PDF
Reciprocating Engine with Hydrodynamic Bearings
Introduction
Fluid film bearings in an assembly should be designed to support the static and dynamic loads transferred to the foundation without metal to metal contact between journals and bushings. In a reciprocating engine it becomes more challenging due to the variation of the pressure in the cylinder during a cycle. As a result, reaction forces on the foundation vary throughout the cycle with the maximum value at the time of combustion of the fuel- air mixture in the cylinder. A single cylinder reciprocating engine supported on two hydrodynamic bearings is analyzed in this example.
The engine assembly is modeled using the Multibody Dynamics interface in the Multibody Dynamics Module, and the bearings are modeled using the Hydrodynamic Bearing interface in the Rotordynamics Module. The Solid-Bearing Coupling multiphysics coupling is used to combine the two interfaces.
A starting torque is first applied on the crankshaft to bring the engine up to the required speed. Then, a loading torque is switched on. After the startup, the engine runs on its own, driven by the cylinder pressure, which is a function of the crankshaft rotation. The crankshaft and foundation in the assembly are treated as elastic bodies, keeping other components rigid. The relative deformation of the crankshaft journal and the foundation is important for determining the accurate pressure distribution in the bearings.
The stress in the crankshaft and foundation is analyzed during the engine operation. Pressure distribution in the bearings and their reactions is an important performance indicator and is studied for a cycle of the engine operation. Some other results include engine speed variation, generated power, brake horse power, and the orbits of the crankshaft in the bearings.
Model Definition
The assembly of the single cylinder reciprocating engine is shown in Figure 1.
Figure 1: Reciprocating engine geometry.
The engine assembly consists of a crankshaft, a flywheel, a cylinder, a piston, and a connecting rod.
•
The cylinder is connected to the piston through a prismatic joint.
•
The piston is connected to the top end of the connecting rod through a hinge joint.
•
The bottom end of the connecting rod is connected to the crankshaft through a hinge joint.
•
The flywheel is mounted on the crankshaft, and this crankshaft-flywheel assembly is supported by journal bearings at both ends.
All components of the engine are assumed to be rigid, except the crankshaft and the foundation. All the components in the assembly are made up of structural steel.
The cylinder is fixed, while the other components are free to move in space. The pressure data for a cycle is available as a function of the crankshaft rotation. It is applied on the top surface of the piston, with a phase difference corresponding to the initial crank orientation. A starting torque of 100 Nm is applied on the crankshaft during the first crankshaft revolution to start the engine. For the first one and a half revolutions of the crankshaft, the engine runs with a no-load condition. After that, an external load proportional to the angular velocity of the crankshaft is applied. Due to this external load, the RPM of the engine slowly reaches a steady-state value.
Initially, during the startup, the angular speed of the crankshaft is small. At this speed, the pressure generated in the bearings will not be enough to support the forces from the connecting rod on the crankshaft. Elastic hinge joints between the crankshaft and foundation, corresponding to the bearings, are used to support the crankshaft initially. The joint stiffness is slowly brought down to zero as the engine picks-up speed. After this, the hydrodynamic bearings will be able to support the load transferred to the foundation.
Results and Discussion
Displacement profile of the engine is shown in Figure 2.
Figure 2: Displacement profile of the engine. Pressure load is shown in red arrows.
Figure 3 shows a plot of the stress profile in the crankshaft at t = 0.12 s. The maximum stress occurs in the crank due to the bending of the crankshaft.
Figure 3: Stress in the crankshaft.
The pressure profile in the bearings at t = 0.12 s is shown in Figure 4. The skewed pressure distribution in the bearings due to the bending of the shaft is clearly visible.
Figure 4: Pressure in the bearings.
Figure 5 shows the stress distribution in the foundation at t = 0.12 s. The maximum stress occurs at the bolt locations and the rear portion of the bearing housings.
Figure 5: Stress in foundation.
The time history of the angular speed of the crankshaft is shown in Figure 6. The starting torque applied in the beginning of the simulation increases the engine speed rapidly. After the removal of the starting torque, the speed increases steadily as there is no external load. Finally, after the application of the external load, the speed approaches a steady-state value close to 3000 rpm.
Figure 6: Crankshaft speed.
The engine angular speed fluctuates due the different strokes in a cycle, namely, compression stroke, combustion, and power stroke. During the power stroke, the piston is pushed to accelerate the crankshaft whereas during the compression stroke, the air-fuel mixture in the cylinder is compressed by the inertia of the components. These fluctuations are large in the single cylinder engine, but can be suppressed by using either a multiple cylinders engine or by using a larger flywheel. The flywheel absorbs the energy during the power stroke as kinetic energy and delivers it during the compression stroke, thus reducing the fluctuations in the engine speed. However, the disadvantage of a large flywheel is the need of a high starting torque and reduced power to weight ratio of the engine.
Figure 7 shows the reactions of the bearings against the load on the piston due to gas pressure. Initially, the reaction force is shared between the hydrodynamic bearing and the elastic joints. At this stage, bearing reactions are small and most of the load is carried by the elastic joints. Subsequently, the elastic stiffness of the joints is reduced linearly to zero. During this time, the share of the load carried by the bearing slowly increases and finally the total load is carried by the bearing itself. Assuming that the crank radius is small when compared to the length of the connecting rod, the force on the crankshaft from the connecting rod will be approximately be equal to the load on the piston. This load is also plotted for comparison.
Figure 7: Bearing reactions and piston load.
Different torques acting on the crankshaft are shown in Figure 8. The starting torque of 100 Nm acts on the crankshaft until the crankshaft completes the first revolution. For the next half revolution, there is no load on the engine, and it accelerates on its own driven by the cylinder pressure. A speed proportional torque is switched on after the crankshaft completes one and half revolutions.
