UG刚柔耦合仿真分析

1.In this lesson
After completing this lesson, you will be able to:
∙Create an SEMODES 103 – Flexible Body solution in Advanced Simulation. ∙Connect the flexible body finite element model to the degrees of freedom in the motion mechanism.
∙Solve the finite element model and generate the RecurDyn Rflex input file.∙Define the flexible body in Motion Simulation and solve the motion mechanism.
∙Animate the motion mechanism and observe the flexible body deformation.
✓✓2. Overview
Typical motion simulations represent mechanisms using rigid bodies that move in prescribed degrees of freedom according to constraints. These rigid-body motion simulations cannot represent certain dynamic characteristics, especially those resulting from conditions such as sharp impacts, sudden changes in motion, or when the component is flexible enough to affect the motion of the mechanism. For these situations, you can use a flexible body analysis to combine both elastic deformation and rigid body motion.
This type of analysis requires NX Motion Simulation with the RecurDyn solver and NX Advanced Simulation with the NX Nastran solver.
T o set up a flexible body analysis for a component in your mechanism, you create a finite element model on the component and define stiffness at the points where it is connected to the mechanism (typically at joint locations). The NX Nastran SEMODES 103 – Flexible Body solution reduces the dynamic behavior of the flexible body to a set of mode shapes, which are stored in an output file. After you solve this modal solution, you associate the flexible body output file (.rfi file) with the link on which the component is defined in the motion simulation. When you solve the motion simulation, the RecurDyn solver communicates with NX Nastran and recovers the FE results. When you animate the mechanism, the contour plot for the flexible component is animated along with the rigid body animation.
3. Workflow
Advanced Simulation steps
1.Create a finite element model and NX Nastran SEMODES 103 – Flexible
Body solution.
2.Create a finite element mesh on the flexible component and assign
material properties.
e a 1D Connection (spider element) or other constraint elements to
define the component's connection points to the mechanism.
4.Add Fixed Boundary Degrees of Freedom constraints to define
connection degrees of freedom.
5.Add Free Boundary Degrees of Freedom constraints to define load
degrees of freedom.
6.Solve the modal solution. A RecurDyn Rflex input (.rfi) file is generated
for the flexible link.
7.Repeat steps 1–6 for each additional flexible component in the
mechanism.
Motion Simulation steps
1.Create a Flexible Body Dynamics motion simulation.
2.Create flexible links on the flexible components. Associate each .rfi file
with each flexible link.
3.Create a Flexible Body solution and add the flexible links to the solution.
4.Solve the mechanism.
5.Run Animation to view the combined rigid body and flexible body motion.
6.Plot the modal degrees of freedom vs. time to determine the contribution
of selected modes to the flexible body results.
You can select one or more modes of the flexible body and then plot the modal displacement, acceleration, or velocity.
4. Activity: Flexible body analysis — Introduction
Estimated time to complete: 12–16 minutes
You will learn how to:
Define the flexible body in Motion Simulation and solve the
motion mechanism.
Animate the motion mechanism and observe the flexible body
deformation.
Note T o complete this activity, you must have the nx_motion_rflex license, in addition to Motion Simulation, Advanced Simulation, and NX Nastran.
Launch the Flexible body analysis — Introduction activity.
5. About the flexible body modal solution
You will use the Advanced Simulation application to create a finite element model of the flexible body and perform a modal analysis. A modal analysis solves for the natural frequencies and mode shapes of flexible bodies.
The NX Nastran SEMODES 103 – Flexible Body modal solution reduces the flexible body's mass and stiffness to modal space to represent its dynamic behavior. These reduced matrices are saved in the RecurDyn Rflex input file (.rfi).
Then, in Motion Simulation, you associate the .rfi file with a link to create the flexible link.
Example mode shapes
6. About the finite element mesh
The finite element model of a given body consists of a finite element mesh, material properties, and constraints.
When you create a mesh on the body, the software divides the body into discrete regions called elements that are joined together at points called nodes. A group of elements is called a mesh.
