PDF
Door Slam Analysis
Introduction
This example illustrates the modeling of a car door slam event. This type analysis is important for several reasons:
•
It should be easy to close the door at different speeds, both by a soft closure and by an aggressive slam.
•
Usually there are loudspeakers mounted in the doors. Such components can be sensitive to excessive accelerations.
•
The hinges must be able to withstand the forces caused by repetitive door slams.
•
The pressure on the seals when the door is closed is an important factor for keeping noise a dust out of the compartment.
•
The sound emitted when a car door is closed is important to the perception of quality.
The model in this example is simplified in several ways, most importantly:
•
The geometry of a real car door is far more complex.
•
There are no components, such as loudspeakers, in the door.
•
The glass pane is omitted.
•
The seals are made from homogeneous rubber. A real door seal will usually have an internal air cavity with intermittent evacuation holes, which makes the stiffness strongly velocity dependent.
•
The locking mechanism is simplified.
Model Definition
Figure 1 shows the geometry of the car door and the frame in the car body. .
Figure 1: Geometry of the car door and the frame.
The material in the door is aluminum, with data taken from the Material Library. The rubber material in the seals have the following properties:
•
Material model: Mooney-Rivlin
•
C10  = 0.37 MPa
•
C01 = 0.11 MPa
•
Mass density 1100 kg/m3
The door starts at position where it is opened 30°. It is given an initial angular velocity of 2 rad/s, corresponding to a velocity of about 1.4 m/s at the outermost point.
A penalty method is chosen for the contact modeling. The penalty factor is set fairly high in order to avoid excessive overclosure of the contact boundaries. The penalty function is set to Smooth ramp. This can improve performance significantly for impact problems.
To model the locking mechanism, simple unidirectional damper with a high viscosity is used. As soon as the velocity if the door is reversed, this damper is activated and effectively stops the rebound. The damper is implemented using a weak contribution.
Results and Discussion
The stress distribution in the door after the system has come to rest is shown in Figure 2. This stress state is an effect of that the locking mechanism keeps the door pressed against seals.
Note that all stress values as such are of little value because of the crude representation of the door and the low-order elements used,
Figure 2: Equivalent von Mises stress in the door at the end of the event.
In Figure 3 and Figure 4, the stress distributions in the two seals at the end of the event are shown.
Figure 3: Stress distribution in the seal on the door at the end of the event.
Figure 4: Stress distribution in the seal at the end of the event.
In Figure 5, the acceleration normal to the door is shown in two points on the door. This type of results are useful for evaluating the forces in components mounted on the door.
Figure 5: Acceleration in two points in the door during the door slam event.
The forces and moments acting on the hinges are shown in Figure 6 to Figure 9.
Figure 6: Forces in the upper hing during the door slam event.
Figure 7: Forces in the lower hinge during the door slam event.
Figure 8: Moments in the upper hinge during the door slam event.
Figure 9: Moments in the lower hinge as during the door slam event.
Figure 10: Rotation in the upper hinge during the door slam event.
Notes About the COMSOL Implementation
Two physics interfaces are used in the model: Solid Mechanics and Joints. All types of joints can be modeled either using the Joints interface or using the Multibody Dynamics interface. If this analysis had involved only linear elastic material, it had been sufficient yo use only a Multibody Dynamics interface. Since the rubber seals are modeled as hyperelastic, the Solid Mechanics interface has to be used. The hinge joints is then most easily introduced by adding a Joints interface. In either case, the Multibody Dynamics module is required.
Linear shape functions are used in this example to speed up the solution. First order elements are known to have bad predictive capabilities for stresses, so this type of modeling is only suitable for determining displacements, velocities, and accelerations.
In this example, a General Contact Pair node together with a General Contact node in the Solid Mechanics interface is used for modeling the contact between seals, car frame, and car door. An alternative is to use three Contact Pair nodes together with a Contact node. The latter method is computationally more efficient, and will in this case lead to about 30% shorter solution time. The setup is however mote complicated, since you need to define three contact pairs together with their boundary selections, and also take meshing constraints into account.
