PDF
Bracket — Thermal-Stress Analysis
Introduction
The various examples based on a bracket geometry form a suite of tutorials which summarizes the fundamentals when modeling structural mechanics problems in COMSOL Multiphysics and the Structural Mechanics Module.
In this example you learn how to perform a thermal-stress analysis.
Model Definition
The model used in this guide is an assembly of a bracket and its mounting bolts, which are all made of steel. The geometry is shown in Figure 1.
In this example, a temperature distribution is computed in the bracket and the resulting thermal stresses are determined. A heat flux of 10000 W/m2 is applied on the lower side of the bolted plates. On all other boundaries, a convection boundary condition is used. The heat transfer coefficient is 10 W/m2·K and room temperature (293.15 K) is used as external temperature.
Results
Figure 1 shows the temperature distribution in the bracket as well as arrows indicating the prescribed influx of heat. The temperature is highest where the inward heat flux is prescribed, and decreases as heat is removed by convection from all other boundaries.
Figure 1: Temperature distribution in the bracket. The prescribed heat flux is indicated by arrows.
Figure 2 shows the von Mises stress distribution in the bracket. You can see how the bracket is deformed by the thermal expansion. Due to the boundary conditions and the nonuniform temperature distribution, thermal stresses develop in the structure.
Figure 2: Von Mises stress distribution in the bracket.
Notes About the COMSOL Implementation
COMSOL Multiphysics contains physics interfaces for structural analysis as well as thermal analysis. You can set up the coupled analysis for thermal–structure interaction using three different methods:
•
Add a Thermal Stress, Solid interface as in this example. The coupling is predefined and appears in the Thermal Expansion nodes under Multiphysics. This is the easiest approach.
•
Add separate Solid Mechanics and Heat Transfer in Solids interfaces. Then add a Thermal Expansion node under Multiphysics, and check the settings in them.
•
Add separate Solid Mechanics and Heat Transfer in Solids interfaces. Add a Thermal Expansion subnode under Linear Elastic Material, and do the appropriate settings there.
In general, the resulting system of equations in a multiphysics problem can be solved using two different strategies:
•
In the fully coupled approach, all degrees of freedom (DOF) are solved simultaneously using a single large system of equations.
•
In the segregated approach, one smaller system of equations is solved for each type of physics. The couplings between the types of DOF are introduced through the load vectors. Except for some special cases, it is then necessary to repeat the solutions several times, until convergence.
In most cases, the segregated approach will be the default suggestion when the solver sequence is generated for a multiphysics problem. Based on your knowledge of the underlying properties of a problem, it is often possible to reduce the solution time by making appropriate changes to the solver settings. In this example, there are two important properties that can be used:
•
Both the heat transfer problem and the solid mechanics problem are linear.
•
The heat transfer problem is independent of the solution to the solid mechanics problem. This is a very common situation in thermal-stress analysis.
As long as the heat transfer problems is solved first, it is thus sufficient to make one pass through the segregated solver, and no iterations are needed for either physics interface.
Application Library path: Structural_Mechanics_Module/Tutorials/bracket_thermal
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.
The Thermal Stress, Solid interface is a multiphysics interface that combines a Solid Mechanics interface with a Heat Transfer in Solids interface. You can see the coupling between the physics interfaces under the Multiphysics node.
4
Click  Study.
5
In the Select Study tree, select General Studies > Stationary.
6
Click  Done.
Geometry 1
Import 1 (imp1)
1
In the Geometry toolbar, click  Import.
2
In the Settings window for Import, locate the Source section.
3
From the Source list, choose COMSOL Multiphysics file.
4
Click  Browse.
5
Browse to the model’s Application Libraries folder and double-click the file bracket.mphbin.
6
Click  Import.
7
Click the  Zoom Extents button in the Graphics toolbar.
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.
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 > Structural steel.
4
Click the Add to Component button in the window toolbar.
5
In the Materials toolbar, click  Add Material to close the Add Material window.
Solid Mechanics (solid)
Now specify the boundary conditions for the Solid Mechanics interface.
Roller 1
1
In the Physics toolbar, click  Boundaries and choose Roller.
2
Select Boundaries 17 and 27 only.