The mesh follows the shape of the body. When the model is solved, as the nodes in the mesh are displaced due to the analysis conditions such as loads, the behavior of each element is described by mathematical equations. The software finds the analysis solution by summing the individual element solutions.
Example mesh of tetrahedral elements
In Advanced Simulation, you create the mesh in the FEM file.
When you use a smaller element size (resulting in more elements in a mesh), the accuracy of the solution is improved. However, as you refine the mesh, the solution time and computer resources needed to solve are also increased.
7. Assigning a material to the mesh
In Motion Simulation, material properties for a component are inherited from the master model on which you create the simulation. In Advanced Simulation, you must assign the same material to the flexible body finite element mesh as the material used for the flexible link in Motion Simulation.
T o assign a material to the mesh, edit the mesh collector that contains the mesh. Then, modify the physical property table for the collector and open the Material List dialog box, where you can select the material to use.
8. Connecting the flexible body FEM to the mechanism
In Advanced Simulation, in the FEM file, you must define the points where the flexible body is connected to the motion mechanism. These connection points must be defined at the origin point of every joint, bushing, force, torque, spring, or damper motion object on the flexible body.
Although you can use any element type to define these connection points, typically you will use a 1D Connection (spider element).
For accuracy in your flexible body solution, a single independent node (such as the core node of the spider element) in this connection element should be coincident with the motion object's origin point. You will define stiffness at this connection node using special constraints described in the next section.
Spider elements defined at revolute joint locations
Make sure the connection node is at a location that creates balanced loading. For example, suppose you are connecting the flexible body to a revolute joint that is defined on a hole. Define the connection node in the bore center of the hole, rather than at the edge of the hole.
Example of pinned connection (Revolute joint defined at bore center of hole)
Connection node improperly defined at edge of hole
Connection node properly defined at bore center of hole
9. Defining connection and load degrees of freedom In Advanced Simulation, in the Simulation file, you must add special constraints to define the connection and load degrees of freedom for the flexible body.
∙At each connection node where the flexible body will be connected to the mechanism through a joint or bushing in Motion Simulation, create a Fixed Boundary Degrees of Freedom constraint to define the connection degrees of freedom.
∙At each connection node where a force, torque, spring, or damper will be applied to the flexible body in Motion Simulation, create a Free Boundary Degrees of Freedom constraint to define the load degrees of freedom.
10. Solving the NX Nastran modal solution
In the Solution dialog box for the SEMODES 103 – Flexible Body solution, you must specify the number of modes for which to solve and the result types to recover. By default, stress and displacement results are selected.
After you have defined the finite element mesh, connection and load degrees of freedom, and solution attributes (such as the number of desired modes), you can solve the model.
The solve produces several results files that you must not delete, move, or rename:
∙.dat — Nastran input file, needed for later results recovery.
∙.op2 — Contains the model geometry and component modes resulting from the modal analysis.
∙_0.op2 — Needed for later results recovery; contains the component mode definitions, modal mass, and modal stiffness.
∙.rfi — RecurDyn Rflex input file, needed for representing the flexible body in the RecurDyn solve.
Remember the location of the .rfi file because you will need to point to it when creating the flexible link in Motion Simulation.
11. Review
Question
In the following example, suppose you are defining this excavator bucket as
a flexible body in Advanced Simulation. In the motion mechanism, a single revolute joint is defined between the two holes (1 in the graphic below) at the top of the bucket. A force load is applied to one of the teeth (2).
In Advanced Simulation, which constraints must you apply before solving the SEMODES 103 – Flexible Body solution? 2
A Fixed Translation constraint and a Pinned constraint
A Fixed Boundary Degrees of Freedom constraint and a Free Boundary Degrees of Freedom constraint
A User Defined constraint and a Pinned constraint
T wo Fixed constraints
After solving the SEMODES 103 – Flexible Body solution, when you create the flexible link in Motion Simulation, what file must you associate with the link to represent the dynamic behavior of the flexible body in the
mechanism?