The locking of the door is modeled by activating a strong viscous damper at the lock position at the moment when the door starts to bounce back. This is implemented in a Weak Contribution node.
Application Library path: Multibody_Dynamics_Module/Tutorials/door_slam_analysis
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
In the Select Physics tree, select Structural Mechanics > Joints (joints).
5
Click Add.
6
Click  Study.
7
In the Select Study tree, select General Studies > Time Dependent.
8
Click  Done.
Geometry 1
You can import the geometry of the door assembly by browsing to the model’s Application Libraries folder.
1
In the Model Builder window, expand the Component 1 (comp1) > Geometry 1 node, then click Geometry 1.
2
In the Settings window for Geometry, locate the Advanced section.
3
From the Geometry representation list, choose CAD kernel.
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 door_slam_analysis.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
In the Geometry toolbar, click  Build All.
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
omegaInit
2[rad/s]
2 rad/s
Initial angular velocity
Definitions
Now, create selections in the geometry. You will use them later when setting up the physics and mesh.
Door Seal
1
In the Definitions toolbar, click  Explicit.
2
Select Domain 4 only.
3
In the Settings window for Explicit, type Door Seal in the Label text field.
Body Seal
1
Right-click Door Seal and choose Duplicate.
2
In the Settings window for Explicit, type Body Seal in the Label text field.
3
Locate the Input Entities section. Click  Clear Selection.
4
Select Domain 1 only.
Seals
1
In the Definitions toolbar, click  Union.
2
In the Settings window for Union, type Seals in the Label text field.
3
Locate the Input Entities section. Under Selections to add, click  Add.
4
In the Add dialog, in the Selections to add list, choose Door Seal and Body Seal.
5
Click OK.
Body
1
In the Model Builder window, right-click Door Seal and choose Duplicate.
2
In the Settings window for Explicit, type Body in the Label text field.
3
Locate the Input Entities section. Click  Clear Selection.
4
Select Domain 2 only.
Door
1
Right-click Body and choose Duplicate.
2
In the Settings window for Explicit, type Door in the Label text field.
3
Locate the Input Entities section. Click  Clear Selection.
4
Select Domains 3 and 5 only.
Hinges
1
Right-click Door and choose Duplicate.
2
In the Settings window for Explicit, type Hinges in the Label text field.
3
Locate the Input Entities section. Click  Clear Selection.
4
Select Domains 6 and 7 only.
Door with Seal and Hinges
1
In the Model Builder window, right-click Seals and choose Duplicate.
2
In the Settings window for Union, type Door with Seal and Hinges in the Label text field.
3
Locate the Input Entities section. In the Selections to add list box, select Body Seal.
4
Under Selections to add, click  Delete.
5
Under Selections to add, click  Add.
6
In the Add dialog, select Door in the Selections to add list.
7
Click OK.
8
In the Settings window for Union, locate the Input Entities section.
9
Under Selections to add, click  Add.
10
In the Add dialog, select Hinges in the Selections to add list.
11
Click OK.
Hinge 1: Inner Boundaries
1
In the Model Builder window, right-click Door Seal and choose Duplicate.
2
In the Settings window for Explicit, type Hinge 1: Inner Boundaries in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Click  Clear Selection.
5
Select the Group by continuous tangent checkbox.
6
Select Boundaries 57, 58, 60, 68, and 74 only.
Hinge 2: Inner Boundaries
1
Right-click Hinge 1: Inner Boundaries and choose Duplicate.
2
In the Settings window for Explicit, type Hinge 2: Inner Boundaries in the Label text field.
3
Locate the Input Entities section. Click  Clear Selection.
4
Select Boundaries 55, 56, 59, 67, and 70 only.
Average 1 (aveop1)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Average.
2
In the Settings window for Average, locate the Source Selection section.
3
From the Geometric entity level list, choose Boundary.
4
Select Boundary 18 only.
5
Locate the Advanced section. From the Frame list, choose Material  (X, Y, Z).
Variables 1
1
In the Model Builder window, right-click Definitions and choose Variables.
2
In the Settings window for Variables, locate the Variables section.
3
Right-click and choose Paste.
