Assembly with a Hinge Joint

In mechanical assemblies, parts are sometimes connected so that they are free to move relative to each other with one or multiple 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 possible to model the connection using joint nodes in the Multibody Dynamics Module.

This example illustrates how to model a barrel hinge connecting two solid objects in an assembly. Two different versions are studied. In one of them, both parts are flexible. In the other version, one of the parts is considered as rigid.

Model Definition

Figure 1 shows the model geometry.

Figure 1: Model geometry.

Two parts of the assembly are connected through a barrel hinge that allows relative rotation as well as sliding along the axis of the pin hole. All the other degrees of freedom are shared between the two parts.

One hole of the forked bottom part is modeled as a hinge joint and other hole is modeled as a cylindrical joint allowing the axial motion.

The pin hole of the top part is constrained in the x direction so that it can slide in the y-z plane.

A force of 1 kN is applied in z direction at a 10 cm distance in the negative y direction from the center of the upper pin hole. The offset of the load introduces both tension and bending of the member.

In a second study, the upper part is considered as rigid, and it only transmits the force through the hinge.

Results and Discussion

The default displacement plot for the flexible model is shown in Figure 2.

Figure 2: Displacement of the flexible structure.

In Figure 3 you can see the stress distribution.

Figure 3: Equivalent stress in the flexible structure

In a model that consists of a mix of rigid and flexible parts, stresses can only be displayed in the flexible parts. This is shown in Figure 4.

If you compare Figure 3 and Figure 4, you can see that the stress distribution in the lower part is essentially unaffected by the fact that the load is transmitted through a rigid body.

Figure 4: Equivalent stress in the flexible part when one component is rigid.

Notes About the COMSOL Implementation

When the flexibility of a component can be neglected and its stress distribution is not of interest, it is efficient to treat such a component as a rigid domain. The rigid domain is a domain that has a material model with only one material parameter, the density.

A node can establish a connection directly between nodes however nodes are needed, defining the connection boundaries, for flexible elements.

Multibody_Dynamics_Module/Tutorials/hinge_joint_assembly

Modeling Instructions

From the menu, choose .

New

In the window, click

Model Wizard

In the window, click

In the tree, select .

Click .

Click

In the tree, select .

Click

Global Definitions

Parameters 1

In the window, under click .

In the window for , locate the section.

In the table, enter the following settings:


Name	Expression	Value	Description
F	1e3[N]	1000 N	Applied load

Geometry 1

Import 1 (imp1)

In the toolbar, click

In the window for , locate the section.

Click

Browse to the model’s Application Libraries folder and double-click the file hinge_assembly.mphbin.

Click

Form Union (fin)

In the window, under click .

In the window for , locate the section.

From the list, choose .

Clear the check box.

Click

Add Material

In the toolbar, click

to open the window.

Go to the window.

In the tree, select .

Click in the window toolbar.

In the toolbar, click

to close the window.

Multibody Dynamics (mbd)

Fixed Constraint 1

In the window, under right-click and choose .

Select Boundaries 133–136 only.

Use node to constrain the motion and apply load.

Rigid Connector 1

In the toolbar, click

and choose .

Select Boundaries 67 and 68 only.

In the window for , locate the section.

Select the check box.

Applied Force 1

In the toolbar, click

and choose .

In the window for , locate the section.

Select the check box.

Specify the Xoffset vector as


0	x
-0.1	y
0	z

The center of rotation for a rigid connector is available in the variables xcx_tag, xcy_tag, and xcz_tag. The default position is the center of gravity of the attached boundaries, which in this case will be the center of the hole.

Locate the section. Specify the F vector as


0	x
0	y
F	z

Attachment 1

In the toolbar, click

and choose .

Select Boundaries 16 and 17 only.

In the window for , locate the section.

From the list, choose .

Attachment 2

In the toolbar, click

and choose .

Select Boundaries 18 and 19 only.

In the window for , locate the section.

From the list, choose .

Attachment 3

In the toolbar, click

and choose .

Select Boundaries 75 and 76 only.

In the window for , locate the section.

From the list, choose .

Hinge Joint 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. Specify the e0 vector as


0	x
1	y
0	z

Cylindrical Joint 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Locate the section. Specify the e0 vector as


0	x
1	y
0	z

If you want accurate stress results, then quadratic shape functions should be used for the displacements. The default value in the Multibody Dynamics interface is linear shape functions.

In the window, click .

In the window for , click to expand the section.

From the list, choose .

Mesh 1

Free Tetrahedral 1

In the toolbar, click

Size 1

Right-click and choose .

In the window for , locate the section.

From the list, choose .

Select Boundaries 41, 42, and 53 only.

Locate the section. Click the button.

Locate the section.

Select the check box. In the associated text field, type 0.002.

Size

In the window, under click .

In the window for , locate the section.

From the list, choose .

Click

Study 1

In the toolbar, click

Results

Displacement (mbd)

In the toolbar, click

The default plot shows the displacement of the assembly. Compare with Figure 2.

Reproduce the stress plot shown in Figure 3 with the following steps.

Stress

In the toolbar, click

and choose .

In the window for , type Stress in the text field.

Surface 1

Right-click and choose .

In the window for , click in the upper-right corner of the section. From the menu, choose .

In the toolbar, click

Click to expand the section. Select the check box.

In the text field, type 6E7.

Locate the section. Click

In the dialog box, select in the tree.

Click .

Stress

In the window, click .

In the window for , locate the section.

Select the check box.

In the toolbar, click

Make the upper lever rigid and analyze that configuration in a new study.

Multibody Dynamics (mbd)

Rigid Material 1

In the toolbar, click

and choose .

Select Domain 1 only.

Use subnodes to constrain the motion and apply load.

Prescribed Displacement/Rotation 1

In the toolbar, click

and choose .

In the window for , locate the section.

Select the check box.

Locate the section. From the list, choose .

Center of Rotation: Boundary 1

In the window, expand the node, then click .

Select Boundaries 67 and 68 only.

Rigid Material 1

In the window, under click .

Applied Force 1

In the toolbar, click

and choose .

In the window for , locate the section.

From the list, choose .

Specify the Xp vector as


mbd.rd1.pdr1.xcx	x
mbd.rd1.pdr1.xcy-0.1	y
mbd.rd1.pdr1.xcz	z

Locate the section. Specify the F vector as


0	x
0	y
F	z

Add an extra node, so that it is easy to rerun the original version of the model. Normally it would have been easier just to utilize the existing joint.

Add Study

In the toolbar, click