Tutorial 19 - Thermal Stress - Switch

Tutorial Number 19: Thermalstress analysis of a bimetallic
switch
Stefano Morlacchi
September 2014
Simuleon B.V.
Sint Antoniestraat 7 5314 LG Bruchem
T. +31(0)418-644699 F. +31(0)418-644690 E. info@simuleon.nl W. www.simuleon.nl
1.
Introduction
In this tutorial, you will create a coupled thermal-stress simulation of a

bimetallic thermostat. This safety tool is used to open an electric circuit when the
electric current increases too much. As a result of the high current, the strip
increases its temperature and bends because of the different thermal expansion
coefficients of the two metals that compose the strip. In this way, the electric
circuit is opened and the current becomes zero.
After creating the coupled thermo-mechanical simulation where temperature field
and displacement are solved together, you will use the sequential approach
(heat transfer analysis + mechanical analysis) to study the same process and
compare the results obtained with the two methods.
When you complete this tutorial, you will be able to:

-
Define the thermo-mechanical properties of materials.
Define thermal loads and boundary conditions used for a coupled thermomechanical analysis.
Import heat transfer analysis results as loading conditions for a pure

mechanical analysis (sequential approach).
Preliminaries
- The model is based on the SI units based on millimetres.
Figure 1: Consistent sets of units available in Abaqus.
- The coupled simulation is created as tutorial and you will be thoroughly guided
to create the model. The sequential approach is proposed as a workshop and
only the main guidelines will be provided.
Simuleon B.V.

2.
Setting up the model
Open the Abaqus database file Tutorial 19.cae

This file contains the geometry of the two parts, the bimetallic strip and the
contact pin, and the correctly positioned assembly. Geometry is in mm so
material properties and loading conditions have to be defined accordingly.
3.
Material and section properties
Enter the property module and define the two material models for the steel and
porcelain. Within a temperature-stress analysis, both mechanical and thermal
material properties have to be defined.
COMMON SI UNITS FOR THERMAL PROPERTIES

- Density
- Conductivity
- Specific Heat
- Thermal expansion coefficient
1. Go into the Property Module and click the Create Material icon. In the Edit
Material dialog box, name the material Steel. From the material editors menu
bar, select Thermal Conductivity. Enter a value of 0.015 W/mm/C. From the
material editors menu bar, select Thermal Specific Heat. Enter a value of
420,000 J/tonn/C. Select Mechanical Elasticity Elastic, enter a Young
Modulus value of 210,000 MPa and a Poisson coefficient equal to 0.35. Select
Mechanical Expansion and enter a value of 1.1E-5 1/C. Select General
Density and enter a value of 8E-9 tonn/mm3. Click OK to exit the material editor.
Simuleon B.V.

2. Go into the Property Module and click the Create Material icon. In the Edit
Material dialog box, name the material Aluminium. From the material editors
menu bar, select Thermal Conductivity. Enter a value of 0.15 W/mm/C.
From the material editors menu bar, select Thermal Specific Heat. Enter a
value of 670,000 J/tonn/C. Select Mechanical Elasticity Elastic, enter a
Young Modulus value of 70,000 MPa and a Poisson coefficient equal to 0.3.
Select Mechanical Expansion and enter a value of 2.3E-5 1/C. Select
General Density and enter a value of 3E-9 tonn/mm3. Click OK to exit the
material editor.
3. Create two solid homogeneous sections referring to Aluminium and Steel.

Assign now the steel section to the Pin and the geometry set of the bimetallic
strip part called Set-STEEL. Assign the Aluminium section to the geometric set of
the bimetallic strip called Set-ALLY.
Simuleon B.V.