4
In the table, enter the following settings:
Name
Expression
Unit
Description
vel
aveop1(d(v,TIME))
m/s
Velocity
disp
aveop1(v)
m
Displacement
General Contact Pair 1 (p1)
Create contact pairs between different components, which can come into contact when the door closes. To make the contact search more efficient, select only domains that can come into contact.
1
In the Definitions toolbar, click  Pairs and choose General Contact Pair.
2
In the Settings window for Pair, locate the Contact Selection section.
3
From the Selection list, choose Manual.
4
Locate the Domain Selection section. Click to select the  Activate Selection toggle button.
5
Select Domains 1–4 only.
Solid Mechanics (solid)
1
In the Model Builder window, under Component 1 (comp1) click Solid Mechanics (solid).
2
In the Settings window for Solid Mechanics, click to expand the Discretization section.
3
From the Displacement field list, choose Linear.
Hyperelastic Material: Seals
1
In the Physics toolbar, click  Domains and choose Hyperelastic Material.
2
In the Settings window for Hyperelastic Material, type Hyperelastic Material: Seals in the Label text field.
3
Locate the Domain Selection section. From the Selection list, choose Seals.
4
Locate the Hyperelastic Material section. From the Material model list, choose Mooney–Rivlin, two parameters.
Damping 1
1
In the Physics toolbar, click  Attributes and choose Damping.
2
In the Settings window for Damping, locate the Damping Settings section.
3
In the αdM text field, type 0.5.
4
In the βdK text field, type 0.002.
Contact Model 1
1
In the Model Builder window, expand the General Contact 1 node, then click Contact Model 1.
2
In the Settings window for Contact Model, locate the Contact Model section.
3
Find the Penalty function subsection. From the list, choose Smooth ramp.
Fixed Constraint: Body
1
In the Physics toolbar, click  Boundaries and choose Fixed Constraint.
2
In the Settings window for Fixed Constraint, type Fixed Constraint: Body in the Label text field.
3
Select Boundary 5 only.
Attachment: Upper Hinge
1
In the Physics toolbar, click  Boundaries and choose Attachment.
2
In the Settings window for Attachment, type Attachment: Upper Hinge in the Label text field.
3
Locate the Boundary Selection section. From the Selection list, choose Hinge 1: Inner Boundaries.
Attachment: Lower Hinge
1
Right-click Attachment: Upper Hinge and choose Duplicate.
2
In the Settings window for Attachment, type Attachment: Lower Hinge in the Label text field.
3
Locate the Boundary Selection section. From the Selection list, choose Hinge 2: Inner Boundaries.
Attachment: Lower Hinge, Attachment: Upper Hinge
1
In the Model Builder window, under Component 1 (comp1) > Solid Mechanics (solid), Ctrl-click to select Attachment: Upper Hinge and Attachment: Lower Hinge.
2
Right-click and choose Group.
Attachments
In the Settings window for Group, type Attachments in the Label text field.
Initial Values: Door
1
In the Physics toolbar, click  Domains and choose Initial Values.
2
In the Settings window for Initial Values, type Initial Values: Door in the Label text field.
3
Locate the Domain Selection section. From the Selection list, choose Door with Seal and Hinges.
4
In the Settings window for Initial Values, locate the Initial Values section.
5
In the Structural velocity field vector, enter
omegaInit*(Y-solid.att1.xcy)
X
-omegaInit*(X-solid.att1.xcx)
Y
6
Click the  Show More Options button in the Model Builder toolbar.
7
In the Show More Options dialog, in the tree, select the checkbox for the node Physics > Advanced Physics Options.
8
Click OK.
9
Click the  Show More Options button in the Model Builder toolbar.
10
In the tree, select the checkbox for the node Physics > Equation Contributions.
11
Click OK.
Weak Contribution: Locking Condition
1
In the Physics toolbar, click  Global and choose Weak Contribution.
The locking mechanism is modeled by a high viscous damping which is activated once the door tries to bounce back.
2
In the Settings window for Weak Contribution, type Weak Contribution: Locking Condition in the Label text field.