The .RFI file
The .DAT file (Nastran input deck)
The .OP2 file
The .MDF file
✓Show feedback
12. Activity: Flexible body analysis — Advanced Simulation tasks
Estimated time to complete: 12–16 minutes
You will learn how to:
Create an SEMODES 103 – Flexible Body solution in Advanced
Simulation and specify a body as flexible.
Connect the flexible body finite element model to the degrees
of freedom in the motion mechanism.
Solve the finite element model and generate the RecurDyn
Rflex input file.
Note T o complete this activity, you must have the nx_motion_rflex license, in addition to Motion Simulation, Advanced Simulation, and NX Nastran.
Launch the Flexible body analysis — Advanced Simulation tasks
activity.
13. Defining the flexible link in the mechanism
In Motion Simulation, you must create a Flexible Link that is associated with the component or body that you defined as flexible in Advanced Simulation.
In the Flexible Link dialog box, you associate the link with the RecurDyn input file (.rfi file) generated by the NX Nastran modal solution. The Flexible Link Preview window helps you determine the correct method for positioning the flexible body on the link.
In the graphics window, the flexible link is displayed with its finite element mesh.
Meshed flexible link defined in the mechanism (and Preview view)
14. Choosing modes to include in the analysis
By default, all modes from the NX Nastran modal solution are included in the motion simulation solve except the first six modes, which are considered
rigid-body modes.
Including all modes ensures a more accurate representation of the structure. However, for better solve performance, you can reduce the modal model by removing insignificant modes.
T o determine which modes to remove, you can view and animate the mode shapes using the Post Processing Navigator and Post Processing toolbar. Make sure to include all modes that resemble the behavior you are analyzing.
Example mode shape
✓✓15. Solving the model and animating the mechanism
In Motion Simulation, you create a Kinematics/Dynamics solution of type Flexible Body.
When you solve the Flexible Body solution, the RecurDyn solver calculates the physical deformations at each point where the flexible body is connected to the rest of the mechanism, for each configuration of the motion mechanism. It saves these deformations in a modal deformation file (.mdf).
Using the .mdf file, the motion solution process calls the NX Nastran solver to recover the deformation, displacement, stress, and other results on the original, unreduced flexible body. These transient results are then returned to Motion Simulation, where you can view them in an animation of the mechanism.
By default, when you animate a flexible body solution, translational deformation results (nodal displacements) are displayed for the flexible body. You can also display other results, such as Displacement – Nodal, Stress – Element – Nodal and Strain – Element – Nodal, depending on the results you requested in the output request for the SEMODES 103 – Flexible Body solution in Advanced Simulation.
16. Activity: Flexible body analysis — Motion Simulation tasks
Estimated time to complete: 12–16 minutes
You will learn how to:
Define the flexible body in Motion Simulation and solve the
motion mechanism.
Animate the motion mechanism and observe the flexible body
deformation and stress.
Run an interference check between the flexible link and a body
panel.
Note T o complete this activity, you must have the nx_motion_rflex license, in addition to Motion Simulation, Advanced Simulation, and NX Nastran.
Launch the Flexible body analysis — Motion Simulation tasks
activity.
Flexible body analysis — Introduction
1. Open the Motion Simulation
Open (Standard toolbar)
∙
∙
∙
∙
OK
∙
The motion simulation opens in the Motion Simulation application.
2. Reset the dialog box settings
The options you select in NX dialog boxes are preserved for the next time you open the same dialog box within an NX session. To ensure that the dialog boxes are in the expected initial state for each step-by-step activity, you should restore the default settings.
Preferences→User Interface
∙
Reset Dialog Box Settings
∙
OK
3. Enable the Flexible Body Dynamics environment The Flexible Body Dynamics environment is available only with the Dynamics analysis type.
