PDF
Helicopter Swashplate Mechanism
Introduction
A swashplate is a device that translates the input of an helicopter flight control into the motion of rotor blades. As the rotor blades are spinning, the swashplate is used to transmit the pilot’s commands from the nonrotating fuselage to the rotating rotor hub and blades.
This model is built using the Multibody Dynamics interface in COMSOL Multiphysics. Transient and eigenfrequency analyses of the swashplate mechanism are performed in the model. Two different cases are considered for the transient analysis. In the first case, all parts of the mechanism are assumed rigid, whereas in the second case the rotor blades are made flexible while keeping the rest of the components rigid. The deformation in the rotor blades is the difference of rigid body motion obtained in the first case and the motion obtained in the second case. The latter includes both the rigid body motion and deformation.
Model Definition
The model geometry is shown in Figure 1. This section describes the components in the swashplate mechanism and the connections between them via different types of joints.
Figure 1: Geometry of the helicopter swashplate mechanism.
A list of all the components together with their state of motion is given below.
•
Baseplate (stationary)
•
Pushrod (3 in number, stationary)
•
Baseplate-Swashplate Link (2 in number, stationary)
•
Lower Swashplate (stationary)
•
Upper Swashplate (rotating)
•
Rotor Hub (rotating)
•
Sphere (rotating)
•
Rotor Blade (3 in number, rotating)
•
Swashplate-Blade Link (3 in number, rotating)
The baseplate is mounted on the fuselage and is connected to the lower swashplate using pushrods and links. Reduced slot, hinge and prismatic joints are used at the baseplate end of the pushrods and links. Ball joints are used at the swashplate end of the pushrods and links.
The lower swashplate is also connected to the upper swashplate through a planar joint and to the sphere through a ball joint. The sphere is connected to the rotor hub though a cylindrical joint.
The upper swashplate is connected to the rotor blades using links. Ball joints are used at the swashplate end of the links, whereas hinge joints are used at the blade end of the links. The rotor blades are connected to the rotor hub with hinge joints.
The cross-section of the rotor blades is modeled using a symmetric airfoil shape, shown in Figure 2.
material
Structural steel is used as a material for all the components of the helicopter swashplate mechanism.
Figure 2: Cross-section of the rotor blades (symmetric airfoil shape).
Lift force on the rotor blades
The helicopter is moving forward with a velocity of 100 km/h. The helicopter rotor and the other rotating parts are initialized to rotate at 300 RPM.
The lift force acts on the rotor blades due to the unsymmetrical pressure distribution in the airflow over the blades. This is modeled as the following distributed boundary load on the bottom surfaces of the rotor blades:
where the parameters read:
•
ρa — density of air (1 kg/m^3)
•
Cl — lift coefficient
•
Ur — relative velocity at a point over the rotor blades
•
α — angle of attack of rotor blades
•
ω — angular velocity of rotor blades
•
vf — forward speed of helicopter
•
d — distance of a point over the rotor blades from the center of rotation
•
x, y — spatial coordinates of a point over the rotor blades
Initial and boundary conditions
The rotor blades, along with all rotating components, are given an initial rotational velocity of 300 RPM. This is needed to avoid the transient effects in the solution.
The baseplate is fixed. The rotor’s hub is prescribed to rotate at 300 RPM. The pushrods are prescribed to move upward with a constant velocity of 0.5 m/s for some time lapse. This is needed to push the swashplate assembly upward and provide the angle of attack to all the rotor blades. The motion of the second pushrod is prescribed for comparatively longer time. This is needed to tilt the swashplate assembly, which in turn changes the angle of attack of rotor blades.
mesh
The mesh in all parts of the helicopter swashplate mechanism is shown in Figure 3. In this model, only the blades are modeled as flexible elements. Hence, a coarse mesh is used in all the other components.
A swept mesh is used to reduce the number of elements in the blades and yet to model the deformation of the blades accurately.
Figure 3: Mesh in the helicopter swashplate mechanism.
analyses performed
The following three types of analyses are performed in this model:
•
Transient analysis with rigid blades
•
Transient analysis with flexible blades
•
Eigenfrequency analysis with flexible blades
In case of eigenfrequency analysis, both the baseplate and rotor hub are fixed. The pushrods are free to move relative to the baseplate.
The second study also computes the displacement of the tip of one of the rotor blade which is pitching about its own axle as well as rotate about the rotor axis.
Results and Discussion
The configuration of the swashplate mechanism at t = 0.3 sec is shown in Figure 4. The tilt of the swashplate assembly can be seen. The velocity of the components is shown with the help of an arrow plot.
Figure 4: Configuration of the swashplate mechanism at a particular instant.
Figure 5 shows the variation in the angle of attack of each rotor blade due to the tilt of the swashplate assembly with respect to the angular rotation.
Initially, all three pushrods move upward with the same velocity, which forces the swashplate to move upward. The upward motion then increases the angle of attack for all the blades. However, after a certain time, only one of the pushrods continues to move upward, which causes the tilt of the swashplate. This tilt provides a continuous change in the angle of attack with respect to the rotation of the rotor.
The angle of attack of each blade changes from 2° to 17°.
Figure 5: Variation of the angle of attack of each rotor blade (rigid case).
Figure 6 shows the total lift force applied on each blade and its variation with respect to the rotation. The total lift on the first blade is computed for the following two cases. First, when the swashplate is tilted, and hence the blades change their angle of attack from 2° to 17°. Second, when the rotor blade is fixed at a mean angle of attack of 9.4°. Figure 7 clearly shows that in case of a varying angle of attack, the lift generated on the blade is much more uniform as compared to the case of a fixed angle of attack.