3
Locate the Weak Contribution section. In the Weak expression text field, type if(disp>0.34&&vel<=0,-1e8*vel*test(disp),0).
Joints (joints)
Upper Hinge
1
In the Physics toolbar, click  Global and choose Hinge Joint.
2
In the Settings window for Hinge Joint, type Upper Hinge in the Label text field.
3
Locate the Attachment Selection section. From the Source list, choose Fixed.
4
From the Destination list, choose Attachment: Upper Hinge (solid).
5
Locate the Axis of Joint section. Specify the e0 vector as
0
x
1
z
Lower Hinge
1
Right-click Upper Hinge and choose Duplicate.
2
In the Settings window for Hinge Joint, type Lower Hinge in the Label text field.
3
Locate the Attachment Selection section. From the Destination list, choose Attachment: Lower Hinge (solid).
Materials
Assign material properties. Use Aluminum for door and body.
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 > Aluminum.
4
Right-click and choose Add to Component 1 (comp1).
5
In the Materials toolbar, click  Add Material to close the Add Material window.
Materials
Add model specific data for the rubber in the seals.
Seal Rubber
1
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Blank Material.
2
In the Settings window for Material, type Seal Rubber in the Label text field.
3
Locate the Geometric Entity Selection section. From the Selection list, choose Seals.
4
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Model parameters
C10
0.37[MPa]
Pa
Mooney-Rivlin
Model parameters
C01
0.11[MPa]
Pa
Mooney-Rivlin
Density
rho
1100
kg/m³
Basic
Mesh 1
Free Triangular 1
1
In the Mesh toolbar, click  More Generators and choose Free Triangular.
2
Select Boundaries 199, 209, and 300 only.
Size 1
1
Right-click Free Triangular 1 and choose Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Extremely fine.
Free Quad 1
1
In the Mesh toolbar, click  More Generators and choose Free Quad.
2
Select Boundaries 41, 42, 47, 48, 51, 54, 63, 66, 72, and 76 only.
Size 1
1
Right-click Free Quad 1 and choose Size.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Extremely fine.
Swept 1
1
In the Mesh toolbar, click  Swept.
2
In the Settings window for Swept, locate the Domain Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domains 1, 2, 4, and 6–34 only.
Distribution 1
1
Right-click Swept 1 and choose Distribution.
2
Select Domains 1, 2, 4, 12–15, 18, 19, 24, 25, 28, 29, 31, and 34 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 40.
Distribution 2
1
In the Model Builder window, right-click Swept 1 and choose Distribution.
2
Select Domains 8–11, 16, 17, 20–27, 30, and 32–34 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 12.
Distribution 3
1
Right-click Swept 1 and choose Distribution.
2
Select Domains 6 and 7 only.
3
In the Settings window for Distribution, locate the Distribution section.
4
In the Number of elements text field, type 6.
Free Triangular 2
1
In the Mesh toolbar, click  More Generators and choose Free Triangular.
2
Select Boundaries 14, 15, 18, and 29–35 only.
Size 1
1
Right-click Free Triangular 2 and choose Size.
2
Select Boundaries 30–35 only.
3
In the Settings window for Size, locate the Element Size section.
4
Click the Custom button.
5
Locate the Element Size Parameters section.
6
Select the Minimum element size checkbox. In the associated text field, type 0.0015.
Size 2
1
In the Model Builder window, right-click Free Triangular 2 and choose Size.
2
Select Boundaries 14, 15, 18, and 29 only.
3
In the Settings window for Size, locate the Element Size section.
4
From the Predefined list, choose Extra fine.
Free Tetrahedral 1
1
In the Mesh toolbar, click  Free Tetrahedral.
2
In the Settings window for Free Tetrahedral, click  Build All.
Size 1
1
Right-click Free Tetrahedral 1 and choose 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
Step 1: Time Dependent
1
In the Model Builder window, under Study 1 click Step 1: Time Dependent.
2
In the Settings window for Time Dependent, locate the Study Settings section.
3
In the Output times text field, type range(0,0.01,0.24) range(0.24,0.0005,0.35).
