PDF
Heating Circuit — Layered Shell Version
Introduction
Small heating circuits find use in many applications. For example, in manufacturing processes they heat up reactive fluids. Figure 1 illustrates a typical heating device shown in this model. The device consists of an electrically resistive layer deposited on a glass plate. The layer causes Joule heating when a voltage is applied to the circuit. The layer’s properties determine the amount of heat produced.
Figure 1: Geometry of a heating device.
In this particular model, there are three important design considerations:
•
Noninvasive heating
•
Minimal deflection of the heating device
•
Avoidance of overheating the process fluid
The heater must also work without failure. The first and second requirements are achieved by inserting a glass plate between the heating circuit and the fluid; it acts as a conducting separator. Glass is an ideal material for both these purposes because it is nonreactive and has a low coefficient of thermal expansion.
Overheating must be avoided due to the risk of self-ignition of the reactive fluid stream. Ignition is also the main reason for separating the electrical circuit from direct contact with the fluid. Heating devices are tailored for each application, making virtual prototyping very important for manufacturers.
For heating circuits in general, the detachment of the resistive layer often determines the failure rate. This is caused by excessive thermally induced interfacial stresses. Once the layer has detached, it gets locally overheated, which further accelerates the detachment. Finally, in the worst case, the circuit might overheat and burn. From this perspective, it is also important to study the interfacial tension due to the different thermal expansion coefficients of the resistive layer and the substrate as well as the differences in temperature. The geometric shape of the layer is a key parameter to design circuits for proper functioning. You can investigate all of the abovementioned aspects by modeling the circuit.
This multiphysics example simulates the electrical heat generation, the heat transfer, and the mechanical stresses and deformations of a heating circuit device. The model uses the Heat Transfer in Shells interface of the Heat Transfer Module in combination with the Electric Currents, Layered Shell interface from the AC/DC Module or the MEMS Module, and the Layered Shell interface from the Composite Materials Module.
Read more about the Composite Materials Module in the COMSOL blog, Introduction to the Composite Materials Module.
Note: In addition to the Composite Materials Module and the Structural Mechanics Module, this model requires the Heat Transfer Module and either the AC/DC Module or the MEMS Module. It is a layered shell version of the model Heating Circuit available in the AC/DC Module, Heat Transfer Module, and Structural Mechanics Module Application Libraries.
Model Definition
Figure 2 shows a drawing of the modeled heating circuit.
Figure 2: Drawing of the heating circuit deposited on a glass plate.
The device consists of a serpentine-shaped Nichrome resistive layer, 10 μm thick and 5 mm wide, deposited on a glass plate. At each end, it has a silver contact pad measuring 10 mm by 10 mm by 10 μm. When the circuit is in use, the deposited side of the glass plate is in contact with surrounding air, and the back side is in contact with the heated fluid. Assume that the edges and sides of the glass plate are thermally insulated.
Table 1 lists the resistor’s dimensions.
Table 1: Dimensions.
object
Length
Width
Thickness
Glass plate
130 mm
80 mm
2 mm
Pads and circuit
-
-
10 µm
Layered Shell Approach
Since this model uses a layered shell interface, in which the through thickness integration is inherent to the layered shell formulation itself, a surface geometry as shown in the Figure 3 is sufficient.
Figure 3: Layered shell version of the model geometry.
The layered shell geometry has many zones with layers of different materials and thicknesses. The spatial position of the different zones can be seen in Figure 4 and material and thicknesses for each zone can be seen in Figure 5.
The different zones of the layered shell are by default disconnected. Therefore, continuity conditions connecting layers from neighboring zones are required in all physics interfaces.
Figure 4: Zones with different layers in the layered shell geometry. The green zone has only glass layer, the red zone has glass and Nichrome layers, and yellow zone has glass and Silver layers.
Figure 5: Cross-sectional view of zones having layers of different material and thickness.
Boundary Conditions
During operation the resistive layer produces heat. Model the electrically generated heat using the Electric Currents, Layered Shell interface from the AC/DC Module or the MEMS Module. An electric potential of 12 V is applied to the pads. In the model, you achieve this effect by setting the potential at one edge of the first pad to 12 V, and that of one edge of the other pad to 0 V.