Environment (Motion toolbar)
∙
Flexible Body Dynamics
∙
OK
✓✓4. Define the flexible link
Flexible Link (Motion toolbar)
∙
∙
Flexible Model
∙Browse
∙intro_flex_body/fbcam_assy_sim2-solution_1_0.rfi
This pre-generated file contains a modal reduction of the flexible body's mass and stiffness, which represen ts the body’s dynamic behavior. The NX Nastran solver generates these reduced matrices and saves them in a RecurDyn Rflex input (RFI) file. In a later activity, you will solve an NX Nastran solution and generate an RFI file.
∙
OK RFI File dialog box
Leave the Flexible Link dialog box open for the next step.
5. Finish defining the flexible link
The Flexible Link dialog box is still open from the previous step.
∙The Flexible Link Preview window shows you the meshed flexible body and its orientation relative to the absolute coordinate system.
∙
∙Because the flexible body is in the same orientation relative to the absolute coordinate system as the corresponding link in the mechanism, Absolute Origin is the appropriate selection.
∙
OK Flexible Link dialog box
6. Create a Flexible Body solution
Motion Navigator
∙motion_1
∙New Solution
∙
∙
∙
∙
∙
OK
7. Add the flexible link to the solution
Motion Navigator
∙Flexible Links
∙L002–fbcam_assy_sim2-solution_1
∙Add to Solution
8. Solve the motion simulation
Motion Navigator
∙Load Container
∙G002
∙Add to Solution
For illustration purposes, this vector force simulates a load on the clevis in the X direction, to exaggerate the flexible behavior.
∙Solution_2
∙Solve
The solve process may take several minutes to complete. After the RecurDyn solve finishes, NX Nastran is called automatically to run the SEMODES 103 –Flexible Body solve. Nastran uses the RecurDyn results file and the original NX Nastran input file to recover the deformation, displacement, stress and other results for the flexible link.
Caution Do NOT close any solve windows until all NX Nastran command prompt windows have closed and the message ―Nastran results
recovery completed‖ appears in the NX status line.
9. Animate the mechanism
Animation (Motion toolbar, Simulation Drop-down list)
∙Play（此处为动图，有需要可联系上传者）
By default, the contour plot of the flexible link displays nodal translational deformation results. You can also display other results, such as Displacement – Nodal and Stress – Element – Nodal, depending on the results you
requested in the output request for the SEMODES 103 – Flexible Body solution in Advanced Simulation.
∙
OK
You completed the activity.
Flexible body analysis — Advanced Simulation tasks
1. Open the simulation
Open (Standard toolbar)
∙
∙
∙
∙
OK
∙
The motion simulation opens in the Motion Simulation application.
2. Reset the dialog box settings
The options you select in NX dialog boxes are preserved for the next time you open the same dialog box within an NX session. To ensure that the dialog boxes are in the expected initial state for each step-by-step activity, you should restore the default settings.
Preferences→User Interface
∙
Reset Dialog Box Settings
∙
OK
3. Solve and animate the solution
Before adding the flexible body, solve and animate the included solution to see the rigid-body motion of the mechanism.
Motion Navigator
∙Solution_1
∙Solve
Animation (Motion toolbar, Simulation Drop-down list)
Packaging Options
∙
Interference
∙
Pause on Event
∙An Interference packaging option has been predefined between the suspension arm and the sheet body panel. When you animate the mechanism, if the suspension arm and body panel come into contact, the interfering
bodies will be highlighted and the animation will pause.
∙Play
As you can see, no interference occurs. Later in this activity, we will check for interference again with the suspension arm defined as a flexible link.
∙
OK
4. Start Advanced Simulation
Motion Navigator
∙_demo_assy
∙Make Work
This command changes the work part from the motion simulation to the part file.
No Save Simulation Part File message
Start→Advanced Simulation
5. Create Simulation and FEM files
Simulation Navigator
∙_demo_assy.prt
∙New FEM and Simulation
The New FEM and Simulation dialog box lists the three new files that will be created: the Simulation, FEM, and idealized part file.
The Solver Environment section lists NX Nastran as the solver. The Analysis Type is Structural.