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
The default solver suggests a segregated solver, which is not appropriate for this type of tight coupling between two physics interfaces.
2
In the Model Builder window, expand the Solution 1 (sol1) node.
3
Right-click Study 1 > Solver Configurations > Solution 1 (sol1) > Time-Dependent Solver 1 and choose Fully Coupled.
By allowing some more iterations, you can avoid many time step changes if the nonlinear solver is on the verge of reaching convergence.
4
In the Settings window for Fully Coupled, click to expand the Method and Termination section.
5
In the Maximum number of iterations text field, type 6.
6
In the Study toolbar, click  Compute.
Results
1
Click the  Show Grid button in the Graphics toolbar.
2
Click the  Zoom Extents button in the Graphics toolbar.
Preferred Units 1
1
In the Results toolbar, click  Configurations and choose Preferred Units.
2
In the Settings window for Preferred Units, locate the Units section.
3
Click  Add Physical Quantity.
4
In the Physical Quantity dialog, type stre in the text field.
5
In the tree, select Solid Mechanics > Stress tensor (N/m^2).
6
Click OK.
7
In the Settings window for Preferred Units, locate the Units section.
8
In the table, enter the following settings:
Quantity
Unit
Preferred unit
Stress tensor
N/m^2
MPa
9
Select the Apply conversions to expressions with the same dimensions checkbox.
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
Click to expand the Range section. Select the Manual color range checkbox.
5
In the Maximum text field, type 10.
6
Click to expand the Quality section. From the Resolution list, choose Normal.
7
From the Smoothing list, choose Everywhere.
8
From the Smoothing threshold list, choose None.
9
In the Stress (solid) toolbar, click  Plot.
Stress: Door Seal
1
In the Model Builder window, right-click Stress (solid) and choose Duplicate.
2
In the Settings window for 3D Plot Group, click to expand the Selection section.
3
From the Geometric entity level list, choose Domain.
4
From the Selection list, choose Door Seal.
5
In the Label text field, type Stress: Door Seal.
Volume 1
1
In the Model Builder window, expand the Stress: Door Seal node, then click Volume 1.
2
In the Settings window for Volume, locate the Range section.
3
In the Maximum text field, type 0.2.
4
In the Stress: Door Seal toolbar, click  Plot.
Stress: Body Seal
1
In the Model Builder window, right-click Stress: Door Seal and choose Duplicate.
2
In the Settings window for 3D Plot Group, type Stress: Body Seal in the Label text field.
3
Locate the Selection section. From the Selection list, choose Body Seal.
4
In the Stress: Body Seal toolbar, click  Plot.
Cut Point 3D 1
1
In the Results toolbar, click  Cut Point 3D.
2
In the Settings window for Cut Point 3D, locate the Point Data section.
3
In the X text field, type -0.6 0.1.
4
In the Y text field, type -0.4.
5
In the Z text field, type 0.2.
6
From the Snapping list, choose Snap to closest boundary.
Acceleration
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Acceleration in the Label text field.
3
Locate the Data section. From the Dataset list, choose Cut Point 3D 1.
4
Click to expand the Title section. From the Title type list, choose None.
Point Graph 1
1
Right-click Acceleration and choose Point Graph.
2
In the Settings window for Point Graph, locate the Data section.
3
From the Dataset list, choose Cut Point 3D 1.
4
Click Replace Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1) > Solid Mechanics > Acceleration and velocity > Acceleration - m/s² > solid.u_ttY - Acceleration, Y-component.
5
Click to expand the Legends section. Select the Show legends checkbox.
6
From the Legends list, choose Manual.
7
In the table, enter the following settings:
Legends
Point A
Point B
8
In the Acceleration toolbar, click  Plot.
Force: Upper Hinge
1
In the Results toolbar, click  1D Plot Group.
2
In the Settings window for 1D Plot Group, type Force: Upper Hinge in the Label text field.
3
Locate the Title section. From the Title type list, choose Label.
4
Locate the Plot Settings section.
5
Select the y-axis label checkbox. In the associated text field, type Joint Force (N).
6
Locate the Legend section. From the Position list, choose Upper left.