4.
Assembly and Step
1. Enter the assembly module and look at the instances already pre-assembled.
Notice the initial interference between the pin and the bimetallic strip.
Figure 2: Bimetallic thermostat assembly. Colours refer to different material properties,

white for steel and blue for ally
2. Enter the step module and create a static general step called StepInterference with duration of 1s. Turn on the nlgeom parameter and enter 0.01
as initial increment size. This step will be used to solve the interference between
the two instances of the model.
Create now two coupled thermal-displacement steps called Step-Heating and
Step-Cooling with duration of 1 s and 10 s, respectively. Select transient
response, enter 0.01 as initial increment size and 5 as maximum allowable
temperature change per increment. In the step-Heating, a body heat flux
condition will be applied to the strip to increase its temperature while in the last
step, strip temperature will decrease due to a surface film condition applied to the
external surfaces. Environmental temperature is set at 20 C.
3. In the Field Output requested by default, make sure that the NT (nodal
temperature) and HFL (heat flux) variables have been selected for all the steps.
4. Create a new History Output request, choosing the set Pin-1.CP as region
and CSTRESS as output variable.
Simuleon B.V.

5.
Mesh
Enter the mesh module and discretize both parts. Select 1.5 as global element
size for the bimetallic strip and hex element shape. Select 1 as global size for the
Pin part. Mesh the parts and make sure that the element type selected is a linear
reduced integration temperature-displacement element (C3D8RT) for both the
parts.
6.
Interactions
Enter the Interaction module and create a mechanical interaction between the
PIN and the STRIP and a surface film condition to model the cooling down of the
strip due to convection.
1. Mechanical interaction. Create a new surface to surface interaction at StepInterference, called Int-FIT, selecting the Pins Surf-INT as master surface and
the Strips surface Surf-INT as slave surface. Click on the Create an Interaction
Property icon at the bottom of the Edit Interaction dialog box as shown in the
following picture. Call the interaction property as Mechanical and select Contact
as Type
in the dialog box. Enter 0.2 as friction coefficient in the Tangential
behaviour option and Hard contact as Normal behaviour. Click ok and select the
Mechanical interaction property in the Edit interaction dialog box. Click on
interference fit options and select Gradually remove slave node overclosure
during the step.
2. Thermal interaction. Create a film condition interaction to model the heat lost
from the strip due to convection with the external air. Create a new interaction
called Int-Convection in Step-Cooling, select Surface Film condition as Type. In
the Edit Interaction dialog box, select all the external surfaces as Region,
Embedded coefficient as definition type, enter 0.0028 as typical film coefficient
with air, enter 20 as sink temperature and Instantaneous as amplitude. Click OK.
Simuleon B.V.

Simuleon B.V.

7.
Boundary and Loading conditions
1. Create an Encastre boundary condition.

In the initial step, create an encastre boundary condition using the surface SurfENC created at the assembly level which comprehends both a region of the Pin
and a region of the strip as shown in the following picture.
Figure 3: Encastre BCs.
2. Create the Body Heat Flux loading condition.

Click on the Create Load Icon in the vertical toolbar. Rename the Load as BodyHeat, select Step-Heating as the Step, Thermal as category and Body Heat Flux
as type, click Continue. Select the whole bimetallic strip part as region and enter
0.2 in the magnitude field. Keep Instantaneous as amplitude. Enter the loads
manager, select the load Body-Heat in correspondence of the Step-Cooling and
click Edit. Enter 0 as magnitude and click OK.
3. Create the Initial Predefined Field.

Click on the Create Predefined Field Icon in the vertical toolbar. Select initial as
the Step, Other as category and Temperature as type, click Continue. Select the
Whole model as region. Enter 20 in the Temperature field and select Direct
specification as method.
8.
Job module
Enter the Job module and create a new Job called Coupled. Submit the job and
monitor the convergence.
Simuleon B.V.

9.
Workshop: Sequential analysis.
In the next workshop, you are invited to investigate the previous thermomechanical process using a sequential approach composed of a pure heat
transfer analysis followed by a pure mechanical analysis. Results of the heat
transfer simulation in terms of nodal temperatures are passed to the mechanical
analysis and used as loading conditions. The main (not all) steps that have to be
performed are summarized in the following paragraphs.
Heat transfer analysis.