Figure 6: Variation of the total lift force on each rotor blade (rigid case).
Figure 7: Comparison of the total lift force on the first blade (rigid case).
Figure 8: Variation of the z-displacement of the tip for the second blade.
The variation of the tip displacement of the rotor blade in the z direction is shown in Figure 8. The tip displacement is shown for both rigid and flexible blades. In the case of rigid blades, the tip moves in the z direction due to the change in the angle of attack. However, in the case of flexible blades, they also deform.
Figure 9 shows the in-plane deformation of the flexible rotor blade at t = 0.3 sec. The deformation is plotted with respect to a reference frame defined by an attachment at the base of the blade. For better visualization, the deformation is scaled by a factor of 50. This in-plane deformation of the flexible blades is often referred to as the lead-lag phenomenon.
Figure 10 shows the out-of-plane deformation of the flexible rotor blade at t = 0.3 sec. The deformation is also scaled by a factor of 50. The out-of-plane deformation of the flexible blades is called the flapping phenomenon. Figure 11 shows the distribution of the von Mises stress in the flexible rotor blade at t = 0.3 sec.
The mode shapes of the helicopter swashplate assembly are shown in Figure 12 and Figure 13. The mechanism has three rigid body modes. The first plot shows the 6th mode, which is a bending mode and has its eigenfrequency close to 11.76 Hz. The second plot shows the 16th mode, which is a torsion mode with an eigenfrequency close to 181.43 Hz.
Figure 9: In-plane deformation of the flexible rotor blade at a particular instant (magnified).
Figure 10: Out-of-plane deformation of the flexible rotor blade at a particular instant (magnified).
Figure 11: von Mises stress distribution in the flexible rotor blade at a particular instant.
Figure 12: Mode shape of the helicopter swashplate mechanism (bending mode).
Figure 13: Mode shape of the helicopter swashplate mechanism (torsion mode).
Notes About the COMSOL Implementation
•
A Joint node can establish a direct connection between Rigid Material nodes. However, for flexible elements, Attachment nodes are needed to define the connection boundaries.
•
Constraint boundary conditions like Rigid Connector and Prescribed Displacement cannot be used with a Rigid Material node. Hence, the Prescribed Displacement/Rotation node (subnode to Rigid Material) is used to constrain or prescribe the corresponding degrees of freedom.
•
The connections set up in the model can be reviewed in the Joints Summary section at the physics node.
•
Both the geometry and mesh have been built using COMSOL Multiphysics. However, the meshed geometry is imported to simplify the modeling.
•
To recompute study-1 in the saved model, make the changes given at the end of the document.
Application Library path: Multibody_Dynamics_Module/Automotive_and_Aerospace/helicopter_swashplate
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>Multibody Dynamics (mbd).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies>Time Dependent.
6
Click  Done.
Import the meshed geometry of the helicopter swashplate mechanism to save modeling time.
Mesh 1
Import 1
1
In the Mesh toolbar, click  Import.
2
In the Settings window for Import, locate the Import section.
3
Click  Browse.
4
Browse to the model’s Application Libraries folder and double-click the file helicopter_swashplate.mphbin.
5
Click  Import.
Information
Click the  Zoom Extents button in the Graphics toolbar.
Define variables and functions to use when setting up the physics.
Global Definitions
Use ramp functions to specify the motion of the pushrods.
Ramp 1 (rm1)
1
In the Home toolbar, click  Functions and choose Global>Ramp.
2
In the Settings window for Ramp, locate the Parameters section.
3
In the Location text field, type 0.002[s].
4
Select the Cutoff check box. In the associated text field, type 0.05[s].
5
Click to expand the Smoothing section.
6
Select the Size of transition zone at start check box. In the associated text field, type 0.005.
7
Select the Size of transition zone at cutoff check box. In the associated text field, type 0.005.
Ramp 2 (rm2)
1
Right-click Ramp 1 (rm1) and choose Duplicate.
2
In the Settings window for Ramp, locate the Parameters section.
3
In the Location text field, type 0.004[s].
4
In the Cutoff text field, type 0.1[s].
5
Locate the Smoothing section. In the Size of transition zone at start text field, type 0.01.
6
In the Size of transition zone at cutoff text field, type 0.01.
Variables 1
1
In the Home toolbar, click  Variables and choose Global Variables.
2
In the Settings window for Variables, locate the Variables section.
3
In the table, enter the following settings:
Name
Expression
Unit
Description
vf
100[km/h]
m/s
Forward speed of helicopter
rpm
300
 
RPM of helicopter rotor
omega
2*pi*rpm/60[s]
1/s
Angular velocity of rotor
theta
omega*t[rad]
rad
Angular rotation of rotor
vp
0.5[m/s]
m/s
Speed of pushrod motion
up1
vp*rm1(t)
m
Motion of pushrod 1 and 3
up2
vp*rm2(t)
m
Motion of pushrod 2
Create selections to define the rotor blades. Either select any entity directly from the geometry or alternatively type entity number using the Paste Selection option.
Definitions
Blade1
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Blade1 in the Label text field.
3
Select Domains 1, 2, 4, 5, 8–10, and 12 only.
Blade2
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Blade2 in the Label text field.
3
Select Domains 17, 19–24, and 26 only.
Blade3
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Blade3 in the Label text field.
3
Select Domains 25, 29–33, 36, and 37 only.
Blades
1
In the Definitions toolbar, click  Union.
2
In the Settings window for Union, type Blades in the Label text field.
3
Locate the Input Entities section. Under Selections to add, click  Add.
