PDF
Assembly with a Hinge
Introduction
In mechanical assemblies, parts are sometimes connected so that they are free to move relative to each other in one or more degrees of freedom. Examples of such connections are ball joints, hinges, and different types of bearings. If the details of the connection are not the subjects of the analysis, it is often possible to model the connection using the Rigid Connector feature in COMSOL Multiphysics combined with some extra equations.
The current example illustrates how to model a barrel hinge connecting two solid objects in an assembly.
You can create a model like this much more conveniently by using the Multibody Dynamics Module. There you will for example find a predefined hinge joint.
Model Definition
Figure 1 shows the model geometry.
Figure 1: Model geometry.
The two parts of the assembly are connected through a barrel hinge that allows relative rotation only along the axis of the pin hole. All other degrees of freedom are common between the two parts.
The two holes of the forked bottom part are bolted, and can be considered as fully constrained.
The pin hole of the top part is constrained in the X direction so that it can slide in the YZ-plane.
A force of 1 kN is applied in the Z direction at a distance 10 cm in the negative Y direction from the center of the upper pin hole. The offset of the load thus introduces both tension and bending of the member.
Results and Discussion
The default plot shown in Figure 2 shows the von Mises stress in the model. You can see the bending of the top part due to the offset of the load. You can also see the stress that is transmitted around the hinge.
In Figure 3 the color gradient in the X direction displacement indicates that the lower, forked, part of the assembly is subjected to bending around the Y axis. Without the hinge, bending from one part would be transmitted to the next part. The upper part, however, shows a fairly constant displacement along the height, which indicates that it has a free rotation around the Y direction in the connection point.
Figure 2: von Mises stress distribution in the hinge assembly.
Figure 3:  Displacement field, X component.
Notes About the COMSOL Implementation
The approach when modeling the mechanism is to attach rigid connectors to both parts, make sure that they have a common center of rotation, and then couple relevant degrees of freedom between them in order to obtain the desired function.
When you model a hinge, all translations and two rotations should be equal in the two parts. As in this case, the displacement and the rotation in the hinge remain small, the procedure simply consists of linking the displacement in all directions as well as the rotation around the X and Z directions. You connect the displacements of the rigid connectors directly using the prescribed displacement setting available in the rigid connector node. In order to constrain the rotation directions independently, you need however to add two global constraints, one for each rotational degree of freedom. The rigid connector uses a quaternion representation of the rotation. For details, see the description in the Structural Mechanics User’s Guide. In this specific example both the b and the d rotation variables are coupled between the two rigid connectors, because they directly correspond to the rotation around X and Z axes for small rotations.
Another rigid connector is used for applying the force to the upper pin hole.
Application Library path: Structural_Mechanics_Module/Connectors_and_Mechanisms/hinge_assembly
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.
Global Definitions
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
F
1e3[N]
1000 N
Applied load
Geometry 1
Import 1 (imp1)
1
In the Home 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 hinge_assembly.mphbin.
5
Click  Import.
Form Union (fin)
1
In the Model Builder window, under Component 1 (comp1) > Geometry 1 click Form Union (fin).
2
In the Settings window for Form Union/Assembly, locate the Form Union/Assembly section.
3
From the Action list, choose Form an assembly.
4
Clear the Create pairs checkbox.
5
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)
Fixed Constraint 1
1
In the Physics toolbar, click  Boundaries and choose Fixed Constraint.
2
Select Boundaries 133–136 only.
Rigid Connector 1
1
In the Physics toolbar, click  Boundaries and choose Rigid Connector.
2
Select Boundaries 67 and 68 only.
3
In the Settings window for Rigid Connector, locate the Prescribed Displacement at Center of Rotation section.
4
Select the Prescribed in x direction checkbox.
Applied Force 1
1
In the Physics toolbar, click  Attributes and choose Applied Force.
2
In the Settings window for Applied Force, locate the Location section.
3
Select the Offset checkbox.
4
Specify the Xoffset vector as
0
x
-0.1
y
0
z
5
Locate the Applied Force section. Specify the F vector as
0
x
0
y
F
z
Rigid Connector 2
1
In the Physics toolbar, click  Boundaries and choose Rigid Connector.
2
Select Boundaries 75 and 76 only.
Rigid Connector 3
1
In the Physics toolbar, click  Boundaries and choose Rigid Connector.
2
Select Boundaries 16–19 only.
Set the translations of this rigid connector equal to the translations of the second rigid connector.
3
In the Settings window for Rigid Connector, locate the Prescribed Displacement at Center of Rotation section.
4
Select the Prescribed in x direction checkbox.
5
In the u0x text field, type solid.rig2.u.
6
Select the Prescribed in y direction checkbox.
7
In the u0y text field, type solid.rig2.v.
8
Select the Prescribed in z direction checkbox.
9
In the u0z text field, type solid.rig2.w.
10
Click the  Show More Options button in the Model Builder toolbar.
11
In the Show More Options dialog, in the tree, select the checkbox for the node Physics > Equation Contributions.
12
Click OK.
Connect the rotations around the x and z directions, using the quaternion degrees of freedom ’b’ and ’d’.
Global Constraint 1
1
In the Physics toolbar, click  Global and choose Global Constraint.
2
In the Settings window for Global Constraint, locate the Global Constraint section.
3
In the Constraint expression text field, type comp1.solid.rig2.b-comp1.solid.rig3.b.
Global Constraint 2
1
In the Physics toolbar, click  Global and choose Global Constraint.
2
In the Settings window for Global Constraint, locate the Global Constraint section.
3
In the Constraint expression text field, type comp1.solid.rig2.d-comp1.solid.rig3.d.
Mesh 1
Free Tetrahedral 1
In the Mesh toolbar, click  Free Tetrahedral.
Size 1
1
Right-click Free Tetrahedral 1 and choose Size.
2
In the Settings window for Size, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Boundary.
4
Select Boundaries 41, 42, and 53 only.
5
Locate the Element Size section. Click the Custom button.
6
Locate the Element Size Parameters section.
7
Select the Maximum element size checkbox. In the associated text field, type 0.002.
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 section.
3
From the Predefined list, choose Fine.
4
Click  Build All.
Study 1
In the Study toolbar, click  Compute.
Results
Stress (solid)
The default plot shows the von Mises stress distribution on the surface of the assembly. Compare with Figure 2.
Finally, reproduce the x-displacement plot shown in Figure 3 with the following steps:
Stress (solid) 1
Right-click Stress (solid) and choose Duplicate.
Volume 1
1
In the Model Builder window, expand the Stress (solid) 1 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 > Displacement > Displacement field - m > u - Displacement field, X-component.
3
In the Stress (solid) 1 toolbar, click  Plot.
x-Displacement
1
In the Model Builder window, under Results click Stress (solid) 1.
2
In the Settings window for 3D Plot Group, type x-Displacement in the Label text field.