The torque on the crankshaft due to the load from the connecting rod is computed approximately by assuming that the force on the crank is equal to the force on the piston and that the crank arm for the torque is rcsin(θ). Here, θ is the angular position of the crankshaft relative to the bottom dead center and rc is the crank radius. During the power stroke, the torque on the crankshaft is positive whereas during the compression stroke it becomes negative and the engine consumes power from the flywheel.
Figure 8: Torque on the crankshaft.
The mechanical power generated by the gas pressure is displayed in Figure 9. During the compression stroke, the power generated is negative and suddenly reverts its sign during the combustion, after which the power generated is positive. The time average of the power over a cycle is the net mechanical power generated in one revolution of the crankshaft.
Figure 9: Power generated by gas pressure.
The power output due to the applied external torque is shown in Figure 10. It shows that the engine initially runs with a no-load condition. Once an external torque is applied, the power output of the engine (BHP) varies with a mean value close to 6.5 bhp.
Figure 10: Brake horse power.
The orbit of the journal in the left bearing is shown in Figure 11. Due to intermittent contact in the bearings and the dynamic nature of the loading, the journal orbit is quite random.
Figure 11: Journal orbit.
The relative eccentricity of the same journal in the bearing is shown in Figure 12. Within a cycle, two peaks are observed. One corresponding to the peak pressure in the power stroke and the other corresponding to the horizontal motion during the compression stroke.
Figure 12: Relative eccentricity of left journal.
Notes About the COMSOL Implementation
•
A Solid-Bearing Coupling multiphysics coupling is used to combine the engine-bearing assembly. The Hydrodynamic Journal Bearing in the Hydrodynamic Bearing physics interface is used to model the thin fluid film flow in the journal bearing. You need one such node per bearing.
•
A hydrodynamic bearing can support the load only when the journal is running at a finite speed. In this model, the engine is started using an external torque on the crankshaft. Therefore, in the beginning the speed of the crankshaft is small and the bearings cannot support the load on the crankshaft from the connecting rod. A Hinge Joint with joint elasticity is used to support the crankshaft in the beginning. The elastic stiffness is slowly decreased to zero after the engine startup.
•
The Applied Moment subnode of the Rigid Connector is used to apply the starting and loading torque. Step functions are used to switch the two torques.
Application Library path: Multibody_Dynamics_Module/Automotive_and_Aerospace/single_cylinder_reciprocating_engine
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
In the Select Physics tree, select Structural Mechanics>Rotordynamics>Hydrodynamic Bearing (hdb).
5
Click Add.
6
Click  Study.
7
In the Select Study tree, select General Studies>Time Dependent.
8
Click  Done.
Geometry 1
Import 1 (imp1)
1
In the Home 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 single_cylinder_reciprocating_engine.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 Home toolbar, click  Build All.
Start by creating the parameters for the model.
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
C
2e-5[m]
2E-5 m
Bearing clearance
mu0
0.072[Pa*s]
0.072 Pa·s
Lubricant viscosity
t1
0.025[s]
0.025 s
Stiffness reduction start
t2
0.04[s]
0.04 s
Stiffness reduction end
kb
1e9[N/m]
1E9 N/m
Bearing stiffness
theta0
240[deg]
4.1888 rad
Initial rotation of crank
For automatic generation of hinge and prismatic joints between different parts, group the identity boundary pairs.
Definitions
In the Model Builder window, expand the Component 1 (comp1)>Definitions node.
Identity Boundary Pair 1 (ap1), Identity Boundary Pair 2 (ap2), Identity Boundary Pair 3 (ap3), Identity Boundary Pair 5 (ap5)
1
In the Model Builder window, under Component 1 (comp1)>Definitions, Ctrl-click to select Identity Boundary Pair 1 (ap1), Identity Boundary Pair 2 (ap2), Identity Boundary Pair 3 (ap3), and Identity Boundary Pair 5 (ap5).
2
Right-click and choose Group.
Hinge Joint Pairs
In the Settings window for Group, type Hinge Joint Pairs in the Label text field.
Prismatic Joint Pair
1
In the Model Builder window, under Component 1 (comp1)>Definitions click Identity Boundary Pair 4 (ap4).
2
In the Settings window for Pair, type Prismatic Joint Pair in the Label text field.
3
Right-click Prismatic Joint Pair and choose Disable.
Define some selections for later use.
Identity Boundary Pair 1 (ap1)
1
In the Model Builder window, under Component 1 (comp1)>Definitions>Hinge Joint Pairs click Identity Boundary Pair 1 (ap1).
2
In the Settings window for Pair, locate the Source Boundaries section.
3
Click  Create Selection.
4
In the Create Selection dialog box, type Journal 1 in the Selection name text field.
5
Click OK.
6
In the Settings window for Pair, locate the Destination Boundaries section.
7
Click  Create Selection.
8
In the Create Selection dialog box, type Foundation 1 in the Selection name text field.
9
Click OK.
Identity Boundary Pair 3 (ap3)
1
In the Model Builder window, click Identity Boundary Pair 3 (ap3).
2
In the Settings window for Pair, locate the Source Boundaries section.
3
Click  Create Selection.
4
In the Create Selection dialog box, type Journal 2 in the Selection name text field.
5
Click OK.
6
In the Settings window for Pair, locate the Destination Boundaries section.
7
Click  Create Selection.
8
In the Create Selection dialog box, type Foundation 2 in the Selection name text field.
9
Click OK.
Piston top
1
In the Definitions toolbar, click  Cylinder.