4
In the Add dialog box, in the Selections to add list, choose Blade1, Blade2, and Blade3.
5
Click OK.
Without Blades
1
In the Definitions toolbar, click  Complement.
2
In the Settings window for Complement, type Without Blades in the Label text field.
3
Locate the Input Entities section. Under Selections to invert, click  Add.
4
In the Add dialog box, select Blade1 in the Selections to invert list.
5
Click OK.
Add Material
1
In the Home 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 Add to Component in the window toolbar.
5
In the Home toolbar, click  Add Material to close the Add Material window.
Multibody Dynamics (mbd)
Define the initial angular velocity at the physics node to use for the rotating parts of the mechanism to avoid transient effects.
1
In the Model Builder window, under Component 1 (comp1) click Multibody Dynamics (mbd).
2
In the Settings window for Multibody Dynamics, click to expand the Initial Values section.
3
Specify the ω vector as
0
x
0
y
omega
z
Rigid Material: Baseplate
1
In the Physics toolbar, click  Domains and choose Rigid Material.
2
In the Settings window for Rigid Material, type Rigid Material: Baseplate in the Label text field.
3
Select Domain 7 only.
Set the initial values of the nonrotating parts to zero locally.
4
Locate the Initial Values section. From the list, choose Locally defined.
Fixed Constraint 1
In the Physics toolbar, click  Attributes and choose Fixed Constraint.
Rigid Material: Pushrod1
1
In the Physics toolbar, click  Domains and choose Rigid Material.
2
In the Settings window for Rigid Material, type Rigid Material: Pushrod1 in the Label text field.
3
Select Domain 6 only.
4
Locate the Initial Values section. From the list, choose Locally defined.
Rigid Materials (Stationary)
Create all similar parts by duplicating the Rigid Material 2 node and changing the settings of the nodes according to the table below.
Name
Selection
Rigid Material: Pushrod2
13
Rigid Material: Pushrod3
35
Rigid Material: Baseplate-Swashplate Link1
27
Rigid Material: Baseplate-Swashplate Link2
28
Rigid Material: Lower Swashplate
3
Rigid Material: Rotor Hub
1
In the Physics toolbar, click  Domains and choose Rigid Material.
2
In the Settings window for Rigid Material, type Rigid Material: Rotor Hub in the Label text field.
3
Select Domain 14 only.
Prescribed Displacement/Rotation 1
1
In the Physics toolbar, click  Attributes and choose Prescribed Displacement/Rotation.
2
In the Settings window for Prescribed Displacement/Rotation, locate the Center of Rotation section.
3
From the list, choose User defined.
4
Locate the Prescribed Displacement at Center of Rotation section. Select the Prescribed in x direction check box.
5
Select the Prescribed in y direction check box.
6
Select the Prescribed in z direction check box.
7
Locate the Prescribed Rotation section. From the By list, choose Prescribed rotation.
8
Specify the Ω vector as
0
x
0
y
1
z
9
In the φ0 text field, type theta.
Rigid Material: Upper Swashplate
1
In the Physics toolbar, click  Domains and choose Rigid Material.
2
In the Settings window for Rigid Material, type Rigid Material: Upper Swashplate in the Label text field.
3
Select Domain 11 only.
Rigid Materials (Rotating)
Create all similar parts using the information given in the table:
Name
Selection
Rigid Material: Sphere
18
Rigid Material: Swashplate-Blade Link1
16
Rigid Material: Swashplate-Blade Link2
15
Rigid Material: Swashplate-Blade Link3
34
Rigid Material: Rotor Blade1
Blade 1
Rigid Material: Rotor Blade2
Blade 2
Rigid Material: Rotor Blade2
Blade 3
Create attachments to set up the connection for the case of flexible rotor blades.
Attachment: Swashplate-Blade1
1
In the Physics toolbar, click  Boundaries and choose Attachment.
2
In the Settings window for Attachment, type Attachment: Swashplate-Blade1 in the Label text field.
3
Select Boundaries 265, 266, 290, and 291 only.
Attachments
You can create more attachments using the information given in the table below.
Name
Selection
Attachment: Swashplate-Blade2
313, 314, 340, 341
Attachment: Swashplate-Blade3
687, 688, 695, 696
Attachment: Hub-Blade1
152, 153, 197, 198
Attachment: Hub-Blade2
414, 415, 445, 447
Attachment: Hub-Blade3
470, 471, 480, 482
After creating the different parts of the mechanism, establish connections between them using joint nodes.
Prismatic Joint 1
1
In the Physics toolbar, click  Global and choose Prismatic Joint.
2
In the Settings window for Prismatic Joint, locate the Attachment Selection section.
3
From the Source list, choose Rigid Material: Baseplate.
4
From the Destination list, choose Rigid Material: Pushrod1.
5
Locate the Center of Joint section. From the Entity level list, choose Point.
6
Locate the Axis of Joint section. Specify the e0 vector as
0
x
0
y
1
z
Center of Joint: Point 1
1
In the Model Builder window, click Center of Joint: Point 1.
2
Select Points 48 and 107 only.
Prismatic Joint 1
In the Model Builder window, click Prismatic Joint 1.
Prescribed Motion 1
1
In the Physics toolbar, click  Attributes and choose Prescribed Motion.
2
In the Settings window for Prescribed Motion, locate the Prescribed Translational Motion section.
3
In the up text field, type up1.
The Reduced Slot joint is used between the second pushrod and the baseplate to provide the tilting freedom to the swashplate assembly.
Reduced Slot Joint 1
1
In the Physics toolbar, click  Global and choose Reduced Slot Joint.