To model the heat transfer in the thin conducting layer, use the Heat Transfer in Shells interface. The heat rate per unit area (measured in W/m2) produced inside the thin layer is given by
(1)
where QDC = J · E = σ|∇tV|2 (W/m3) is the power density. The generated heat appears as an inward heat flux at the surface of the glass plate.
At steady state, the resistive layer dissipates the heat it generates in two ways: on its upside to the surrounding air (at 293 K), and on its downside to the glass plate. The glass plate is similarly cooled in two ways: on its circuit side by air, and on its back side by a process fluid (353 K). You model the heat fluxes to the surroundings using heat transfer coefficients, h. For the heat transfer to air, h = 5 W/(m2·K), representing natural convection. On the glass plate’s back side, h = 20 W/(m2·K), representing convective heat transfer to the fluid. The sides of the glass plate are insulated.
The model simulates thermal expansion using static structural mechanics analyses. It uses the Layered Shell interface for the glass plate as well as for the circuit layer. The stresses are set to zero at 293 K. You determine the boundary conditions for the Layered Shell interface by adding a rigid motion suppression node and restricting all rigid body modes.
Material Properties
Table 2 summarizes the material properties used in the model.
Table 2: Material properties.
Material
E [GPa]
 ν
α [1/K]
k [W/(m·K)]
ρ [kg/m3]
Cp [J/(kg·K)]
Silver
83
0.37
1.89e-5
420
10500
230
Nichrome
213
0.33
1e-5
15
9000
20
Glass
73.1
0.17
5.5e-7
1.38
2203
703
Results and Discussion
Figure 6 shows the heat that the resistive layer generates.
Figure 6: Stationary heat generation in the resistive layer when 12 V is applied.
The highest heating power occurs at the inner corners of the curves due to the higher current density at these spots. The total generated heat, as calculated by integration, is approximately 13.8 W.
Figure 7 shows the temperature of the resistive layer and the glass plate at steady state.
Figure 7: Temperature distribution in the heating device at steady state.
The highest temperature is approximately 424 K, and it appears in the central section of the circuit layer. Interestingly, the temperature differences between the fluid side and the circuit side of the glass plate are quite small because the plate is very thin. Using boundary integration, the integral heat flux on the fluid side evaluates to approximately 8.5 W. This means that the device transfers the majority of the heat it generates 8.5 W out of 13.8 W to the fluid, which is good from a design perspective, although the thermal resistance of the glass plate results in some losses.
The temperature rise also induces thermal stresses due the materials’ different coefficients of thermal expansion. As a result, mechanical stresses and deformations arise in the layer and in the glass plate. Figure 8 and Figure 9 shows the effective stress distribution in the device and the resulting deformations. During operation, the glass plate bends toward the air side.
Figure 8: The thermally induced von Mises stress plotted with the deformation in glass plate.
The highest effective stress, approximately 17.5 MPa, occurs at the inner corners of the curves of the Nichrome circuit. The highest effective stress, approximately 380 MPa, occurs in the conducting layer.
Stresses in the interface between the resistive layer and the glass plate must also be considered. Assume that the yield stress of the surface adhesion in the interface is in the region of 50 MPa a value significantly lower than the yield stresses of the other materials in the device. If the effective stress increases above this value, the resistive layer locally detaches from the glass. Once it has detached, heat transfer is locally impeded, which can lead to overheating of the resistive layer and eventually cause the device to fail.
Figure 9: The thermally induced von Mises stress plotted with the deformation in resistive layer.
Figure 10 displays the interface stress acting on the adhesive layer during heater operation. As the figure shows, the device experiences a maximum interfacial stress that is approximately five times smaller than the yield stress. This means that the device is safe in terms of the adhesive stress.
Finally, the warping of the device, that is, its deviation from a plane surface as shown in Figure 11 are studied. The maximum deviation from being a planar surface, is approximately 48 μm. For high-precision applications, such as semiconductor processing, this might be a significant value that limits the device’s operating temperature.
Figure 10: The stress in the interface between the resistive layer and the glass plate.
Figure 11: Deviation from a plane surface on the fluid side of the glass plate.
Notes About the COMSOL Implementation
•
Modeling a composite laminate as a layered shell requires a surface geometry, in general referred to as a base surface, and a Layered Material node which adds an extra dimension (1D) to the base surface geometry in the surface normal direction. You can use the Layered Material functionality to model several layers stacked on top of each other having different thicknesses, material properties, and fiber orientations. You can optionally specify the interface materials between the layers, and control the number of through-thickness mesh elements for each layer.
