PDF
Stresses and Strains in a Wrench
Introduction
This tutorial demonstrates how to set up a simple static structural analysis. The analysis is exemplified on a combination wrench during the application of torque on a bolt.
Despite its simplicity, and the fact that very few engineers would run a structural analysis before trying to turn a bolt, the example provides an excellent overview of structural analysis in COMSOL Multiphysics.
Another, more extensive variant of this tutorial is available in the Introduction to COMSOL Multiphysics document.
Model Definition
The model geometry is shown below.
The bolt’s fixed constraint is at the cross section shown below. A load is applied at the box end of the combination wrench.
Here, assume that there is perfect contact between the wrench and the bolt. A possible extension is to apply a contact condition between the wrench and the bolt where the friction and the contact pressure determines the position of the contact surface.
Application Library path: COMSOL_Multiphysics/Structural_Mechanics/wrench
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 > Solid Mechanics (solid).
3
Click Add.
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
Click  Browse.
4
Browse to the model’s Application Libraries folder and double-click the file wrench.mphbin.
5
Click  Build All Objects.
6
Click the  Zoom Extents button in the Graphics toolbar.
Boundary load
1
In the Geometry toolbar, click  Selections and choose Explicit Selection.
2
In the Settings window for Explicit Selection, type Boundary load in the Label text field.
3
Locate the Entities to Select section. From the Geometric entity level list, choose Boundary.
4
On the object imp1, select Boundary 111 only.
5
Click  Build Selected.
Fixed constraint
1
In the Geometry toolbar, click  Selections and choose Explicit Selection.
2
In the Settings window for Explicit Selection, type Fixed constraint in the Label text field.
3
Locate the Entities to Select section. From the Geometric entity level list, choose Boundary.
4
Click the  Wireframe Rendering button in the Graphics toolbar.
5
On the object imp1, select Boundary 35 only.
6
Click the  Wireframe Rendering button in the Graphics toolbar to turn off wireframe rendering.
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 Geometry Cleanup dialog that opens, click Clean Up Automatically to automatically clean up the geometry by removing some narrow face regions.
6
In the Materials toolbar, click  Add Material to close the Add Material window.
Global Definitions
Parameters 1
1
In the Settings window for Parameters, locate the Parameters section.
2
In the table, enter the following settings:
Name
Expression
Value
Description
F
150[N]
150 N
Applied force
Solid Mechanics (solid)
Fixed Constraint 1
1
In the Physics toolbar, click  Boundaries and choose Fixed Constraint.
2
In the Settings window for Fixed Constraint, locate the Boundary Selection section.
3
From the Selection list, choose Fixed constraint.
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
In the Settings window for Boundary Load, locate the Boundary Selection section.
3
From the Selection list, choose Boundary load.
4
Locate the Force section. From the Load type list, choose Total force.
5
Specify the Ftot vector as
0
x
0
y
-F
z
The minus sign means that the force is applied downward.
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 Normal.
Study 1
If your computer has more than 16 GB of RAM, you can skip the following four instructions and continue directly to the section Compute the Solution. Otherwise, follow these steps to use an iterative solver:
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
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
Right-click Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 > Suggested Iterative Solver (solid) and choose Enable.
Iterative solvers require less memory but can be less robust than direct solvers.
Compute the Solution
In the Study toolbar, click  Compute.
Results
Stress (solid)
The default plot group shows the von Mises stress in a Surface plot with the displacement visualized using a Deformation subnode. Change to a more suitable unit as follows.
Volume 1
1
In the Model Builder window, expand the Results > 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
In the Stress (solid) toolbar, click  Plot.
5
Click the  Zoom Extents button in the Graphics toolbar.
First Principal Strain
1
In the Model Builder window, right-click Stress (solid) and choose Duplicate.
2
In the Settings window for 3D Plot Group, type First Principal Strain in the Label text field.
Volume 1
1
In the Model Builder window, expand the First Principal Strain node, then click Volume 1.
2
In the Settings window for Volume, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Solid Mechanics > Strain > Principal strains > solid.ep1 - First principal strain - 1.
3
In the First Principal Strain toolbar, click  Plot.
Notice that the maximum principal strain is about 2%, a result that satisfies the small strain assumption.