2
In the Settings window for Reduced Slot Joint, locate the Attachment Selection section.
3
From the Source list, choose Rigid Material: Baseplate.
4
From the Destination list, choose Rigid Material: Pushrod2.
5
Locate the Center of Joint section. From the Entity level list, choose Point.
6
Locate the Axes of Joint section. From the Joint translational axis list, choose Attached on source.
7
Specify the etr0 vector as
0
x
0
y
1
z
8
Specify the erot0 vector as
cos(pi/6)
x
sin(pi/6)
y
0
z
Center of Joint: Point 1
1
In the Model Builder window, click Center of Joint: Point 1.
2
Select Points 197, 248, 274, and 378 only.
Reduced Slot Joint 1
In the Model Builder window, click Reduced Slot Joint 1.
Prescribed Motion 1
1
In the Physics toolbar, click  Attributes and choose Prescribed Motion.
2
In the Settings window for Prescribed Motion, locate the Prescribed Translational Motion section.
3
In the up text field, type up2.
4
Locate the Prescribed Rotational Motion section. From the Activation condition list, choose Never active.
Prismatic Joint 2
1
In the Physics toolbar, click  Global and choose Prismatic Joint.
2
In the Settings window for Prismatic Joint, locate the Attachment Selection section.
3
From the Source list, choose Rigid Material: Baseplate.
4
From the Destination list, choose Rigid Material: Pushrod3.
5
Locate the Center of Joint section. From the Entity level list, choose Point.
6
Locate the Axis of Joint section. Specify the e0 vector as
0
x
0
y
1
z
Center of Joint: Point 1
1
In the Model Builder window, click Center of Joint: Point 1.
2
Select Points 1115 and 1219 only.
Prismatic Joint 2
In the Model Builder window, click Prismatic Joint 2.
Prescribed Motion 1
1
In the Physics toolbar, click  Attributes and choose Prescribed Motion.
2
In the Settings window for Prescribed Motion, locate the Prescribed Translational Motion section.
3
In the up text field, type up1.
Hinge Joint 1
1
In the Physics toolbar, click  Global and choose Hinge Joint.
2
In the Settings window for Hinge Joint, locate the Attachment Selection section.
3
From the Source list, choose Rigid Material: Baseplate.
4
From the Destination list, choose Rigid Material: Baseplate-Swashplate Link1.
5
Locate the Center of Joint section. From the Entity level list, choose Point.
6
Locate the Axis of Joint section. From the list, choose Select a parallel edge.
Center of Joint: Point 1
1
In the Model Builder window, click Center of Joint: Point 1.
2
Select Points 757, 774, 863, and 896 only.
Joint Axis 1
1
In the Model Builder window, click Joint Axis 1.
2
Select Edge 1236 only.
Hinge Joint 2
1
In the Physics toolbar, click  Global and choose Hinge Joint.
2
In the Settings window for Hinge Joint, locate the Attachment Selection section.
3
From the Source list, choose Rigid Material: Baseplate-Swashplate Link1.
4
From the Destination list, choose Rigid Material: Baseplate-Swashplate Link2.
5
Locate the Center of Joint section. From the Entity level list, choose Point.
6
Locate the Axis of Joint section. From the list, choose Select a parallel edge.
Center of Joint: Point 1
1
In the Model Builder window, click Center of Joint: Point 1.
2
Select Points 914, 930, 980, and 996 only.
Joint Axis 1
1
In the Model Builder window, click Joint Axis 1.
2
Select Edge 1509 only.
Ball Joint 1
1
In the Physics toolbar, click  Global and choose Ball Joint.
2
In the Settings window for Ball Joint, locate the Attachment Selection section.
3
From the Source list, choose Rigid Material: Pushrod1.
4
From the Destination list, choose Rigid Material: Lower Swashplate.
5
Locate the Center of Joint section. From the Entity level list, choose Point.
Center of Joint: Point 1
1
In the Model Builder window, click Center of Joint: Point 1.
2
Select Points 73 and 75 only.
Ball Joints
Create all similar connections by duplicating the above joint with the information given in the table below.
Name
Source
Destination
Center of Joint Selection (points)
Ball joint 2
Rigid Material: Pushrod 2
Rigid Material: Lower Swashplate
263, 265
Ball joint 3
Rigid Material: Pushrod 3
Rigid Material: Lower Swashplate
1062, 1240
Ball joint 4
Rigid Material: Baseplate-Swashplate Link2
Rigid Material: Lower Swashplate
798, 834
Ball joint 5
Rigid Material: Sphere
Rigid Material: Lower Swashplate
558, 723
Ball joint 6
Rigid Material: Upper Swashplate
Rigid Material: Swashplate-Blade Link1
337, 490
Ball joint 7
Rigid Material: Upper Swashplate
Rigid Material: Swashplate-Blade Link2
342, 491
Ball joint 8
Rigid Material: Upper Swashplate
Rigid Material: Swashplate-Blade Link3
993, 1208
Planar Joint 1
1
In the Physics toolbar, click  Global and choose Planar Joint.
2
In the Settings window for Planar Joint, locate the Attachment Selection section.
3
From the Source list, choose Rigid Material: Lower Swashplate.
4
From the Destination list, choose Rigid Material: Upper Swashplate.
5
Locate the Center of Joint section. From the list, choose User defined.
6
Locate the Axis of Joint section. Specify the e0 vector as
0
x
0
y
1
z
Cylindrical Joint 1
1
In the Physics toolbar, click  Global and choose Cylindrical Joint.
2
In the Settings window for Cylindrical Joint, locate the Attachment Selection section.
3
From the Source list, choose Rigid Material: Sphere.