•
The third direction for the selected coordinate system in the Single Layer Material, Layered Material Link, or Layered Material Stack represents the normal direction of the Layered Shell or Shell physics. This is also the direction in which the layer stacking is interpreted from bottom to top, and therefore, it is crucial to know it during modeling. There are two ways to achieve this:
-
Using physics symbols: Go to the physics settings, find the Physics Symbols section, and select the Enable physics symbols checkbox. Then go to the material feature, for instance, Linear Elastic Material, to see the normal direction represented by green arrows in the geometry.
-
Using result templates: When a solution dataset is available, use the result template Thickness and Orientation to plot the normal direction.
•
The Thermal Stress, Layered Shell multiphysics interface includes the Heat Transfer in Shell and the Layered Shell interfaces. In the silica glass, these two interfaces solve for temperature and displacements, respectively. In the conducting layer representing the circuit, the temperature, electric potential, and displacement are solved by Heat Transfer in Shell, Electric Currents in Layered Shells, and the Layered Shell interfaces.
Application Library path: Composite_Materials_Module/Multiphysics/heating_circuit_layered
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, Layered Shell.
3
Click Add.
4
In the Select Physics tree, select AC/DC > Electric Fields and Currents > Electric Currents in Layered Shells (ecis).
5
Click Add.
6
Click  Study.
7
In the Select Study tree, select General Studies > Stationary.
8
Click  Done.
Global Definitions
Parameters 1
Load the parameters from a file.
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file heating_circuit_layered_parameters.txt.
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 mm.
Work Plane 1 (wp1)
1
In the Geometry toolbar, click  Work Plane.
2
In the Settings window for Work Plane, click  Go to Plane Geometry.
Work Plane 1 (wp1) > Plane Geometry
In the Model Builder window, click Plane Geometry.
Work Plane 1 (wp1) > Square 1 (sq1)
1
In the Work Plane toolbar, click  Square.
2
In the Settings window for Square, locate the Size section.
3
In the Side length text field, type 10.
4
Locate the Position section. In the xw text field, type 7.
5
In the yw text field, type 10.
6
Click  Build Selected.
Work Plane 1 (wp1) > Square 2 (sq2)
1
Right-click Component 1 (comp1) > Geometry 1 > Work Plane 1 (wp1) > Plane Geometry > Square 1 (sq1) and choose Duplicate.
2
In the Settings window for Square, locate the Position section.
3
In the xw text field, type 30.
4
In the yw text field, type 8.
5
Click  Build Selected.
Work Plane 1 (wp1) > Polygon 1 (pol1)
1
In the Work Plane toolbar, click  Polygon.
2
In the Settings window for Polygon, locate the Coordinates section.
3
From the Data source list, choose File.
4
Click  Browse.
5
Browse to the model’s Application Libraries folder and double-click the file heating_circuit_layered_polygon.txt.
6
Click  Build Selected.
Work Plane 1 (wp1) > Fillet 1 (fil1)
1
In the Work Plane toolbar, click  Fillet.
2
On the object pol1, select Points 2–8, 23–29, 34, 36, 37, 41, and 42 only.
It might be easier to select the points by using the Selection List window. To open this window, navigate to the Home toolbar, click Windows, and choose Selection List. (If you are running the cross-platform desktop, you find Windows in the main menu.)
3
In the Settings window for Fillet, locate the Radius section.
4
In the Radius text field, type 10.
5
Click  Build Selected.
Work Plane 1 (wp1) > Fillet 2 (fil2)
1
In the Work Plane toolbar, click  Fillet.
2
On the object fil1, select Points 6–12, 26–31, 37, 40, 43, 46, 49, and 50 only.
3
In the Settings window for Fillet, locate the Radius section.
4
In the Radius text field, type 5.
5
Click  Build Selected.
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 80.
4
In the Height text field, type 130.
Form Union (fin)
In the Home toolbar, click  Build All.
Before creating layered material stacks, add the materials for individual layers.
Add Material
1
In the Materials toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Built-in > Silica glass.
4
Right-click and choose Add to Global Materials.
5
In the Materials toolbar, click  Add Material to close the Add Material window.
Global Definitions
Silica Glass
In the Settings window for Material, type Silica Glass in the Label text field.
Silver Layer
1
In the Model Builder window, right-click Materials and choose Blank Material.
