ug振动响应分析详细分析教程

Top Gun 2008
HESSI Satellite
Assembly FEM/Response Simulation Workshop
In the last workshop, you built the satellite in the deployed configuration. For the launch loads applied with in this workshop we need the satellite in the deployed configuration.
Since this would be a repeat of steps that you had done, this was done for you using the following steps:
1. Used the solid properties and calculated the mass
of a panel.
2. Unmapped the panels from the assembly FEM.
3. Added 3 concentrated masses at the connection
points for the solar panels.
Steps of this Workshop:
1. Apply Enforced Displacement Restraints
2. Create the global damping
3. Solve for the normal modes
4. Create a response simulation
5. Review the results for the mass participation
6. Create the sensors
7. Create a random excitation
8. Calculate the acceleration at the sensors
9. Calculate the RMS for the middle platform
PART II: Response Simulation
Open and load necessary files
Select “File, open” to open “satellite_sim1.sim” file.
Set ‘Files of type’ to “Simulation Files (*.sim)”
•
•
Navigate to the appropriate folder and select “satellite.sim”
•
Select OK
In the simulation navigator, create a new solution. Solution type is Sol 103 Response Simulation.
Make sure to move all the contact sets to the new solution.
Create the restraints and enforced motion locations
Select the “No Rotation” icon and the center node of the rigid element on the base of the satellite.
Select the “Enforced Motion Location” icon, and select the same node. Assign the 3 translational DOF to the motion.
Save your work.
Set up Normal Modes Solution
Highlight the Dynamic Subcase, and use the RMB to select “Edit Solution Step” .
Create an output request for Displacement and Stress. Then create a Lanczos solve for 100 modes between 0 and 500 HZ.
Highlight the solution and use RMB to select “Edit Solution” . Select the Parameters tab, and set the “AutoMPC” to “Yes” and the “G” to 0.04. G sets the global damping. (Note: G is 2 times the rat io C/C 0)
Save
your work.
The solution should take
about 4 minutes.
Review Normal Modes
Switch to Post-Processing and load the results. The first mode should be around 44 HZ.
Return to the simulation navigator. Highlight the SIM and using RMB, select “New Solution Proces s”and ‘Response Simulation” .
Select OK when the form comes up. This allows the user to select the desired solution if more then one normal modes analysis has been done.
In the simulation navigator, highlight the normal modes. Open the Response Simulation Details View and review the total percent of mass participating using the 100 modes. This typically should be between 80% and 85%.
Save your work. The damped frequencies are calculated from the NXN damping matrix.
Set up the response simulation analysis
The file will have groups created in it. Open the groups, and you will see some that end in “elements”and some that end in“nodes”. These are used for the creating the sensors. Display a node group. Then highlight“Sensors”in the simulation navigator and using RMB, create new sensor. You can either select t h e nodes shown or change method to“Nodes by Group”and select one of the nodes. Repeat the process for the other 2 groups.
You should have 3 sensors that contain 4, 3, and 12 nodes. If you highlight one, you should see the sensor locations highlighted in orange. These can be changed using the Style under RMB.
Create an event. Select Random and give it the name Launch.
To create an excitation, you will need to associate an AFU file with your SIM file. Select the XY Function Navigator. Highlight the Associated AFU and use RMB and select Open. Navigate to the appropriate folder and select the“satellite_sim1.afu”file.
Switch back to the simulation navigator. Select the Nodal Translation Excitation icon or highlight the Excitations and use RMB to select New Excitation/Nodal Translation. Select Node 549 from the list and turn off the X & Y excitation functions.
Under the green arrow select“function manager. Select the only record in the AFU file. Then OK out of the two forms.
There are 3 directions creating in the solution run. Normally the vertical direction uses a different random function from the lateral directions. They are similar but often scaled different. This is taken
form a requirements document for a satellite.
Calculate and Review Results
Select the Calculate Modal Response icon. This will create a
modal response in the simulation navigator. This must be
deleted if any changes are to be made to the response simulation
solution.
A good practice is to verify the input by reviewing the results. Select the Evaluate Nodal Function and fill out the form as shown. Select the node that where the enforced motion was created.
This should look like the input. Next calculate the sensor results. It is a good practice to calculate each separately so that each sensor group has a unique identifier. Make sure that you turn on the“Store to AFU. It will create a new associated AFU file. You will need to repeat this for all 3 sensors.
Top Gun 2008
This is the plots from the equipment sensors. The X axis has been changed to only extend to 530 HZ. You will note that the first big spike in the graph is at around 100.4 HZ. If you look at the mass participation, you will see that the first dominate Z mode is 101.3 HZ and excites 49.5% of the mass. The red dashed line is the response at the input node.
These graphs can also be calculated for element quantities. Next you will calculate the RMS for the elements and review a contour plot using the post-processing application.
Display only the middle platform group or use the Elements by Group method. We will calculate the RMS stress for this surface only. This takes about 8 minutes, so you may want to do only a few elements. When it completes, double click on the result in the simulation navigator.
The results will all be zero. The default result is the element stress. This stress is at the midplane and is zero in most cases.
Top Gun 2008
Open the Post View and switch the results to either top or bottom.
If you turn off all elements except the CQUAD4_ 17 mesh, you will see this plot.
The Hessi Satellite Response Simulation workshop is now complete. Save your work.。