2
In the Settings window for Cylinder, type Piston top in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Boundary.
4
Locate the Size and Shape section. In the Outer radius text field, type 0.042.
5
In the Top distance text field, type 0.208.
6
In the Bottom distance text field, type 0.196.
7
Locate the Output Entities section. From the Include entity if list, choose Entity inside cylinder.
Hide the connecting rod and foundations to make the selection easier.
8
Click the  Click and Hide button in the Graphics toolbar.
9
In the Graphics window toolbar, clicknext to  Select Boundaries, then choose Select Domains.
10
Select Domain 6 only.
11
Select Domain 8 only.
12
Select Domain 9 only.
13
In the Graphics window toolbar, clicknext to  View Unhidden, then choose View Hidden Only.
Journals
1
In the Definitions toolbar, click  Union.
2
In the Settings window for Union, type Journals in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Boundary.
4
Locate the Input Entities section. Under Selections to add, click  Add.
5
In the Add dialog box, in the Selections to add list, choose Journal 1 and Journal 2.
6
Click OK.
Foundations
1
Right-click Journals and choose Duplicate.
2
In the Settings window for Union, type Foundations in the Label text field.
3
Locate the Input Entities section. In the Selections to add list, select Journal 1.
4
Under Selections to add, click  Delete.
5
Under Selections to add, click  Delete.
6
Under Selections to add, click  Add.
7
In the Add dialog box, in the Selections to add list, choose Foundation 1 and Foundation 2.
8
Click OK.
Bearing System
1
Right-click Foundations and choose Duplicate.
2
In the Settings window for Union, type Bearing System in the Label text field.
3
Locate the Input Entities section. In the Selections to add list, select Foundation 1.
4
Under Selections to add, click  Delete.
5
Under Selections to add, click  Delete.
6
Under Selections to add, click  Add.
7
In the Add dialog box, in the Selections to add list, choose Journals and Foundations.
8
Click OK.
Fixed 1
1
In the Definitions toolbar, click  Cylinder.
2
In the Settings window for Cylinder, type Fixed 1 in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Boundary.
4
Locate the Size and Shape section. In the Outer radius text field, type 0.006.
5
Locate the Position section. In the x text field, type -0.035.
6
In the y text field, type -0.0514.
7
Locate the Output Entities section. From the Include entity if list, choose Entity inside cylinder.
Fixed 2
1
Right-click Fixed 1 and choose Duplicate.
2
In the Settings window for Cylinder, type Fixed 2 in the Label text field.
3
Locate the Position section. In the y text field, type 0.0514.
Fixed 3
1
Right-click Fixed 2 and choose Duplicate.
2
In the Settings window for Cylinder, type Fixed 3 in the Label text field.
3
Locate the Position section. In the x text field, type 0.035.
Fixed 4
1
Right-click Fixed 3 and choose Duplicate.
2
In the Settings window for Cylinder, type Fixed 4 in the Label text field.
3
Locate the Position section. In the y text field, type -0.0514.
Fixed
1
In the Definitions toolbar, click  Union.
2
In the Settings window for Union, type Fixed in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Boundary.
4
Locate the Input Entities section. Under Selections to add, click  Add.
5
In the Add dialog box, in the Selections to add list, choose Fixed 1, Fixed 2, Fixed 3, and Fixed 4.
6
Click OK.
Define the integration operator on the piston’s top surface to compute the projected area of the piston.
Integration over piston top
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
From the Selection list, choose Piston top.
5
Locate the Advanced section. From the Frame list, choose Material  (X, Y, Z).
6
In the Label text field, type Integration over piston top.
Define the step functions for switching the loading and starting torques.
Step: Loading Torque Start
1
In the Definitions toolbar, click  More Functions and choose Step.
2
In the Settings window for Step, locate the Parameters section.
3
In the Location text field, type 3*pi.
4
Click to expand the Smoothing section. In the Size of transition zone text field, type pi/18.
5
In the Label text field, type Step: Loading Torque Start.
Step: Starting Torque Cutoff
1
Right-click Step: Loading Torque Start and choose Duplicate.
2
In the Settings window for Step, type Step: Starting Torque Cutoff in the Label text field.
3
Locate the Parameters section. In the Location text field, type 2*pi.
4
In the From text field, type 1.
5
In the To text field, type 0.
6
Locate the Smoothing section. In the Size of transition zone text field, type pi/36.
Import the cylinder pressure data from the file. This data can also be computed using a thermodynamics analysis. See the Reciprocating Engine model in the Multibody Dynamics Module for the details of the thermodynamic analysis.
Interpolation: pressure
1
In the Definitions toolbar, click  Interpolation.
2
In the Settings window for Interpolation, locate the Definition section.
3
In the Function name text field, type pressure.
4
In the Label text field, type Interpolation: pressure.
5
Locate the Definition section. Click  Load from File.
6
Browse to the model’s Application Libraries folder and double-click the file single_cylinder_reciprocating_engine_pressure_data.txt.
7
Locate the Units section. In the Argument table, enter the following settings:
Argument
Unit
t
rad
8
In the Function table, enter the following settings:
Function
Unit
pressure
bar
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)
Rigid Domain: Cylinder
1
In the Model Builder window, under Component 1 (comp1) right-click Multibody Dynamics (mbd) and choose Material Models>Rigid Domain.
2
In the Settings window for Rigid Domain, in the Graphics window toolbar, clicknext to  View Unhidden, then choose View All.
3
Select Domains 2–5 only.
4
In the Label text field, type Rigid Domain: Cylinder.
Fixed Constraint 1
In the Physics toolbar, click  Attributes and choose Fixed Constraint.