2
Right-click Material 2 (mat2) and choose Rename.
3
In the Rename Material dialog, type Silver Layer in the New label text field.
4
Click OK.
Nichrome Layer
1
In the Model Builder window, right-click Materials and choose Blank Material.
2
Right-click Material 3 (mat3) and choose Rename.
3
In the Rename Material dialog, type Nichrome Layer in the New label text field.
4
Click OK.
The stacking of the Silver and Nichrome layers is not the same across the glass plate. In order to model the stacking, add a Layered Material Stack node with Layered Material subnodes having different selections.
Materials
Layered Material Stack 1 (stlmat1)
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Layers > Layered Material Stack.
Layered Material Link 1 (stlmat1.stllmat1)
In the Model Builder window, under Component 1 (comp1) > Materials > Layered Material Stack 1 (stlmat1) right-click Layered Material Link 1 (stlmat1.stllmat1) and choose Delete.
Layered Material Stack 1 (stlmat1)
1
In the Settings window for Layered Material Stack, locate the Orientation and Position section.
2
From the Position list, choose Bottom side on boundary.
Glass
1
Right-click Layered Material Stack 1 (stlmat1) and choose Layered Material.
2
In the Settings window for Layered Material, type Glass in the Label text field.
3
Locate the Layer Definition section. In the table, enter the following settings:
Layer
Material
Rotation
Value (m)
Thickness
Mesh elements
Layer 1
Silica Glass (mat1)
0.0
0 rad
d_glass
3
Silver
1
Right-click Layered Material Stack 1 (stlmat1) and choose Layered Material.
2
In the Settings window for Layered Material, type Silver in the Label text field.
3
Locate the Boundary Selection section. Click  Clear Selection.
4
Click  Paste Selection.
5
In the Paste Selection dialog, type 2 4 in the Selection text field.
6
Click OK.
7
In the Settings window for Layered Material, locate the Layer Definition section.
8
In the table, enter the following settings:
Layer
Material
Rotation
Value (m)
Thickness
Mesh elements
Layer 1
Silver Layer (mat2)
0.0
0 rad
d_layer
1
Nichrome
1
Right-click Layered Material Stack 1 (stlmat1) and choose Layered Material.
2
In the Settings window for Layered Material, type Nichrome in the Label text field.
3
Locate the Boundary Selection section. Click  Clear Selection.
4
Click  Paste Selection.
5
In the Paste Selection dialog, type 3 in the Selection text field.
6
Click OK.
7
In the Settings window for Layered Material, locate the Layer Definition section.
8
In the table, enter the following settings:
Layer
Material
Rotation
Value (m)
Thickness
Mesh elements
Layer 1
Nichrome Layer (mat3)
0.0
0 rad
d_layer
1
To visualize the stacking, create a Layer Cross Section Preview plot through an action button in the Layered Material Settings section.
Layered Material Stack 1 (stlmat1)
1
In the Model Builder window, click Layered Material Stack 1 (stlmat1).
2
In the Settings window for Layered Material Stack, click Layer Cross-Section Preview in the upper-right corner of the Layered Material Settings section. From the menu, choose Create Layer Cross-Section Plot.
Results
Layer Cross-Section Preview
1
In the Model Builder window, expand the Results node, then click Layer Cross-Section Preview.
2
In the Layer Cross-Section Preview toolbar, click  Plot.
Before adding the material properties, it is a good idea to first set up the physics, so that COMSOL Multiphysics can detect which material properties are needed.
Layered Shell (lshell)
Linear Elastic Material 1
1
In the Model Builder window, under Component 1 (comp1) > Layered Shell (lshell) click Linear Elastic Material 1.
2
In the Settings window for Linear Elastic Material, locate the Linear Elastic Material section.
3
From the Material symmetry list, choose Isotropic.
Rigid Motion Suppression 1
In the Physics toolbar, click  Boundaries and choose Rigid Motion Suppression.
Continuity 1
1
In the Physics toolbar, click  Edges and choose Continuity.
2
In the Settings window for Continuity, locate the Layer Selection section.
3
From the Source list, choose Layered Material Stack 1 (stlmat1.zone1).
4
From the Destination list, choose Layered Material Stack 1 (stlmat1.zone2).
Continuity 2
1
In the Physics toolbar, click  Edges and choose Continuity.
2
In the Settings window for Continuity, locate the Layer Selection section.
