to show the minimum and maximum displacement, and adjust the deformation scaling to reproduce the plot shown in Figure 3.
Volume 1
1
In the Model Builder window, expand the Stress (solid) node, then click Volume 1.
2
In the Settings window for Volume, locate the Expression section.
3
From the Unit list, choose MPa.
Stress (solid)
In the Model Builder window, click Stress (solid).
Max/Min Volume 1
1
In the Stress (solid) toolbar, click  More Plots and choose Max/Min Volume.
2
In the Settings window for Max/Min Volume, locate the Coloring and Style section.
3
From the Color list, choose Blue.
Deformation
1
In the Model Builder window, expand the Results>Stress (solid)>Volume 1 node, then click Deformation.
2
In the Settings window for Deformation, locate the Scale section.
3
Select the Scale factor check box. In the associated text field, type 200.
4
In the Stress (solid) toolbar, click  Plot.
5
Click the  Go to Default View button in the Graphics toolbar.
Temperature (ht)
The second default plots shows the temperature field that should be similar to that displayed in Figure 2.
1
In the Model Builder window, under Results click Temperature (ht).
2
In the Settings window for 3D Plot Group, click to expand the Number Format section.
3
Select the Manual color legend settings check box.
4
In the Precision text field, type 6.
5
In the Temperature (ht) toolbar, click  Plot.
Next include the thermal expansion effect for the circuit board. First, add another material to represent it.
Add Material
1
In the Home toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Built-in>FR4 (Circuit Board).
4
Right-click and choose Add to Component 1 (comp1).
5
In the Home toolbar, click  Add Material to close the Add Material window.
Materials
FR4 (Circuit Board) (mat2)
1
In the Settings window for Material, locate the Geometric Entity Selection section.
2
From the Geometric entity level list, choose Boundary.
3
From the Selection list, choose Fixed.
Now add a Thermal Expansion subfeature to the Fixed Constraint feature, and define temperature and reference temperature as model inputs on boundaries.
Solid Mechanics (solid)
Fixed Constraint 1
In the Model Builder window, under Component 1 (comp1)>Solid Mechanics (solid) click Fixed Constraint 1.
Thermal Expansion 1
1
In the Physics toolbar, click  Attributes and choose Thermal Expansion.
2
In the Settings window for Thermal Expansion, locate the Boundary Selection section.
3
From the Selection list, choose Fixed.
4
Locate the Model Input section. Click  Create Model Input for Volume reference temperature.
Shared Properties
Model Input 1
1
In the Model Builder window, under Component 1 (comp1)>Definitions>Shared Properties click Model Input 1.
2
In the Settings window for Model Input, locate the Definition section.
3
In the text field, type 298[K].
Solid Mechanics (solid)
Thermal Expansion 1
1
In the Model Builder window, under Component 1 (comp1)>Solid Mechanics (solid)>Fixed Constraint 1 click Thermal Expansion 1.
2
In the Settings window for Thermal Expansion, locate the Model Input section.
3
Click  Create Model Input for Temperature.
Shared Properties
Model Input 2
1
In the Model Builder window, under Component 1 (comp1)>Definitions>Shared Properties click Model Input 2.
2
In the Settings window for Model Input, locate the Definition section.
3
In the text field, type solid.T.
Add a second study for computation with board thermal expansion.
Add Study
1
In the Home toolbar, click  Add Study to open the Add Study window.
2
Go to the Add Study window.
3
Find the Studies subsection. In the Select Study tree, select General Studies>Stationary.
4
Click Add Study in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Expanded Board
1
In the Model Builder window, click Study 2.
2
In the Settings window for Study, type Expanded Board in the Label text field.
3
Locate the Study Settings section. Clear the Generate default plots check box.
4
In the Home toolbar, click  Compute.
Group and duplicate the existing plots, then set them to the newly created dataset.
Results
Isothermal Contours (ht), Stress (solid), Temperature (ht)
1
In the Model Builder window, under Results, Ctrl-click to select Stress (solid), Temperature (ht), and Isothermal Contours (ht).
2
Right-click and choose Group.
Fixed Board
In the Settings window for Group, type Fixed Board in the Label text field.