Rigid Domain: Piston
1
In the Physics toolbar, click  Domains and choose Rigid Domain.
2
Select Domain 7 only.
3
In the Settings window for Rigid Domain, type Rigid Domain: Piston in the Label text field.
Rigid Domain: Connecting Rod
1
In the Physics toolbar, click  Domains and choose Rigid Domain.
2
Select Domain 8 only.
3
In the Settings window for Rigid Domain, type Rigid Domain: Connecting Rod in the Label text field.
Joints between different components of engine can be created automatically from <l>Automated Model Setup</l> section of Multibody Dynamics node. For creating <l>Hinge Joint</l> nodes between cylindrical boundaries, use <l>Hinge Joint Pairs</l>.
4
In the Model Builder window, click Multibody Dynamics (mbd).
5
In the Settings window for Multibody Dynamics, locate the Automated Model Setup section.
6
Find the Joint types subsection. From the Planar boundaries list, choose None.
7
From the Spherical boundaries list, choose None.
8
Click Physics Node Generation in the upper-right corner of the Automated Model Setup section. From the menu, choose Create Joints.
Attachment: Journal 1
1
In the Model Builder window, expand the Hinge Joints node, then click Attachment 1.
2
In the Settings window for Attachment, type Attachment: Journal 1 in the Label text field.
Attachment: Foundation 1
1
In the Model Builder window, under Component 1 (comp1)>Multibody Dynamics (mbd)>Hinge Joints click Attachment 2.
2
In the Settings window for Attachment, type Attachment: Foundation 1 in the Label text field.
Joints between the crankshaft journals and the foundations are usually not needed if the bearings are modeled explicitly. In this analysis, however, crankshaft speed is small during the startup and the bearings will not generate enough pressure to support the load from the connecting rod. Create elastic hinge joints with a finite stiffness which is slowly decreased to zero once the engine starts.
Hinge Joint 1
1
In the Model Builder window, click Hinge Joint 1.
2
In the Settings window for Hinge Joint, locate the Joint Elasticity section.
3
From the list, choose Elastic joint.
Joint Elasticity 1
1
In the Model Builder window, click Joint Elasticity 1.
2
In the Settings window for Joint Elasticity, locate the Spring section.
3
In the ku text field, type kb*(1-(t-t1)/(t2-t1)*(t>t1))*(t<=t2).
Attachment: Crankpin
1
In the Model Builder window, under Component 1 (comp1)>Multibody Dynamics (mbd)>Hinge Joints click Attachment 3.
2
In the Settings window for Attachment, type Attachment: Crankpin in the Label text field.
Attachment: Journal 2
1
In the Model Builder window, under Component 1 (comp1)>Multibody Dynamics (mbd)>Hinge Joints click Attachment 4.
2
In the Settings window for Attachment, type Attachment: Journal 2 in the Label text field.
Attachment: Foundation 2
1
In the Model Builder window, under Component 1 (comp1)>Multibody Dynamics (mbd)>Hinge Joints click Attachment 5.
2
In the Settings window for Attachment, type Attachment: Foundation 2 in the Label text field.
Hinge Joint 3
1
In the Model Builder window, click Hinge Joint 3.
2
In the Settings window for Hinge Joint, locate the Joint Elasticity section.
3
From the list, choose Elastic joint.
Joint Elasticity 1
1
In the Model Builder window, click Joint Elasticity 1.
2
In the Settings window for Joint Elasticity, locate the Spring section.
3
In the ku text field, type kb*(1-(t-t1)/(t2-t1)*(t>t1))*(t<=t2).
For automatically creating <l>Prismatic Joint</l> nodes between cylindrical boundaries, use <l>Prismatic Joint Pair</l>.
Definitions
Hinge Joint Pairs
In the Model Builder window, under Component 1 (comp1)>Definitions right-click Hinge Joint Pairs and choose Disable.
Prismatic Joint Pair (ap4)
In the Model Builder window, right-click Prismatic Joint Pair (ap4) and choose Enable.
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, locate the Automated Model Setup section.
3
Find the Joint types subsection. From the Cylindrical boundaries list, choose Prismatic joint.
4
Click Physics Node Generation in the upper-right corner of the Automated Model Setup section. From the menu, choose Create Joints.
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.
Define some variables for setting up the model and postprocessing.
Definitions
Variables 1
1
In the Model Builder window, under Component 1 (comp1) right-click Definitions and choose Variables.
2
In the Settings window for Variables, locate the Variables section.
3
In the table, enter the following settings:
Name
Expression
Unit
Description
theta
abs(mbd.hgj1.th)
rad
Shaft rotation
p
pressure(mod(theta+theta0,2*pi))
Pa
Cylinder pressure
Ti
100[N*m]*step2(theta)
N·m
Starting torque
To
0.05[N*m*s/rad]*d(theta,t)*step1(theta)
N·m
Output torque
A
intop1(root.nZ)
m²
Projected area of piston
P
-p*A*mbd.prj1.u_t/746[W]
 
Power generated
BHP
To*d(theta,t)/746[W]
rad
Brake horse power
Multibody Dynamics (mbd)
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 Piston top.
4
Locate the Force section. From the Load type list, choose Pressure.
5
In the p text field, type p.
Use the <l>Rigid Connector</l> feature to apply the starting and loading torque on the crankshaft.
Rigid Connector 1
1
In the Physics toolbar, click  Boundaries and choose Rigid Connector.
2
In the Settings window for Rigid Connector, in the Graphics window toolbar, clicknext to  View Unhidden, then choose View Unhidden.
3
Select Boundary 78 only.