4
From the Destination list, choose Rigid Material: Rotor Hub.
5
Locate the Center of Joint section. From the list, choose User defined.
6
Locate the Axis of Joint section. Specify the e0 vector as
0
x
0
y
1
z
Prescribed Motion 1
1
In the Physics toolbar, click  Attributes and choose Prescribed Motion.
2
In the Settings window for Prescribed Motion, locate the Prescribed Translational Motion section.
3
From the Activation condition list, choose Never active.
Hinge Joint 3
1
In the Physics toolbar, click  Global and choose Hinge Joint.
2
In the Settings window for Hinge Joint, locate the Attachment Selection section.
3
From the Source list, choose Rigid Material: Swashplate-Blade Link1.
4
From the Destination list, choose Attachment: Swashplate-Blade1.
5
Locate the Axis of Joint section. From the list, choose Select a parallel edge.
Joint Axis 1
1
In the Model Builder window, click Joint Axis 1.
2
Select Edge 551 only.
Hinge Joints
1
Create all similar connections by duplicating the above joint and using the information given in the table below.
Name
Source
Destination
Joint Axis (Edge)
Hinge Joint 4
Rigid Material: Swashplate-Blade Link2
Attachment: Swashplate-Blade2
660
Hinge Joint 5
Rigid Material: Swashplate-Blade Link3
Attachment: Swashplate-Blade3
1681
Hinge Joint 6
Rigid Material: Rotor Hub
Attachment: Hub-Blade1
535
Hinge Joint 7
Rigid Material: Rotor Hub
Attachment: Hub-Blade2:
1053
Hinge Joint 8
Rigid Material: Rotor Hub
Attachment: Hub-Blade3
1144
All connections are summarized in the Joints Summary section of the physics node.
Define the angle-of-attack of each rotor blade using joint variables.
Definitions
Variables 2
1
In the Home toolbar, click  Variables and choose Local Variables.
2
In the Settings window for Variables, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Domain.
4
From the Selection list, choose Blade1.
5
Locate the Variables section. In the table, enter the following settings:
Name
Expression
Unit
Description
alpha
-mbd.hgj6.th
rad
Angle of attack
Variables 3
1
In the Home toolbar, click  Variables and choose Local Variables.
2
In the Settings window for Variables, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Domain.
4
From the Selection list, choose Blade2.
5
Locate the Variables section. In the table, enter the following settings:
Name
Expression
Unit
Description
alpha
mbd.hgj7.th
rad
Angle of attack
Variables 4
1
In the Home toolbar, click  Variables and choose Local Variables.
2
In the Settings window for Variables, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Domain.
4
From the Selection list, choose Blade3.
5
Locate the Variables section. In the table, enter the following settings:
Name
Expression
Unit
Description
alpha
mbd.hgj8.th
rad
Angle of attack
Define nonlocal integration couplings to use for computing the total lift force on each rotor blade and the tip displacement of the second rotor blade.
Integration 1 (intop1)
1
In the Definitions toolbar, click  Nonlocal Couplings and choose Integration.
2
In the Settings window for Integration, locate the Source Selection section.
3
From the Geometric entity level list, choose Boundary.
4
Select Boundary 3 only.
5
Locate the Advanced section. From the Frame list, choose Material  (X, Y, Z).
Integration 2 (intop2)
1
Right-click Integration 1 (intop1) and choose Duplicate.
2
In the Settings window for Integration, locate the Source Selection section.
3
Click  Clear Selection.
4
Select Boundary 400 only.
Integration 3 (intop3)
1
Right-click Integration 2 (intop2) and choose Duplicate.
2
In the Settings window for Integration, locate the Source Selection section.
3
Click  Clear Selection.
4
Select Boundary 714 only.
Integration 4 (intop4)
1
Right-click Integration 3 (intop3) and choose Duplicate.
2
In the Settings window for Integration, locate the Source Selection section.
3
From the Geometric entity level list, choose Point.
4
Select Point 580 only.
Variables 5
1
In the Definitions toolbar, click  Local Variables.
2
In the Settings window for Variables, locate the Variables section.
3
In the table, enter the following settings:
Name
Expression
Unit
Description
d
sqrt(x^2+y^2)
m
Distance from the center
Ur
omega*d-vf*y/d
m/s
Relative velocity
CL
4*alpha
rad
Lift coefficient
FL
0.5*1[kg/m^3]*Ur^2*CL*sign(Ur)
Pa
Lift force
FL_tot1
intop1(FL)
N
Total lift force - blade1
FL_tot2
intop2(FL)
N
Total lift force - blade2
FL_tot3
intop3(FL)
N
Total lift force - blade3
alphaM
9.4[deg]
rad
Mean angle of attack
CL_alphaM
4*alphaM
rad
Mean lift coefficient
FL_tot1_alphaM
intop1(0.5*1[kg/m^3]*Ur^2*CL_alphaM*sign(Ur))
N
Total lift force (mean)- blade1
w_tip
intop4(w)
m
Tip displacement z direction
Apply the lift force on the rotor blades using a Boundary Load node.
Multibody Dynamics (mbd)
Boundary Load 1
1
In the Physics toolbar, click  Boundaries and choose Boundary Load.
2
Select Boundaries 3, 400, and 714 only.
3
In the Settings window for Boundary Load, locate the Force section.
4
Specify the FA vector as
0
x
0
y
FL
z
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(0,0.001,0.3).
4
In the Model Builder window, click Study 1.
5
In the Settings window for Study, type Study: Rigid Blades in the Label text field.