3
From the Source list, choose Layered Material Stack 1 (stlmat1.zone1).
4
From the Destination list, choose Layered Material Stack 1 (stlmat1.zone3).
Continuity 3
1
In the Physics toolbar, click  Edges and choose Continuity.
2
In the Settings window for Continuity, locate the Layer Selection section.
3
From the Source list, choose Layered Material Stack 1 (stlmat1.zone2).
4
From the Destination list, choose Layered Material Stack 1 (stlmat1.zone3).
5
In the Selection table, enter the following settings:
 
Layered material
Offset (m)
√
Layered Material 3
0
The absolute displacement of the glass plate is not important in itself, since it is just a function of how the rigid body constraints are applied. Instead, you want to see how much the boundary deviates from being planar.
Warpage 1
1
In the Physics toolbar, click  Boundaries and choose Warpage.
2
In the Settings window for Warpage, locate the Boundary Selection section.
3
From the Selection list, choose All boundaries.
4
Locate the Interface Selection section. From the Apply to list, choose Bottom interface.
5
Locate the Warpage section. From the Reference plane list, choose From points.
6
Locate the Reference Plane, Point 1 section. Click to select the  Activate Selection toggle button.
7
Select Point 1 only.
8
Locate the Reference Plane, Point 2 section. Click to select the  Activate Selection toggle button.
9
Select Point 2 only.
10
Locate the Reference Plane, Point 3 section. Click to select the  Activate Selection toggle button.
11
Select Point 61 only.
Heat Transfer in Shells (htlsh)
Solid 1
1
In the Model Builder window, under Component 1 (comp1) > Heat Transfer in Shells (htlsh) click Solid 1.
2
In the Settings window for Solid, locate the Layer Model section.
3
Clear the Layerwise constant properties checkbox.
Heat Flux, Interface 1
1
In the Physics toolbar, click  Boundaries and choose Heat Flux, Interface.
2
In the Settings window for Heat Flux, Interface, locate the Boundary Selection section.
3
From the Selection list, choose All boundaries.
4
Locate the Interface Selection section. From the Apply to list, choose Top interface.
5
Locate the Heat Flux section. From the Flux type list, choose Convective heat flux.
6
In the h text field, type h_air.
7
In the Text text field, type T_air.
Heat Flux, Interface 2
1
In the Physics toolbar, click  Boundaries and choose Heat Flux, Interface.
2
In the Settings window for Heat Flux, Interface, locate the Boundary Selection section.
3
From the Selection list, choose All boundaries.
4
Locate the Interface Selection section. From the Apply to list, choose Bottom interface.
5
Locate the Heat Flux section. From the Flux type list, choose Convective heat flux.
6
In the h text field, type h_fluid.
7
In the Text text field, type T_fluid.
Continuity 1
1
In the Physics toolbar, click  Edges and choose Continuity.
2
In the Settings window for Continuity, locate the Layer Selection section.
3
From the Source list, choose Layered Material Stack 1 (stlmat1.zone1).
4
From the Destination list, choose Layered Material Stack 1 (stlmat1.zone2).
Continuity 2
1
In the Physics toolbar, click  Edges and choose Continuity.
2
In the Settings window for Continuity, locate the Layer Selection section.
3
From the Source list, choose Layered Material Stack 1 (stlmat1.zone1).
4
From the Destination list, choose Layered Material Stack 1 (stlmat1.zone3).
Continuity 3
1
In the Physics toolbar, click  Edges and choose Continuity.
2
In the Settings window for Continuity, locate the Layer Selection section.
3
From the Source list, choose Layered Material Stack 1 (stlmat1.zone2).
4
From the Destination list, choose Layered Material Stack 1 (stlmat1.zone3).
5
In the Selection table, enter the following settings:
 
Layered material
Offset (m)
√
Layered Material 3
0
Electric Currents in Layered Shells (ecis)
1
In the Model Builder window, under Component 1 (comp1) click Electric Currents in Layered Shells (ecis).
2
In the Settings window for Electric Currents in Layered Shells, locate the Boundary Selection section.
3
In the list box, select 1 (stlmat1).
4
Click  Remove from Selection.
5
Select Boundaries 2–4 only.
6
Locate the Shell Properties section. Clear the Use all layers checkbox.
7
In the Selection table, clear the checkbox for Layer 1 - Glass.