Applied Moment 1
1
In the Physics toolbar, click  Attributes and choose Applied Moment.
2
In the Settings window for Applied Moment, locate the Applied Moment section.
3
Specify the M vector as
Ti
x
0
y
0
z
Applied Moment 2
1
Right-click Applied Moment 1 and choose Duplicate.
2
In the Settings window for Applied Moment, locate the Applied Moment section.
3
Specify the M vector as
-To
x
0
y
0
z
Define a reference frame attached to <l>Journal 1</l> to be used in postprocessing.
4
In the Model Builder window, click Multibody Dynamics (mbd).
5
In the Settings window for Multibody Dynamics, click to expand the Results section.
6
From the Body defining reference frame list, choose Attachment: Journal 1.
Hydrodynamic Bearing (hdb)
1
In the Model Builder window, under Component 1 (comp1) click Hydrodynamic Bearing (hdb).
2
In the Settings window for Hydrodynamic Bearing, locate the Boundary Selection section.
3
From the Selection list, choose Journals.
4
Click the  Show More Options button in the Model Builder toolbar.
5
In the Show More Options dialog box, in the tree, select the check box for the node Physics>Advanced Physics Options.
6
Click OK.
7
In the Settings window for Hydrodynamic Bearing, click to expand the Cavitation section.
8
Select the Cavitation check box.
Hydrodynamic Journal Bearing 1
1
In the Model Builder window, under Component 1 (comp1)>Hydrodynamic Bearing (hdb) click Hydrodynamic Journal Bearing 1.
2
In the Settings window for Hydrodynamic Journal Bearing, locate the Bearing Properties section.
3
In the C text field, type C.
4
Locate the Fluid Properties section. From the μ list, choose User defined. In the associated text field, type mu0.
5
In the ρc text field, type 866[kg/m^3].
Hydrodynamic Journal Bearing 2
1
Right-click Component 1 (comp1)>Hydrodynamic Bearing (hdb)>Hydrodynamic Journal Bearing 1 and choose Duplicate.
2
In the Settings window for Hydrodynamic Journal Bearing, locate the Boundary Selection section.
3
From the Selection list, choose Journal 2.
Multiphysics
Solid-Bearing Coupling 1 (sbco1)
1
In the Physics toolbar, click  Multiphysics Couplings and choose Boundary>Solid-Bearing Coupling.
2
In the Settings window for Solid-Bearing Coupling, locate the Boundary Selection section.
3
From the Selection list, choose Journal 1.
4
Locate the Foundation section. Select the Include foundation check box.
5
Locate the Foundation Selection section. From the Selection list, choose Foundation 1.
Solid-Bearing Coupling 2 (sbco2)
1
Right-click Solid-Bearing Coupling 1 (sbco1) and choose Duplicate.
2
In the Settings window for Solid-Bearing Coupling, locate the Boundary Selection section.
3
From the Selection list, choose Journal 2.
4
Locate the Foundation Selection section. From the Selection list, choose Foundation 2.
Define a selection for exterior bearing edges to be used in the mesh.
Hydrodynamic Bearing (hdb)
Border 1
1
In the Model Builder window, under Component 1 (comp1)>Hydrodynamic Bearing (hdb) click Border 1.
2
In the Settings window for Border, locate the Edge Selection section.
3
Click  Create Selection.
4
In the Create Selection dialog box, type Bearing Exterior Edges in the Selection name text field.
5
Click OK.
Definitions
Foundation Exterior Edges
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, locate the Input Entities section.
3
From the Geometric entity level list, choose Edge.
4
Select Edges 314 and 666 only.
5
Select the Group by continuous tangent check box.
6
In the Label text field, type Foundation Exterior Edges.
Bearing System Exterior Edges
1
In the Definitions toolbar, click  Union.
2
In the Settings window for Union, locate the Geometric Entity Level section.
3
From the Level list, choose Edge.
4
Locate the Input Entities section. Under Selections to add, click  Add.
5
In the Add dialog box, in the Selections to add list, choose Bearing Exterior Edges and Foundation Exterior Edges.
6
Click OK.
7
In the Settings window for Union, type Bearing System Exterior Edges in the Label text field.
Use a mapped mesh with appropriate distribution on the journal and foundation surfaces to capture the pressure distribution in the bearings.
Mesh 1
Mapped 1
1
In the Mesh toolbar, click  Boundary and choose Mapped.
2
In the Settings window for Mapped, locate the Boundary Selection section.
3
From the Selection list, choose Bearing System.
Distribution 1
1
Right-click Mapped 1 and choose Distribution.
2
Select Edges 39 and 151 only.
3
In the Settings window for Distribution, in the Graphics window toolbar, clicknext to  View Unhidden, then choose View Hidden Only.
4
Select Edges 39, 151, 321, and 631 only.
5
Locate the Distribution section. In the Number of elements text field, type 10.
Distribution 2
1
In the Model Builder window, right-click Mapped 1 and choose Distribution.
2
In the Settings window for Distribution, locate the Edge Selection section.
3
From the Selection list, choose Bearing System Exterior Edges.
4
Locate the Distribution section. In the Number of elements text field, type 12.
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
In the Graphics window toolbar, clicknext to  View Unhidden, then choose View Unhidden.
5
Select Domains 2–5 only.
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 Domain.
4
Select Domain 8 only.
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 Finer.
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(0,5e-5,0.12).
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 1 (sol1) node, then click Time-Dependent Solver 1.
3
In the Settings window for Time-Dependent Solver, click to expand the Time Stepping section.
4
From the Steps taken by solver list, choose Intermediate.