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, under Study: Rigid Blades>Solver Configurations>Solution 1 (sol1) click Time-Dependent Solver 1.
4
In the Settings window for Time-Dependent Solver, click to expand the Time Stepping section.
5
From the Steps taken by solver list, choose Intermediate.
6
In the Study toolbar, click  Compute.
Now you can add a new study for performing the transient analysis with flexible blades.
For viewing the motion of the blades with respect to a reference frame, use the option of defining a reference frame available in the Multibody Dynamics interface and plot the postprocessing variables with respect to the reference frame.
Multibody Dynamics (mbd)
1
In the Model Builder window, under Component 1 (comp1) click Multibody Dynamics (mbd).
2
In the Settings window for Multibody Dynamics, click to expand the Results section.
3
From the Body defining reference frame list, choose Attachment: Hub-Blade1.
Add Study
1
In the Study toolbar, click  Add Study to open the Add Study window.
2
Go to the Add Study window.
3
Find the Studies subsection. In the Select Study tree, select General Studies>Time Dependent.
4
Click Add Study in the window toolbar.
5
In the Study toolbar, click  Add Study to close the Add Study window.
Study 2
Step 1: Time Dependent
1
In the Settings window for Time Dependent, locate the Study Settings section.
2
In the Output times text field, type range(0,0.001,0.3).
3
Locate the Physics and Variables Selection section. Select the Modify model configuration for study step check box.
4
In the tree, select Component 1 (comp1)>Multibody Dynamics (mbd), Controls spatial frame>Rigid Material: Rotor Blade1, Component 1 (comp1)>Multibody Dynamics (mbd), Controls spatial frame>Rigid Material: Rotor Blade2, and Component 1 (comp1)>Multibody Dynamics (mbd), Controls spatial frame>Rigid Material: Rotor Blade3.
5
Right-click and choose Disable.
6
In the Model Builder window, click Study 2.
7
In the Settings window for Study, type Study: Flexible Blades in the Label text field.
8
Locate the Study Settings section. Clear the Generate default plots check box.
Solution 2 (sol2)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 2 (sol2) node.
3
In the Model Builder window, expand the Study: Flexible Blades>Solver Configurations>Solution 2 (sol2)>Time-Dependent Solver 1 node, then click Fully Coupled 1.
4
In the Settings window for Fully Coupled, click to expand the Method and Termination section.
5
From the Stabilization and acceleration list, choose Anderson acceleration.
6
In the Dimension of iteration space text field, type 5.
7
In the Mixing parameter text field, type 0.9.
8
In the Study toolbar, click  Compute.
Results
Displacement (mbd)
The default plots show the displacement and velocity profiles in the mechanism.
Follow the instructions to generate the velocity plot shown in Figure 4.
You can also adjust the view for better visualization and use it in the plot.
Velocity (mbd)
1
In the Model Builder window, click Velocity (mbd).
2
In the Settings window for 3D Plot Group, locate the Plot Settings section.
3
From the View list, choose New view.
4
In the Velocity (mbd) toolbar, click  Plot.
Create a new dataset to plot the deformation of the flexible rotor blades.
Study: Flexible Blades/Solution 2 (3) (sol2)
1
In the Model Builder window, expand the Results>Datasets node.
2
Right-click Results>Datasets>Study: Flexible Blades/Solution 2 (sol2) and choose Duplicate.
Selection
1
In the Results toolbar, click  Attributes and choose Selection.
2
In the Settings window for Selection, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Domain.
4
From the Selection list, choose Blade1.
Study: Flexible Blades/Solution 2 (4) (sol2)
In the Model Builder window, under Results>Datasets right-click Study: Flexible Blades/Solution 2 (3) (sol2) and choose Duplicate.
Selection
1
In the Model Builder window, expand the Study: Flexible Blades/Solution 2 (4) (sol2) node, then click Selection.
2
In the Settings window for Selection, locate the Geometric Entity Selection section.
3
Click  Clear Selection.
4
From the Selection list, choose Without Blades.
Follow the instructions to plot the deformation in the flexible blade as shown in Figure 9 and Figure 10.
Displacement: Flexible Blade1
1
In the Model Builder window, right-click Displacement (mbd) and choose Duplicate.
2
In the Settings window for 3D Plot Group, type Displacement: Flexible Blade1 in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study: Flexible Blades/Solution 2 (3) (sol2).
4
Locate the Plot Settings section. From the Frame list, choose Material  (X, Y, Z).
5
Click the  Zoom Extents button in the Graphics toolbar.
6
In the Displacement: Flexible Blade1 toolbar, click  Plot.
Increase the deformation scale factor for better visualization.
Surface
1
In the Model Builder window, expand the Displacement: Flexible Blade1 node, then click Surface.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type mbd.disp_ref.
Deformation
1
In the Model Builder window, expand the Surface node, then click Deformation.
2
In the Settings window for Deformation, locate the Expression section.
3
In the X component text field, type u_ref.
4
In the Y component text field, type v_ref.
5
In the Z component text field, type w_ref.
6
Locate the Scale section. In the Scale factor text field, type 50.
Displacement: Flexible Blade1
1
In the Model Builder window, under Results click Displacement: Flexible Blade1.
2
In the Settings window for 3D Plot Group, locate the Plot Settings section.
3
From the View list, choose New view.
4
Click the  Go to XY View button in the Graphics toolbar.
5
Click the  Zoom Extents button in the Graphics toolbar.
6
In the Displacement: Flexible Blade1 toolbar, click  Plot.
7
In the Model Builder window, click Displacement: Flexible Blade1.
8
From the View list, choose New view.
9
Click the  Go to YZ View button in the Graphics toolbar.