∙
∙(the lower suspension arm)
∙
OK New FEM and Simulation dialog box
∙The Solution dialog box appears.
∙
∙
Case Control
∙Edit (Lanczos Data)
∙
∙
∙This specified frequency range means the solver will calculate the lowest-frequency modes within the first 20 modes starting from the
frequency of 0.
∙If you increase the number of desired modes, you can achieve a more accurate representation of the structure, but at the expense of solution time.
You should include enough modes to cover the frequency range of interest (based on your particular mechanical system).
∙
OK Real Eigenvalue – Lanczos dialog box
Caution Accept the default settings for Flexible Body Solution Type and Flexible Body Export Options. These options are intended for
manual integration with RecurDyn or Adams software packages, and
should not be changed for NX Motion Simulation. If you change these
default settings, the Motion Simulation flexible body solution may
not solve.
∙
OK Solution dialog box
∙
6. Connect the flexible body FEM to the mechanism You must define the points where the flexible body is connected to other degrees of freedom in the motion mechanism. Although you can use any element
type to connect the flexible body, typically you will use a 1D Connection (spider element).
Simulation Navigator
∙
Simulation File View
Note If the Simulation File View is not visible, click the
bar at the bottom of the Simulation Navigator to open it.
∙_demo_assy_fem1
The FEM file is displayed in the graphics window, and is listed at the top of the Simulation Navigator.
Static Wireframe (View toolbar, Rendering Style Drop-down list)
1D Connection (Advanced Simulation toolbar, Connections
Drop-down list)
∙
∙(Select Point)
∙
∙Arc/Ellipse/Sphere Center (Specify Point 1 and Specify Point 2)
∙,
Note Select the arc centers of the top and bottom edges.
∙
OK Point dialog box
∙(the face)
∙
Connection Element
∙
∙
Apply
∙
∙This creates a connection recipe. In a later step in this activity, when you create a solid mesh on the part, the connection recipe will generate a spider element using nodes defined in the geometry mesh.
∙Repeat the above steps to create Point to Face RBE2 connection recipes on the other two ends of the arm, as shown in the following pictures.
When you are finished, close the 1D Connection dialog box.
7.Mesh the part
Now create a tetrahedral mesh on the solid body.
Shaded with Edges (View toolbar, Rendering Style Drop-down list)
3D Tetrahedral Mesh (Advanced Simulation toolbar, Mesh
Drop-down
list)
∙the part
∙
∙
Mesh Parameters
∙
∙
in the regions where bending is predicted. At least three layers of solid
elements are needed to accurately model bending.
∙
OK
∙
∙The part is meshed with tetrahedral solid elements and the connection recipes are now 1D spider elements.
∙
8. Create a node group
Later in this activity, you will need to define stiffness at the node at the center of each of the three 1D connections you created previously. To make that step easier, you will add these nodes to a node group.
Simulation Navigator
∙Groups
∙New Group
∙
Node Labels
∙Because you created the connection recipes before you meshed the part, the core nodes of the resulting 1D connections are labeled 1, 2, and 3. You will add these nodes to the group by entering their labels.
∙
∙Select
∙
∙
OK
9. Define material properties
Simulation Navigator
∙3D Collectors (expand)
∙Solid(1)
∙Edit
∙Edit (Solid Property)
∙
Properties
∙Choose material
∙
∙
OK all dialog boxes
10. Display the Simulation file
Simulation Navigator
∙
Simulation File View
∙_demo_assy_sim1
11. Define connection degrees of freedom
In a previous step, you created spider elements at the three ends of the suspension arm. The independent node at the center of each spider element was defined to be coincident with the origin point of a joint or bushing that connects this component to the mechanism. You will now define the local stiffness at these connection points using a Fixed Boundary Degrees of Freedom constraint.
Static Wireframe (View toolbar, Rendering Style Drop-down list)
Fixed Boundary Degrees of Freedom (Advanced Simulation toolbar,
Constraint Type list )
∙
Model Objects
∙
Group Reference
∙
_demo_assy_fem2::connection_nodes
Note This is the node group you created in the previous step.