5
In the Model Builder window, expand the Study 1>Solver Configurations>Solution 1 (sol1)>Time-Dependent Solver 1 node, then click Fully Coupled 1.
6
In the Settings window for Fully Coupled, click to expand the Method and Termination section.
7
From the Jacobian update list, choose Once per time step.
8
In the Maximum number of iterations text field, type 10.
9
From the Termination criterion list, choose Solution or residual.
10
In the Study toolbar, click  Compute.
Results
Displacement (mbd)
Displacement and velocity are the default plots from the Multibody Dynamics interface. Make the following changes in the displacement plot to reproduce the plot shown in Figure 2.
Study 1/Solution 1: Cylinder
1
In the Model Builder window, expand the Results>Datasets node.
2
Right-click Results>Datasets>Study 1/Solution 1 (sol1) and choose Duplicate.
3
In the Settings window for Solution, type Study 1/Solution 1: Cylinder in the Label text field.
Selection
1
In the Results toolbar, click  Attributes and choose Selection.
2
In the Settings window for Selection, in the Graphics window toolbar, clicknext to  View Unhidden, then choose View Unhidden.
3
Locate the Geometric Entity Selection section. From the Geometric entity level list, choose Domain.
4
Select Domains 2–5 only.
Study 1/Solution 1: Engine without cylinder
1
In the Model Builder window, under Results>Datasets right-click Study 1/Solution 1: Cylinder (sol1) and choose Duplicate.
2
In the Model Builder window, click Study 1/Solution 1: Cylinder 1 (sol1).
3
In the Settings window for Solution, type Study 1/Solution 1: Engine without cylinder in the Label text field.
Selection
1
In the Model Builder window, click Selection.
2
In the Settings window for Selection, locate the Geometric Entity Selection section.
3
Click  Clear Selection.
4
Select Domains 1 and 6–9 only.
Displacement (mbd)
1
In the Model Builder window, under Results click Displacement (mbd).
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Dataset list, choose Study 1/Solution 1: Engine without cylinder (sol1).
Surface 2
1
In the Model Builder window, expand the Displacement (mbd) node.
2
Right-click Surface and choose Duplicate.
3
In the Model Builder window, click Surface 2.
4
In the Settings window for Surface, locate the Data section.
5
From the Dataset list, choose Study 1/Solution 1: Cylinder (sol1).
6
From the Solution parameters list, choose From parent.
Transparency 1
Right-click Surface 2 and choose Transparency.
Material Appearance 1
1
In the Model Builder window, right-click Surface 2 and choose Material Appearance.
2
In the Settings window for Material Appearance, locate the Appearance section.
3
Clear the Use the material’s selection check box.
Applied Loads (mbd)
In the Model Builder window, expand the Results>Applied Loads (mbd) node.
Boundary Load 1
1
In the Model Builder window, expand the Results>Applied Loads (mbd)>Boundary Loads (mbd) node.
2
Right-click Boundary Load 1 and choose Copy.
Boundary Load 1
In the Model Builder window, right-click Displacement (mbd) and choose Paste Arrow Surface.
Displacement (mbd)
1
In the Settings window for 3D Plot Group, locate the Color Legend section.
2
From the Position list, choose Right double.
3
Click the  Zoom Extents button in the Graphics toolbar.
4
Click the  Go to Default View button in the Graphics toolbar.
5
In the Displacement (mbd) toolbar, click  Plot.
Pressure is the default plot from the Hydrodynamic Bearing interface. Make the following changes to reproduce the plot shown in Figure 4.
Study 1/Solution 1: Bearing
1
In the Model Builder window, under Results>Datasets right-click Study 1/Solution 1 (sol1) and choose Duplicate.
2
In the Settings window for Solution, type Study 1/Solution 1: Bearing in the Label text field.
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 Boundary.
4
From the Selection list, choose Journals.
Fluid Pressure (hdb)
1
In the Model Builder window, under Results click Fluid Pressure (hdb).
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Dataset list, choose Study 1/Solution 1: Bearing (sol1).
4
Locate the Plot Settings section. Clear the Plot dataset edges check box.
5
From the View list, choose New view.
Arrow Surface 1
1
Right-click Fluid Pressure (hdb) and choose Arrow Surface.
2
In the Settings window for Arrow Surface, locate the Expression section.
3
In the X component text field, type hdb.fbx.
4
In the Y component text field, type hdb.fby.
5
In the Z component text field, type hdb.fbz.
6
Locate the Arrow Positioning section. From the Placement list, choose Mesh nodes.
7
Locate the Coloring and Style section.
8
Select the Scale factor check box. In the associated text field, type 1e-8.
9
Click the  Zoom Extents button in the Graphics toolbar.
10
In the Fluid Pressure (hdb) toolbar, click  Plot.
Plot the stress in the crankshaft and foundations, shown in Figure 3 and Figure 5, using the following instructions. First you start by duplicating the original solution and restricting the selections of the duplicated solutions to the specific components.
Study 1/Solution 1: Crankshaft
1
In the Model Builder window, under Results>Datasets right-click Study 1/Solution 1 (sol1) and choose Duplicate.
2
In the Settings window for Solution, type Study 1/Solution 1: Crankshaft in the Label text field.
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
Select Domain 1 only.
Study 1/Solution 1: Foundation
1
In the Model Builder window, under Results>Datasets right-click Study 1/Solution 1: Crankshaft (sol1) and choose Duplicate.
2
In the Settings window for Solution, type Study 1/Solution 1: Foundation in the Label text field.
Selection
1
In the Model Builder window, expand the Results>Datasets>Study 1/Solution 1: Foundation (sol1) node, then click Selection.
2
In the Settings window for Selection, locate the Geometric Entity Selection section.