Spring Foundation 1
1
In the Physics toolbar, click  Boundaries and choose Spring Foundation.
2
Select Boundaries 18–21 and 31–34 only.
3
In the Settings window for Spring Foundation, locate the Spring section.
4
From the Spring type list, choose Total spring constant.
5
From the list, choose Diagonal.
6
Specify the ktot matrix as
600[kN/mm]
0
0
0
600[kN/mm]
0
0
0
0
Heat Transfer in Solids (ht)
Heat Flux 1
1
In the Physics toolbar, click  Boundaries and choose Heat Flux.
2
From the Selection list, choose All boundaries. Then remove boundaries 17 and 27.
3
In the Settings window for Heat Flux, locate the Heat Flux section.
4
From the Flux type list, choose Convective heat flux.
5
In the h text field, type 10.
Heat Flux 2
1
In the Physics toolbar, click  Boundaries and choose Heat Flux.
2
Select Boundaries 17 and 27 only.
3
In the Settings window for Heat Flux, locate the Heat Flux section.
4
In the q0 text field, type 1e4.
Mesh 1
1
In the Model Builder window, under Component 1 (comp1) click Mesh 1.
2
In the Settings window for Mesh, locate the Physics-Controlled Mesh section.
3
From the Element size list, choose Finer.
4
Locate the Sequence Type section. From the list, choose User-controlled mesh.
Size
1
In the Model Builder window, under Component 1 (comp1) > Mesh 1 click Size.
2
In the Settings window for Size, locate the Element Size Parameters section.
3
In the Maximum element size text field, type 6[mm].
4
Click  Build All.
Study 1
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
By default, a segregated solver is generated. In this case, the problem is linear and — because the heat-transfer problem is independent of the structural-mechanics solution — unidirectionally coupled. The thermal strains and the elastic properties depend on the temperature field. This means that it is sufficient to solve once for each physics interface as long as the heat-transfer problem is solved first. You can speed up the solution by using this fact.
2
In the Model Builder window, expand the Solution 1 (sol1) node.
3
In the Model Builder window, expand the Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 node.
4
In the Model Builder window, under Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 click Segregated 1.
5
In the Settings window for Segregated, locate the General section.
6
From the Termination technique list, choose Iterations.
7
In the Study toolbar, click  Compute.
Results
Stress (solid)
Under the Results node, two plot groups are automatically added to show the results for the structural and thermal analyses. The first plot group, Stress (solid), shows the von Mises stresses on a scaled deformed geometry, as shown in Figure 2.
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.
4
Click the  Show Grid button in the Graphics toolbar.
5
Click the  Zoom Extents button in the Graphics toolbar.
6
In the Stress (solid) toolbar, click  Plot.
Temperature (ht)
The second plot group, Temperature (ht), displays the temperature distribution. Add some arrows indicating the thermal loading.
Arrow Surface 1
1
In the Model Builder window, right-click Temperature (ht) and choose Arrow Surface.
2
In the Settings window for Arrow Surface, locate the Expression section.
3
In the X-component text field, type 0.
4
In the Y-component text field, type 0.
5
In the Z-component text field, type 1.
6
Locate the Coloring and Style section. From the Arrow base list, choose Head.
Selection 1
1
Right-click Arrow Surface 1 and choose Selection.
2
Select Boundaries 17 and 27 only.
Arrow Surface 1
1
In the Model Builder window, click Arrow Surface 1.
2
In the Settings window for Arrow Surface, locate the Arrow Positioning section.
3
In the Number of arrows text field, type 100.
4
Locate the Coloring and Style section.
5
Select the Scale factor checkbox. In the associated text field, type 0.02.
Volume 1
1
In the Model Builder window, click Volume 1.
2
In the Settings window for Volume, locate the Expression section.
3
In the Unit field, type degC.
Transparency 1
1
Right-click Volume 1 and choose Transparency.
2
In the Settings window for Transparency, locate the Transparency section.
3
Find the Transparency subsection. Set the Transparency value to 0.4.
4
Find the Fresnel transmittance subsection. Set the Fresnel transmittance value to 0.4.
5
In the Temperature (ht) toolbar, click  Plot.