Expanded Board
1
Right-click Fixed Board and choose Duplicate.
2
In the Model Builder window, click Fixed Board 1.
3
In the Settings window for Group, type Expanded Board in the Label text field.
Stress (solid) 1
1
In the Model Builder window, click Stress (solid) 1.
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Dataset list, choose Expanded Board/Solution 2 (sol2).
4
In the Stress (solid) 1 toolbar, click  Plot.
The computed stress field and deformation should be similar to that shown in Figure 4.
Temperature (ht) 1
1
In the Model Builder window, click Temperature (ht) 1.
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Dataset list, choose Expanded Board/Solution 2 (sol2).
Isothermal Contours (ht) 1
1
In the Model Builder window, click Isothermal Contours (ht) 1.
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Dataset list, choose Expanded Board/Solution 2 (sol2).
Duplicate the first plot group to show both solutions in the same plot, like in Figure 5.
Stress Comparison
1
In the Model Builder window, right-click Stress (solid) and choose Duplicate.
2
Right-click Stress (solid) 2 and choose Move Out.
3
Right-click Stress (solid) 2 and choose Move Down.
4
In the Settings window for 3D Plot Group, type Stress Comparison in the Label text field.
5
Locate the Plot Settings section. Clear the Plot dataset edges check box.
Max/Min Volume 1
1
In the Model Builder window, expand the Stress Comparison node.
2
Right-click Results>Stress Comparison>Max/Min Volume 1 and choose Delete.
Line 1
1
In the Model Builder window, right-click Stress Comparison and choose Line.
2
In the Settings window for Line, locate the Expression section.
3
In the Expression text field, type 1.
4
Click to expand the Title section. From the Title type list, choose None.
5
Locate the Coloring and Style section. From the Coloring list, choose Uniform.
6
From the Color list, choose Black.
7
Click to expand the Inherit Style section. From the Plot list, choose Volume 1.
8
Clear the Color check box.
9
Clear the Color and data range check box.
Deformation 1
Right-click Line 1 and choose Deformation.
Line 1, Volume 1
1
In the Model Builder window, under Results>Stress Comparison, Ctrl-click to select Volume 1 and Line 1.
2
Right-click and choose Duplicate.
Volume 2
1
In the Settings window for Volume, locate the Data section.
2
From the Dataset list, choose Expanded Board/Solution 2 (sol2).
3
Click to expand the Title section. From the Title type list, choose None.
4
Click to expand the Inherit Style section. From the Plot list, choose Volume 1.
Translation 1
1
Right-click Volume 2 and choose Translation.
2
In the Settings window for Translation, locate the Translation section.
3
In the y text field, type 120.
Line 2
1
In the Model Builder window, under Results>Stress Comparison click Line 2.
2
In the Settings window for Line, locate the Data section.
3
From the Dataset list, choose Expanded Board/Solution 2 (sol2).
Translation 1
1
Right-click Line 2 and choose Translation.
2
In the Settings window for Translation, locate the Translation section.
3
In the y text field, type 120.
4
In the Stress Comparison toolbar, click  Plot.
Line 2
1
In the Model Builder window, click Line 2.
2
Click  Plot.
3
Click the  Go to Default View button in the Graphics toolbar.
Volume 1
1
In the Model Builder window, click Volume 1.
2
In the Settings window for Volume, locate the Coloring and Style section.
3
From the Color table transformation list, choose Nonlinear.
4
Set the Color calibration parameter value to -1.5 to show better color resolution for low values.
Stress Comparison
1
In the Model Builder window, click Stress Comparison.
2
In the Settings window for 3D Plot Group, locate the Plot Settings section.
3
From the View list, choose New view.
4
In the Stress Comparison toolbar, click  Plot.
Finally, disable the circuit board thermal expansion in the first study, so that you can compute the fixed configuration again.
Fixed Board
Step 1: Stationary
1
In the Model Builder window, under Fixed Board click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Physics and Variables Selection section.
3
Select the Modify model configuration for study step check box.
4
In the tree, select Component 1 (comp1)>Solid Mechanics (solid)>Fixed Constraint 1>Thermal Expansion 1.
5
Click  Disable.