3
Click  Clear Selection.
4
In the Graphics window toolbar, clicknext to  View Unhidden, then choose View Hidden Only.
5
Select Domains 6 and 9 only.
Crankshaft Stress
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Crankshaft Stress in the Label text field.
3
Locate the Data section. From the Dataset list, choose Study 1/Solution 1: Crankshaft (sol1).
Surface 1
1
Right-click Crankshaft Stress and choose Surface.
2
In the Settings window for Surface, locate the Expression section.
3
In the Expression text field, type mbd.mises.
4
Locate the Coloring and Style section. From the Color table list, choose Prism.
5
Click to expand the Range section. Select the Manual color range check box.
6
In the Maximum text field, type 1e7.
Deformation 1
1
Right-click Surface 1 and choose Deformation.
Highlight the deformation in the crankshaft by scaling it. Use the deformation in the body fixed reference frame to remove the effect of the finite rotation in the deformation.
2
In the Settings window for Deformation, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1)>Multibody Dynamics>Displacement>u_ref,...,w_ref - Displacement field, reference frame (spatial frame).
3
Locate the Scale section.
4
Select the Scale factor check box. In the associated text field, type 800.
Crankshaft Stress
1
In the Model Builder window, under Results click Crankshaft Stress.
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  Zoom Extents button in the Graphics toolbar.
5
Click the  Go to XY View button in the Graphics toolbar.
6
In the Crankshaft Stress toolbar, click  Plot.
Foundation Stress (mbd)
1
Right-click Crankshaft Stress and choose Duplicate.
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Dataset list, choose Study 1/Solution 1: Foundation (sol1).
4
In the Label text field, type Foundation Stress (mbd).
5
Locate the Plot Settings section. From the View list, choose New view.
6
Click the  Go to Default View button in the Graphics toolbar.
7
Click the  Zoom Extents button in the Graphics toolbar.
Surface 1
1
In the Model Builder window, expand the Foundation Stress (mbd) node, then click Surface 1.
2
In the Settings window for Surface, locate the Range section.
3
In the Maximum text field, type 3e6.
Deformation 1
1
In the Model Builder window, expand the Surface 1 node, then click Deformation 1.
2
In the Settings window for Deformation, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1)>Multibody Dynamics>Displacement>u,v,w - Displacement field.
3
Locate the Scale section. In the Scale factor text field, type 3e3.
Foundation Stress (mbd)
1
In the Model Builder window, under Results click Foundation Stress (mbd).
2
In the Foundation Stress (mbd) toolbar, click  Plot.
The variation in the engine speed is shown in Figure 6. Reproduce this plot using the instructions below.
Engine Speed
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Engine Speed in the Label text field.
Global 1
1
Right-click Engine Speed 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
d(theta,t)*60[s]/(2*pi[rad])
RPM
Engine speed
4
In the Engine Speed toolbar, click  Plot.
Engine Speed
1
In the Model Builder window, click Engine Speed.
2
In the Settings window for 1D Plot Group, locate the Plot Settings section.
3
Select the y-axis label check box. In the associated text field, type Engine speed (RPM).
4
Click to expand the Title section. From the Title type list, choose Label.
5
Locate the Legend section. Clear the Show legends check box.
6
In the Engine Speed toolbar, click  Plot.
Figure 7 shows the reactions of the bearings to the pressure variation in cylinder. Reproduce this plot using the instructions below.
Bearing Reactions and Piston Load
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Bearing Reactions and Piston Load in the Label text field.
Global 1
1
Right-click Bearing Reactions and Piston Load 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)>Hydrodynamic Bearing>Fluid loads>Fluid load on journal (spatial frame) - N>hdb.hjb1.Fjz - Fluid load on journal, z component.
3
Click Add Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1)>Hydrodynamic Bearing>Fluid loads>Fluid load on journal (spatial frame) - N>hdb.hjb2.Fjz - Fluid load on journal, z component.
4
Click Add Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1)>Multibody Dynamics>Hinge joints>Hinge Joint 1>Joint force (elastic) - N>mbd.hgj1.F_elz - Joint force (elastic), z component.
5
Click Add Expression in the upper-right corner of the y-Axis Data section. From the menu, choose Component 1 (comp1)>Multibody Dynamics>Hinge joints>Hinge Joint 3>Joint force (elastic) - N>mbd.hgj3.F_elz - Joint force (elastic), z component.
6
Locate the y-Axis Data section. In the table, enter the following settings:
Expression
Unit
Description
hdb.hjb1.Fjz
N
Bearing (left)
hdb.hjb2.Fjz
N
Bearing (right)
mbd.hgj1.F_elz
N
Elastic joint (left)
mbd.hgj3.F_elz
N
Elastic joint (right)
p*A
N
Piston load
hdb.hjb1.Fjz+hdb.hjb2.Fjz+mbd.hgj1.F_elz+mbd.hgj3.F_elz
N
Total
7
In the Bearing Reactions and Piston Load toolbar, click  Plot.
Bearing Reactions and Piston Load
1
In the Model Builder window, click Bearing Reactions and Piston Load.
2
In the Settings window for 1D Plot Group, locate the Title section.
3
From the Title type list, choose Label.
4
Locate the Plot Settings section.
5
Select the y-axis label check box. In the associated text field, type Force (N).
6
Locate the Legend section. From the Position list, choose Upper left.
7
In the Bearing Reactions and Piston Load toolbar, click  Plot.
Reproduce Figure 8 for various torques on the crankshaft using the instructions below.
Crankshaft Torque
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Crankshaft Torque 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 check box. In the associated text field, type Torque (N*m).