- Copy the Model-Coupled to the Model-Sequential-HT so that most of the things
are already included.
- Only the bimetallic strip part should be included in the model.
- Only the last two steps are useful in this analysis.
- Replace the steps with heat transfer steps and the element type to DC3D8.
- Use the same step lengths of the coupled analysis. Mesh and step increments
can be changed and optimized for this kind of analysis.
Mechanical analysis.
- Copy the Model-Coupled to the Model-Sequential-Mech
- Replace the steps with static steps. Change the element type to C3D8R.
- Make sure the temperature variable NT is included in the field output requests.
- Include a new Predefined Field to import the results of the previous analysis in
terms of nodal temperatures. This has to be modified at every step...
Simuleon B.V.

10. Results Visualization

At the end of the simulations, enter the Visualization module by clicking results
in the Job manager.
- Animate the simulation to look at the mechanical deformations due to

temperature change and different expansion coefficient.
Figure 4: Von Mises contour plots. Undeformed configuration is superimposed.
- Compare the coupled and uncoupled simulations in terms of temperature

changes, contact pressures and computational cost.
Figure 5: Temperature contour plot at the end of the Step-Heating. Undeformed

configuration is superimposed.
Simuleon B.V.

10
Figure 6: Contact pressure calculated at the central node of the Pin (history output) with
the coupled and uncoupled approached. Similar results are obtained. Differences mainly
due to the different increments used.
Simuleon B.V.

11

Tutorial 19 - Thermal Stress - Switch

Uploaded by

Copyright:

Available Formats

Tutorial 19 - Thermal Stress - Switch

Uploaded by

Document Information

Original Description:

Copyright

Available Formats

Share this document

Share or Embed Document

Sharing Options

Did you find this document useful?

Is this content inappropriate?

Copyright:

Available Formats

Tutorial 19 - Thermal Stress - Switch

Uploaded by

Copyright:

Available Formats

How does a bimetallic thermostat work?

How does a bimetallic thermostat work?

What are the steps to create a coupled thermal-stress simulation?

What are the steps to create a coupled thermal-stress simulation?

Tutorial Number 19: Thermalstress analysis of a bimetallic

In this tutorial, you will create a coupled thermal-stress simulation of a

When you complete this tutorial, you will be able to:

Define the thermo-mechanical properties of materials.

Import heat transfer analysis results as loading conditions for a pure

Figure 1: Consistent sets of units available in Abaqus.

Sint Antoniestraat 7 5314 LG Bruchem

Setting up the model

Open the Abaqus database file Tutorial 19.cae

Material and section properties

COMMON SI UNITS FOR THERMAL PROPERTIES

- Thermal expansion coefficient

Sint Antoniestraat 7 5314 LG Bruchem

3. Create two solid homogeneous sections referring to Aluminium and Steel.

Sint Antoniestraat 7 5314 LG Bruchem

Assembly and Step

Figure 2: Bimetallic thermostat assembly. Colours refer to different material properties,

Sint Antoniestraat 7 5314 LG Bruchem

in the dialog box. Enter 0.2 as friction coefficient in the Tangential

Sint Antoniestraat 7 5314 LG Bruchem

Sint Antoniestraat 7 5314 LG Bruchem

Boundary and Loading conditions

1. Create an Encastre boundary condition.

Figure 3: Encastre BCs.

2. Create the Body Heat Flux loading condition.

3. Create the Initial Predefined Field.

Sint Antoniestraat 7 5314 LG Bruchem

Workshop: Sequential analysis.

Heat transfer analysis.

Sint Antoniestraat 7 5314 LG Bruchem

10. Results Visualization

- Animate the simulation to look at the mechanical deformations due to

Figure 4: Von Mises contour plots. Undeformed configuration is superimposed.

- Compare the coupled and uncoupled simulations in terms of temperature

Figure 5: Temperature contour plot at the end of the Step-Heating. Undeformed

Sint Antoniestraat 7 5314 LG Bruchem

Sint Antoniestraat 7 5314 LG Bruchem

You might also like