∙
Degrees of Freedom
∙All On
T o ensure the correct local stiffness at the connection points, always set all DOF to On when creating Fixed Boundary Degrees of Freedom or Free Boundary Degrees of Freedom constraints in a flexible body analysis.
∙
OK
∙
∙When you created the connection recipe for each spider element, you placed the independent node at the bore center of the hole rather than at the arc center of the edge of the hole. This placement ensures balanced loading.
Save (Standard toolbar)
12. Solve the model
You will solve the model to generate the .rfi file that contains the reduced matrices that represent the component's dynamic behavior. This file will be used later in the activity when you solve the Flexible Body solution in Motion Simulation.
Simulation Navigator (main view)
∙Solution 1
∙Solve
∙
OK
∙Y ou can ignore the Information window warning concerning rigid links.
∙The Analysis Job Monitor dialog box appears.
∙Wait for the job to finish and for the command window to close. This process may take several minutes.
∙
Close Solution Monitor dialog box
∙
Cancel Analysis Job Monitor dialog box
∙Information window
∙Solution 1
∙Browse
In the explorer window that opens, note the location of the .rfi file. It should be located in the f1_car_flex_body folder, and should be named similar to
_demo_assy_sim1-solution_1_0.rfi.
13. View the mode shapes
Simulation Navigator
∙Results
Post Processing Navigator
∙Solution 1 (expand)
The first six modes are rigid body modes.
∙Mode 7 (expand)
∙Displacement – Nodal (expand)
∙Magnitude
Note The ends of the part overlap because of the default deformation scale, which is set to 10% of the model. You can reduce the scaling using Edit
Post View(Post-Processing toolbar).
Next Mode/Iteration (Post Processing toolbar)
Use the Next Mode/Iteration command to view additional modes.
Return to Model (Layout Manager toolbar)
Save (Standard toolbar)
In a later activity, you will connect the flexible body to a motion mechanism. If you plan to complete the next Flexible Body activity, leave this simulation file open in NX.
You completed the activity.
Flexible body analysis — Motion Simulation tasks
1. Open the Motion Simulation
If you completed the steps in the previous Flexible Body activity and your
_demo_assy_sim1.sim part is still open in NX, use these steps.
If the part is not still open, or if you did not complete the previous Flexible Body activity, skip to the next page.
Simulation Navigator
∙
Simulation File View
∙_demo_assy
∙Make Displayed Part
This command changes the work part from the simulation file to the master model assembly.
Start→Motion Simulation
Motion Navigator
∙motion_1
Skip the next page and move on to page 3.
2. Open the Motion Simulation
Use these steps if the _demo_assy_sim1.sim part was not still open from the previous Flexible Body activity.
Open (Standard toolbar)
∙
∙
∙
∙
OK
∙
The motion simulation opens in the Motion Simulation application.
3. Reset the dialog box settings
The options you select in NX dialog boxes are preserved for the next time you open the same dialog box within an NX session. To ensure that the dialog boxes are in the expected initial state for each step-by-step activity, you should restore the default settings.
Preferences→User Interface
∙
Reset Dialog Box Settings
∙
OK
4. Enable the Flexible Body Dynamics environment
The Flexible Body Dynamics environment is available only with the Dynamics analysis type.
Environment (Motion toolbar)
∙
Flexible Body Dynamics
∙
OK
5. Define the flexible link
Flexible Link (Motion toolbar)
∙
Note You can select any part of the indicated link.
∙
Flexible Model
∙Browse
∙_demo_assy_sim1–solution_1_0.rfi
This is the .rfi file generated from the NX Nastran solve in the previous Flexible Body activity. It should be located in the f1_car_flex_body folder along with the FEM and Simulation files you created in Advanced Simulation.
Note If you did not complete the previous Flexible Body activity, copy the provided Simulation file, named _demo_assy_sim1.sim, from the。