10
Click the  Zoom Extents button in the Graphics toolbar.
11
In the Displacement: Flexible Blade1 toolbar, click  Plot.
Follow the instructions below to generate the von Mises stress distribution shown in Figure 11.
Stress: Flexible Blade1
1
Right-click Displacement: Flexible Blade1 and choose Duplicate.
2
In the Settings window for 3D Plot Group, type Stress: Flexible Blade1 in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study: Flexible Blades/Solution 2 (2) (sol2).
4
Locate the Plot Settings section. From the View list, choose View 1.
5
From the Frame list, choose Spatial  (x, y, z).
Surface
1
In the Model Builder window, expand the Stress: Flexible Blade1 node, then click Surface.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Study: Flexible Blades/Solution 2 (3) (sol2).
4
From the Solution parameters list, choose From parent.
5
Locate the Expression section. In the Expression text field, type mbd.mises.
6
Click to expand the Range section. Select the Manual color range check box.
7
In the Minimum text field, type 0.
8
In the Maximum text field, type 3e7.
Deformation
1
In the Model Builder window, expand the Surface node, then click Deformation.
2
In the Settings window for Deformation, locate the Expression section.
3
In the X component text field, type u.
4
In the Y component text field, type v.
5
In the Z component text field, type w+10*w_ref.
6
Locate the Scale section. In the Scale factor text field, type 1.
Surface 2
1
In the Model Builder window, right-click Surface and choose Duplicate.
2
In the Settings window for Surface, locate the Data section.
3
From the Dataset list, choose Study: Flexible Blades/Solution 2 (4) (sol2).
4
Locate the Expression section. In the Expression text field, type dom.
5
Click to expand the Title section. From the Title type list, choose None.
6
Locate the Coloring and Style section. From the Coloring list, choose Uniform.
7
From the Color list, choose Gray.
Deformation
1
In the Model Builder window, expand the Surface 2 node, then click Deformation.
2
In the Settings window for Deformation, locate the Expression section.
3
In the Z component text field, type w.
4
Click the  Go to Default View button in the Graphics toolbar.
5
Click the  Zoom Extents button in the Graphics toolbar.
6
In the Stress: Flexible Blade1 toolbar, click  Plot.
To plot the angle of attack variation of rotor blades shown in Figure 5, follow the instructions below.
Angle of Attack
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Angle of Attack in the Label text field.
Global 1
1
Right-click Angle of Attack and choose Global.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
-mbd.hgj6.th
deg
Relative rotation
mbd.hgj7.th
deg
Relative rotation
mbd.hgj8.th
deg
Relative rotation
4
Locate the x-Axis Data section. From the Parameter list, choose Expression.
5
In the Expression text field, type theta*180/pi.
6
Click to expand the Coloring and Style section. From the Width list, choose 2.
7
Find the Line markers subsection. From the Marker list, choose Cycle.
8
From the Positioning list, choose Interpolated.
9
Click to expand the Legends section. From the Legends list, choose Manual.
10
In the table, enter the following settings:
Legends
Angle of attack: blade1
Angle of attack: blade2
Angle of attack: blade3
Angle of Attack
1
In the Model Builder window, click Angle of Attack.
2
In the Settings window for 1D Plot Group, locate the Plot Settings section.
3
Select the x-axis label check box. In the associated text field, type Angular rotation of rotor (deg).
4
Select the y-axis label check box. In the associated text field, type Angle of attack (deg).
5
Click to expand the Title section. From the Title type list, choose None.
6
In the Angle of Attack toolbar, click  Plot.
7
Locate the Axis section. Select the Manual axis limits check box.
8
In the y maximum text field, type 25.
9
In the Angle of Attack toolbar, click  Plot.
To plot the total lift force on the rotor blades shown in Figure 6, follow the instructions below.
Total Lift Force
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Total Lift Force in the Label text field.
3
Locate the Data section. From the Time selection list, choose Interpolated.
4
In the Times (s) text field, type range(0,0.003,0.3).
Global 1
1
Right-click Total Lift Force and choose Global.
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)>Definitions>Variables>FL_tot1 - Total lift force - blade1 - N.
3
Click Add Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1)>Definitions>Variables>FL_tot2 - Total lift force - blade2 - N.
4
Click Add Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1)>Definitions>Variables>FL_tot3 - Total lift force - blade3 - N.
5
Locate the x-Axis Data section. From the Parameter list, choose Expression.
6
In the Expression text field, type theta*180/pi.
7
Locate the Coloring and Style section. From the Width list, choose 2.
8
Find the Line markers subsection. From the Marker list, choose Cycle.
9
From the Positioning list, choose Interpolated.
Total Lift Force
1
In the Model Builder window, click Total Lift Force.
2
In the Settings window for 1D Plot Group, locate the Plot Settings section.
3
Select the x-axis label check box. In the associated text field, type Angular rotation of rotor (deg).
4
Select the y-axis label check box. In the associated text field, type Total lift force (N).
5
Locate the Title section. From the Title type list, choose None.
6
In the Total Lift Force toolbar, click  Plot.
Duplicate the above figure to generate the plot shown in Figure 7.
Total Lift Force: Blade1
1
Right-click Total Lift Force and choose Duplicate.
2
In the Settings window for 1D Plot Group, type Total Lift Force: Blade1 in the Label text field.
3
Locate the Data section. In the Times (s) text field, type range(0.1,0.003,0.3).
Global 1
1
In the Model Builder window, expand the Total Lift Force: Blade1 node, then 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)>Definitions>Variables>FL_tot1 - Total lift force - blade1 - N.