Ground 1
1
In the Physics toolbar, click  Edges and choose Ground.
2
Select Edge 38 only.
3
In the Settings window for Ground, locate the Shell Properties section.
4
From the Layered material list, choose Layered Material Stack 1 (stlmat1.zone2).
Electric Potential 1
1
In the Physics toolbar, click  Edges and choose Electric Potential.
2
Select Edge 5 only.
3
In the Settings window for Electric Potential, locate the Shell Properties section.
4
From the Layered material list, choose Layered Material Stack 1 (stlmat1.zone2).
5
Locate the Electric Potential section. In the V0 text field, type V_in.
Electric Continuity 1
1
In the Physics toolbar, click  Edges and choose Electric Continuity.
2
In the Settings window for Electric Continuity, locate the Layer Selection section.
3
From the Source list, choose Layered Material Stack 1 (stlmat1.zone2).
4
From the Destination list, choose Layered Material Stack 1 (stlmat1.zone3).
5
In the Selection table, enter the following settings:
 
Layered material
Offset (m)
√
Layered Material 3
0
Multiphysics
Electromagnetic Heating, Layered Shell 1 (ehls1)
In the Physics toolbar, click  Multiphysics Couplings and choose Boundary > Electromagnetic Heating, Layered Shell.
Global Definitions
Silver Layer (mat2)
1
In the Model Builder window, under Global Definitions > Materials click Silver Layer (mat2).
2
In the Settings window for Material, locate the Material Contents section.
3
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
83e9
Pa
Young’s modulus and Poisson’s ratio
Poisson’s ratio
nu
0.37
1
Young’s modulus and Poisson’s ratio
Density
rho
10500
kg/m³
Basic
Thermal conductivity
k_iso ; kii = k_iso, kij = 0
420
W/(m·K)
Basic
Heat capacity at constant pressure
Cp
230
J/(kg·K)
Basic
Electric conductivity
sigma_iso ; sigmaii = sigma_iso, sigmaij = 0
sigma_silver
S/m
Basic
Relative permittivity
epsilonr_iso ; epsilonrii = epsilonr_iso, epsilonrij = 0
1
1
Basic
Coefficient of thermal expansion
alpha_iso ; alphaii = alpha_iso, alphaij = 0
18.9e-6
1/K
Basic
Nichrome Layer (mat3)
1
In the Model Builder window, click Nichrome Layer (mat3).
2
In the Settings window for Material, locate the Material Contents section.
3
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Young’s modulus
E
213e9
Pa
Young’s modulus and Poisson’s ratio
Poisson’s ratio
nu
0.33
1
Young’s modulus and Poisson’s ratio
Density
rho
9000
kg/m³
Basic
Thermal conductivity
k_iso ; kii = k_iso, kij = 0
15
W/(m·K)
Basic
Heat capacity at constant pressure
Cp
20
J/(kg·K)
Basic
Electric conductivity
sigma_iso ; sigmaii = sigma_iso, sigmaij = 0
sigma_nichrome
S/m
Basic
Relative permittivity
epsilonr_iso ; epsilonrii = epsilonr_iso, epsilonrij = 0
1
1
Basic
Coefficient of thermal expansion
alpha_iso ; alphaii = alpha_iso, alphaij = 0
10e-6
1/K
Basic
Mesh 1
Free Triangular 1
1
In the Mesh toolbar, click  More Generators and choose Free Triangular.
2
In the Settings window for Free Triangular, locate the Boundary Selection section.
3
From the Selection list, choose All boundaries.
Size 1
1
Right-click Free Triangular 1 and choose Size.
2
In the Settings window for Size, locate the Geometric Entity Selection section.
3
In the list box, select 1.
4
Click  Remove from Selection.
5
Select Boundaries 2–4 only.
6
Locate the Element Size section. Click the Custom button.
7
Locate the Element Size Parameters section.
8
Select the Maximum element size checkbox. In the associated text field, type 2.
9
Click  Build All.
Study 1
Switch off the generation of default plots in the study. We will use Result Templates.
1
In the Model Builder window, click Study 1.
2
In the Settings window for Study, locate the Study Settings section.
3
Clear the Generate default plots checkbox.
4
In the Study toolbar, click  Compute.
Set default units for result presentation.
Results
Preferred Units 1
1
In the Results toolbar, click  Configurations and choose Preferred Units.