Global 1
1
Right-click Force: Upper Hinge and choose Global.
2
In the Settings window for Global, click Add Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1) > Joints > Hinge joints > Upper Hinge > Joint force - N > All expressions in this group.
Force: Upper Hinge
1
In the Model Builder window, click Force: Upper Hinge.
2
In the Force: Upper Hinge toolbar, click  Plot.
Force: Lower Hinge
1
Right-click Force: Upper Hinge and choose Duplicate.
2
In the Model Builder window, click Force: Upper Hinge 1.
3
In the Settings window for 1D Plot Group, type Force: Lower Hinge in the Label text field.
Global 1
1
In the Model Builder window, click Global 1.
2
In the Settings window for Global, click Replace Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1) > Joints > Hinge joints > Lower Hinge > Joint force - N > All expressions in this group.
Force: Lower Hinge
1
In the Model Builder window, click Force: Lower Hinge.
2
In the Force: Lower Hinge toolbar, click  Plot.
Moment: Upper Hinge
1
Right-click Force: Lower Hinge and choose Duplicate.
2
In the Model Builder window, click Force: Lower Hinge 1.
3
In the Settings window for 1D Plot Group, type Moment: Upper Hinge in the Label text field.
4
Locate the Plot Settings section. In the y-axis label text field, type Joint Moment (N-m).
Global 1
1
In the Model Builder window, click Global 1.
2
In the Settings window for Global, click Replace Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1) > Joints > Hinge joints > Upper Hinge > Joint moment - N·m > All expressions in this group.
Moment: Upper Hinge
1
In the Model Builder window, click Moment: Upper Hinge.
2
In the Moment: Upper Hinge toolbar, click  Plot.
Moment: Lower Hinge
1
Right-click Moment: Upper Hinge and choose Duplicate.
2
In the Model Builder window, click Moment: Upper Hinge 1.
3
In the Settings window for 1D Plot Group, type Moment: Lower Hinge in the Label text field.
Global 1
1
In the Model Builder window, click Global 1.
2
In the Settings window for Global, click Replace Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1) > Joints > Hinge joints > Lower Hinge > Joint moment - N·m > All expressions in this group.
Moment: Lower Hinge
1
In the Model Builder window, click Moment: Lower Hinge.
2
In the Moment: Lower Hinge toolbar, click  Plot.
Joint Rotation
1
Right-click Moment: Lower Hinge and choose Duplicate.
2
In the Model Builder window, click Moment: Lower Hinge 1.
3
In the Settings window for 1D Plot Group, type Joint Rotation in the Label text field.
4
Locate the Legend section. Clear the Show legends checkbox.
5
Locate the Plot Settings section. In the y-axis label text field, type Rotation (deg).
Global 1
1
In the Model Builder window, click Global 1.
2
In the Settings window for Global, locate the y-Axis Data section.
3
Click  Clear Table.
4
In the table, enter the following settings:
Expression
Unit
Description
-joints.hgj1.th
deg
Rotation
Joint Rotation
1
In the Model Builder window, click Joint Rotation.
2
In the Joint Rotation toolbar, click  Plot.
Force: Lower Hinge, Force: Upper Hinge
1
In the Model Builder window, under Results, Ctrl-click to select Force: Upper Hinge and Force: Lower Hinge.
2
Right-click and choose Group.
Joint Forces
In the Settings window for Group, type Joint Forces in the Label text field.
Moment: Lower Hinge, Moment: Upper Hinge
1
In the Model Builder window, under Results, Ctrl-click to select Moment: Upper Hinge and Moment: Lower Hinge.
2
Right-click and choose Group.
Joint Moments
In the Settings window for Group, type Joint Moments in the Label text field.
Stress
1
In the Results toolbar, click  Animation and choose Player.
2
In the Settings window for Animation, type Stress in the Label text field.
3
Locate the Frames section. In the Number of frames text field, type 200.
Displacement
1
Right-click Stress and choose Duplicate.
2
In the Settings window for Animation, type Displacement in the Label text field.
3
Locate the Scene section. From the Subject list, choose Acceleration.