3
Click Add Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1)>Definitions>Variables>FL_tot1_alphaM - Total lift force (mean)- blade1 - N.
Total Lift Force: Blade1
1
In the Model Builder window, click Total Lift Force: Blade1.
2
In the Settings window for 1D Plot Group, locate the Plot Settings section.
3
In the y-axis label text field, type Total lift force on blade1 (N).
4
In the Total Lift Force: Blade1 toolbar, click  Plot.
5
Locate the Legend section. From the Position list, choose Upper left.
6
In the Total Lift Force: Blade1 toolbar, click  Plot.
Follow the instructions below to generate the tip displacement plot shown in Figure 8.
Tip Displacement
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Tip Displacement in the Label text field.
Global 1
1
Right-click Tip Displacement and choose Global.
2
In the Settings window for Global, locate the Data section.
3
From the Dataset list, choose Study: Rigid Blades/Solution 1 (sol1).
4
Click Replace Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1)>Definitions>Variables>w_tip - Tip displacement z direction - m.
5
Locate the y-Axis Data section. In the table, enter the following settings:
Expression
Unit
Description
w_tip
mm
Tip displacement z direction
6
Locate the x-Axis Data section. From the Parameter list, choose Expression.
7
In the Expression text field, type theta*180/pi.
8
Locate the Coloring and Style section. From the Width list, choose 2.
9
Find the Line markers subsection. From the Marker list, choose Cycle.
10
From the Positioning list, choose Interpolated.
11
Locate the Legends section. From the Legends list, choose Manual.
12
In the table, enter the following settings:
Legends
Tip disp. z direction (Rigid blades)
Global 2
1
Right-click Global 1 and choose Duplicate.
2
In the Settings window for Global, locate the Data section.
3
From the Dataset list, choose Study: Flexible Blades/Solution 2 (3) (sol2).
4
Locate the Legends section. In the table, enter the following settings:
Legends
Tip disp. z direction (Flexible blades)
Tip Displacement
1
In the Model Builder window, click Tip Displacement.
2
In the Settings window for 1D Plot Group, locate the Legend section.
3
From the Position list, choose Upper left.
4
Locate the Title section. From the Title type list, choose None.
5
Locate the Plot Settings section.
6
Select the x-axis label check box. In the associated text field, type Angular rotation of rotor (deg).
7
In the Tip Displacement toolbar, click  Plot.
Add a new study to perform an eigenfrequency analysis of this mechanism with flexible blades.
Add Study
1
In the Home toolbar, click  Add Study to open the Add Study window.
2
Go to the Add Study window.
3
Find the Studies subsection. In the Select Study tree, select General Studies>Eigenfrequency.
4
Click Add Study in the window toolbar.
5
In the Home toolbar, click  Add Study to close the Add Study window.
Study 3
Step 1: Eigenfrequency
1
In the Settings window for Eigenfrequency, locate the Study Settings section.
2
Select the Desired number of eigenfrequencies check box. In the associated text field, type 20.
3
Locate the Physics and Variables Selection section. Select the Modify model configuration for study step check box.
4
In the tree, select Component 1 (comp1)>Multibody Dynamics (mbd)>Rigid Material: Rotor Blade1, Component 1 (comp1)>Multibody Dynamics (mbd)>Rigid Material: Rotor Blade2, Component 1 (comp1)>Multibody Dynamics (mbd)>Rigid Material: Rotor Blade3, Component 1 (comp1)>Multibody Dynamics (mbd)>Prismatic Joint 1>Prescribed Motion 1, Component 1 (comp1)>Multibody Dynamics (mbd)>Reduced Slot Joint 1>Prescribed Motion 1, and Component 1 (comp1)>Multibody Dynamics (mbd)>Prismatic Joint 2>Prescribed Motion 1.
5
Right-click and choose Disable.
6
In the Model Builder window, click Study 3.
7
In the Settings window for Study, type Study: Flexible Blades[Eigenfrequency] in the Label text field.
8
In the Home toolbar, click  Compute.
Results
Mode Shape (mbd)
Follow the instructions below to generate the mode shapes shown in Figure 12 and Figure 13.
1
In the Settings window for 3D Plot Group, locate the Data section.
2
From the Eigenfrequency (Hz) list, choose 11.762.
3
In the Mode Shape (mbd) toolbar, click  Plot.
4
In the Model Builder window, expand the Mode Shape (mbd) node.
Deformation
1
In the Model Builder window, expand the Results>Mode Shape (mbd)>Surface node, then click Deformation.
2
In the Settings window for Deformation, locate the Scale section.
3
Select the Scale factor check box. In the associated text field, type 0.02.
Mode Shape (mbd)
1
In the Model Builder window, under Results click Mode Shape (mbd).
2
In the Mode Shape (mbd) toolbar, click  Plot.
3
In the Settings window for 3D Plot Group, locate the Data section.
4
From the Eigenfrequency (Hz) list, choose 181.43.
5
In the Mode Shape (mbd) toolbar, click  Plot.
Finally, generate an animation of the helicopter swashplate mechanism showing the displacement of all the components.
Animation 1
1
In the Results toolbar, click  Animation and choose Player.
2
In the Settings window for Animation, locate the Frames section.
3
In the Number of frames text field, type 50.
Animation 2
1
Right-click Animation 1 and choose Duplicate.
2
In the Settings window for Animation, locate the Scene section.
3
From the Subject list, choose Displacement: Flexible Blade1.
Animation 3
1
Right-click Animation 2 and choose Duplicate.
2
In the Settings window for Animation, locate the Scene section.
3
From the Subject list, choose Stress: Flexible Blade1.