2
In the Settings window for Preferred Units, locate the Units section.
3
Click  Add Physical Quantity.
4
In the Physical Quantity dialog, select General > Displacement (m) in the tree.
5
Click OK.
6
In the Settings window for Preferred Units, locate the Units section.
7
In the table, enter the following settings:
Quantity
Unit
Preferred unit
Displacement
m
µm
8
Click  Add Physical Quantity.
9
In the Physical Quantity dialog, select Solid Mechanics > Stress tensor (N/m^2) in the tree.
10
Click OK.
11
In the Settings window for Preferred Units, locate the Units section.
12
In the table, enter the following settings:
Quantity
Unit
Preferred unit
Stress tensor
N/m^2
MPa
13
Select the Apply conversions to expressions with the same dimensions checkbox.
14
Click  Apply.
Result Templates
1
In the Home toolbar, click  Windows and choose Result Templates.
2
Go to the Result Templates window.
3
In the tree, select Study 1/Solution 1 (sol1) > Layered Shell > von Mises Stress (lshell).
4
Click the Add Result Template button in the window toolbar.
5
In the tree, select Study 1/Solution 1 (sol1) > Layered Shell > Stress, Slice (lshell).
6
Click the Add Result Template button in the window toolbar.
Results
Stress, Assembly (lshell)
1
In the Settings window for 3D Plot Group, type Stress, Assembly (lshell) in the Label text field.
2
In the Stress, Assembly (lshell) toolbar, click  Plot.
Stress, Glass (lshell)
1
In the Model Builder window, under Results click Stress, Slice (lshell).
2
In the Settings window for 3D Plot Group, type Stress, Glass (lshell) in the Label text field.
3
Click to expand the Title section. From the Title type list, choose Manual.
4
In the Title text area, type Layered Material Slice: von Mises stress (MPa), Glass.
Layered Material Slice 1
1
In the Model Builder window, expand the Stress, Glass (lshell) node, then click Layered Material Slice 1.
2
In the Settings window for Layered Material Slice, locate the Expression section.
3
In the Expression text field, type lshell.misesGp.
4
Locate the Through-Thickness Location section. From the Location definition list, choose Physical.
5
In the Local z-coordinate text field, type 0 d_glass.
6
In the Stress, Glass (lshell) toolbar, click  Plot.
Stress, Conducting Layer (lshell)
1
In the Model Builder window, right-click Stress, Glass (lshell) and choose Duplicate.
2
In the Model Builder window, click Stress, Glass (lshell) 1.
3
In the Settings window for 3D Plot Group, type Stress, Conducting Layer (lshell) in the Label text field.
4
Locate the Title section. In the Title text area, type Layered Material Slice: von Mises stress (MPa), Conducting Layer.
Layered Material Slice 1
1
In the Model Builder window, click Layered Material Slice 1.
2
In the Settings window for Layered Material Slice, locate the Through-Thickness Location section.
3
In the Local z-coordinate text field, type d_glass+d_layer.
4
In the Stress, Conducting Layer (lshell) toolbar, click  Plot.
Result Templates
1
Go to the Result Templates window.
2
In the tree, select Study 1/Solution 1 (sol1) > Heat Transfer in Shells > Temperature, Shell (htlsh).
3
Click the Add Result Template button in the window toolbar.
4
In the tree, select Study 1/Solution 1 (sol1) > Electric Currents in Layered Shells > Electric Potential (ecis).
5
Click the Add Result Template button in the window toolbar.
6
In the Home toolbar, click  Windows and choose Result Templates.
Results
Temperature, Shell (htlsh)
1
In the Model Builder window, under Results click Temperature, Shell (htlsh).
2
In the Temperature, Shell (htlsh) toolbar, click  Plot.
Surface 1
1
In the Model Builder window, expand the Electric Potential (ecis) node, then click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type ecis.Vc.
4
In the Electric Potential (ecis) toolbar, click  Plot.
Result Templates
1
Go to the Result Templates window.
2
In the tree, select Study 1/Solution 1 (sol1) > Layered Shell > Geometry and Layup (lshell) > Shell Geometry (lshell).
3
Click the Add Result Template button in the window toolbar.
4
In the Results toolbar, click  Result Templates to close the Result Templates window.
Results
Stack Zones
1
In the Model Builder window, right-click Shell Geometry (lshell) and choose Duplicate.