Global 1
1
Right-click Crankshaft Torque 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
-p*A*sin(theta+theta0)*0.02[m]
N*m
Torque on crankshaft (approximate)
Ti
N*m
Starting torque
To
N*m
Output torque
4
In the Crankshaft Torque toolbar, click  Plot.
Follow the instructions below to plot the power generated in the engine shown in Figure 9.
Power Generated
1
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
2
In the Settings window for 1D Plot Group, type Power Generated in the Label text field.
Global 1
1
Right-click Power Generated 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
P
HP
Power generated
4
In the Power Generated toolbar, click  Plot.
5
Click to expand the Legends section. Clear the Show legends check box.
Power Generated
1
In the Model Builder window, click Power Generated.
2
In the Settings window for 1D Plot Group, locate the Plot Settings section.
3
Select the y-axis label check box. In the associated text field, type Power generated (HP).
4
Locate the Title section. From the Title type list, choose Label.
Duplicate the current plot and make the following changes to reproduce the plot for the BHP shown in Figure 10.
BHP
1
Right-click Power Generated and choose Duplicate.
2
In the Settings window for 1D Plot Group, type BHP in the Label text field.
3
Locate the Plot Settings section. In the y-axis label text field, type BHP.
Global 1
1
In the Model Builder window, expand the BHP node, then click Global 1.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
BHP
HP
Brake horse power
4
In the BHP toolbar, click  Plot.
Figure 11 is a plot of the orbit of the left journal. You can reproduce it using the following instructions.
1D Plot Group 13
In the Home toolbar, click  Add Plot Group and choose 1D Plot Group.
Global 1
1
Right-click 1D Plot Group 13 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)>Multibody Dynamics>Attachments>Attachment: Journal 1>Rigid body displacement (spatial frame) - m>mbd.att1.w - Rigid body displacement, z component.
3
Locate the y-Axis Data section. In the table, enter the following settings:
Expression
Unit
Description
mbd.att1.w/C
1
 
4
Locate the x-Axis Data section. From the Parameter list, choose Expression.
5
Click Replace Expression in the upper-right corner of the x-Axis Data section. From the menu, choose Component 1 (comp1)>Multibody Dynamics>Attachments>Attachment: Journal 1>Rigid body displacement (spatial frame) - m>mbd.att1.v - Rigid body displacement, y component.
6
Locate the x-Axis Data section. In the Expression text field, type mbd.att1.v/C.
7
In the 1D Plot Group 13 toolbar, click  Plot.
Journal 1 Orbit
1
In the Model Builder window, under Results click 1D Plot Group 13.
2
In the Settings window for 1D Plot Group, type Journal 1 Orbit in the Label text field.
3
Locate the Title section. From the Title type list, choose Label.
4
Locate the Legend section. Clear the Show legends check box.
5
Locate the Plot Settings section.
6
Select the x-axis label check box. In the associated text field, type Relative y displacement.
7
Select the y-axis label check box. In the associated text field, type Relative z displacement.
8
In the Journal 1 Orbit toolbar, click  Plot.
Duplicate the current plot, and make the following changes to plot the journal eccentricity shown in Figure 12.
Journal Eccentricity
1
Right-click Journal 1 Orbit and choose Duplicate.
2
In the Settings window for 1D Plot Group, type Journal Eccentricity in the Label text field.
3
Locate the Plot Settings section. Clear the x-axis label check box.
4
In the y-axis label text field, type Relative eccentricity.
Global 1
1
In the Model Builder window, expand the Journal Eccentricity node, then click Global 1.
2
In the Settings window for Global, locate the y-Axis Data section.
3
In the table, enter the following settings:
Expression
Unit
Description
sqrt(mbd.att1.v^2+mbd.att1.w^2)/C
1
Relative eccentricity
4
Locate the x-Axis Data section. From the Parameter list, choose Time.
5
In the Journal Eccentricity toolbar, click  Plot.
Finally create animations for the displacement, bearing pressure, and foundation stress using the instructions below.
Animation: Displacement
1
In the Results toolbar, click  Animation and choose Player.
2
In the Settings window for Animation, type Animation: Displacement in the Label text field.
3
Locate the Animation Editing section. From the Time selection list, choose Manual.
4
In the Time indices (1-2401) text field, type range(1000,1,1201).
5
Click the  Zoom Extents button in the Graphics toolbar.
6
Locate the Frames section. In the Number of frames text field, type 100.
7
Click the  Play button in the Graphics toolbar.
Fluid Pressure (hdb)
Click the  Go to Default View button in the Graphics toolbar.
Animation: Fluid Pressure
1
In the Results toolbar, click  Animation and choose Player.
2
In the Settings window for Animation, type Animation: Fluid Pressure in the Label text field.
3
Locate the Scene section. From the Subject list, choose Fluid Pressure (hdb).
4
Locate the Frames section. In the Number of frames text field, type 100.
5
Locate the Animation Editing section. From the Time selection list, choose Manual.
6
In the Time indices (1-2401) text field, type range(700,1,801).
7
Click the  Zoom Extents button in the Graphics toolbar.
8
Click the  Play button in the Graphics toolbar.
Animation: Foundation Stress
1
In the Results toolbar, click  Animation and choose Player.
2
In the Settings window for Animation, type Animation: Foundation Stress in the Label text field.
3
Locate the Scene section. From the Subject list, choose Foundation Stress (mbd).
4
Locate the Animation Editing section. From the Time selection list, choose Manual.
5
In the Time indices (1-2401) text field, type range(1100,1,1200).
6
Click the  Zoom Extents button in the Graphics toolbar.
7
Click the  Play button in the Graphics toolbar.