2
Drag and drop Shell Geometry (lshell) 1 below Layer Cross-Section Preview.
3
In the Settings window for 3D Plot Group, type Stack Zones in the Label text field.
Surface 1
1
In the Model Builder window, expand the Stack Zones node, then click Surface 1.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Layered materials > Layered Material Stack 1 (stlmat1) > stlmat1.zone - Zone index - 1.
3
Locate the Coloring and Style section. From the Coloring list, choose Color table.
4
From the Color table list, choose TrafficLight.
5
In the Stack Zones toolbar, click  Plot.
Surface Losses
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Surface Losses in the Label text field.
Surface 1
1
In the Surface Losses toolbar, click  Surface.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Electric Currents in Layered Shells > Heating and losses > ecis.Qsh - Surface loss density, electromagnetic - W/m².
3
In the Surface Losses toolbar, click  Plot.
Take the following steps to generate a plot of the norm of the surface traction vector in the surface plane.
Interface Stress
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Interface Stress in the Label text field.
3
Locate the Title section. From the Title type list, choose Manual.
4
In the Title text area, type Layered Material Slice: Interface Stress (MPa).
Layered Material Slice 1
1
In the Interface Stress toolbar, click  More Plots and choose Layered Material Slice.
2
In the Settings window for Layered Material Slice, locate the Expression section.
3
In the Expression text field, type sqrt(lshell.sxz^2+lshell.syz^2).
4
Locate the Through-Thickness Location section. From the Location definition list, choose Physical.
5
In the Local z-coordinate text field, type d_glass.
Selection 1
1
Right-click Layered Material Slice 1 and choose Selection.
2
Select Boundaries 2–4 only.
3
In the Interface Stress toolbar, click  Plot.
Next, plot the glass plate’s deviation from being plane.
Result Templates
1
In the Results toolbar, click  Result Templates to open the Result Templates window.
2
Go to the Result Templates window.
3
In the tree, select Study 1/Solution 1 (sol1) > Layered Shell > Warpage (wrp1).
4
Click the Add Result Template button in the window toolbar.
5
In the Results toolbar, click  Result Templates to close the Result Templates window.
Results
Warpage (wrp1)
In the Warpage (wrp1) toolbar, click  Plot.
To calculate the values for the total generated heat and the integrated heat flux on the fluid side, perform a boundary integration. Before creating evaluation group, add a Layered Material dataset with evaluation set on interfaces.
Layered Material 1a
1
In the Model Builder window, expand the Results > Datasets node.
2
Right-click Layered Material and choose Duplicate.
3
In the Settings window for Layered Material, locate the Layers section.
4
From the Evaluate in list, choose Interfaces.
Total Heat Generated
1
In the Results toolbar, click  Evaluation Group.
2
In the Settings window for Evaluation Group, type Total Heat Generated in the Label text field.
3
Locate the Data section. From the Dataset list, choose Layered Material 1a.
Surface Integration 1
1
Right-click Total Heat Generated and choose Integration > Surface Integration.
2
Select Boundaries 2–4 only.
3
In the Settings window for Surface Integration, locate the Through-Thickness Location section.
4
From the Location input list, choose Manual.
5
From the Location definition list, choose Physical.
6
Click Replace Expression in the upper-right corner of the Expressions section. From the menu, choose Component 1 (comp1) > Electric Currents in Layered Shells > Heating and losses > ecis.Qsh - Surface loss density, electromagnetic - W/m².
7
In the Total Heat Generated toolbar, click  Evaluate.
The result should be close to 13.8 W.
Total Heat Transferred to Fluid
1
In the Results toolbar, click  Evaluation Group.
2
In the Settings window for Evaluation Group, type Total Heat Transferred to Fluid in the Label text field.
3
Locate the Data section. From the Dataset list, choose Layered Material 1a.
Surface Integration 1
1
Right-click Total Heat Transferred to Fluid and choose Integration > Surface Integration.
2
In the Settings window for Surface Integration, locate the Selection section.
3
From the Selection list, choose All boundaries.
4
Click Replace Expression in the upper-right corner of the Expressions section. From the menu, choose Component 1 (comp1) > Heat Transfer in Shells > Boundary fluxes > htlsh.hfi2.q0 - Boundary convective heat flux - W/m².
5
In the Total Heat Transferred to Fluid toolbar, click  Evaluate.
The result should be close to 8.5 W.