This PSD acceleration function will be applied in the workshop as enforced motion loading on the fender at the connection to the fork. We want to evaluate the dynamic displacements and stresses in the fender.
The PSD excitation will also be converted to a transient excitation and the solution re-solved in the time domain. Conversion to time domain is useful if one wants to perform a fatigue analysis of what is an inherently random loading since most fatigue software operates on time domain data. Also if frequency loads (such as from an engine), and random loads (such as from road input), occur at the same time, it is not possible to combine them in the frequency domain, but you can in the time domain.
Steps of Workshop:
· Set Role
· Open .prt file
· Create a fem
· Generate a Mesh
· Create a simulation
· Define boundary conditions
· Define solver parameters
· Solve for Modes UsingNX NastranSolver
· Post Process the Results to View the Mode Shapes
· Create Response Simulation
· Define Random Excitation Function
· Create Response Simulation Event for a Random Excitation
· Compute Response Functions for the Random Event
· Compute Full Field Response for the Random Event
· Convert PSD excitation to Transient
· Create Response Simulation Event for Transient Excitation
· Compute Response Functions for the Transient Event
· Convert Transient Results to PSD
· Compare PSD event Results to Transient Results
Set Role
Start NX 5. Select the ‘Roles’ tab on the
resource bar (
· Set the role to ‘Advanced with full menus’
Open the .prt File
Select “File, open” to open “fender.prt”.
· Set ‘Files of type’ to “Part Files (*.prt)”
· Navigate to the appropriate folder and select ‘fender.prt’
· Select ‘OK’
The part file contains a sheet body of the fender and a point located at the center of the four mounting holes.
Create a new FEM model
Start Advanced Simulation
Open the Simulation Navigator
Right click on fender.prt and select ‘New FEM…’. Name the new fem fender_fem’
On the New FEM form:
Generate Mesh
Generate a 2D Mesh
This will create a 2D collector container and a thin shell collector (ThinShell(1)) for the mesh.
Right click on the ThinShell(1) collector and pick ‘Edit…’
Select the Modify button
Create a 1D mesh
There are no properties to define for rigid elements. This completes the mesh for the fender
Create a Simulation
Right click on the fender_fem in the Simulation Navigator and select “New Simulation”.
· Enter a new filename of ‘fender_sim.sim’
· Select ‘OK’
· Hit ‘OK’ on the New Simulation form:
· Change the Solution Type to ‘SEMODES 103 – Response Simulation’ on the Create Solution form.
· Modify the name of the solution if you wish
· Select ‘OK’
· The result is a new simulation that contains an empty Response Simulation solution
Define Boundary Conditions
The input for this analysis is a displacement time history measured during a rough road test. The nodes at the input location must be marked as enforced motion locations so that theNX Nastransolution output includes the necessary constraint modes.
· Node display may be off by default in the new sim file. In order to define boundary conditions on nodes, they must be visible.
o Select ‘Preferences, Node and Element Display…’ on the menu bar.
o Set the Node Marker to ‘Dot’ (or asterisk if you prefer)
o Select ‘OK’
· Right click on ‘Constraints’ under the Response Simulation solution
· Select ‘New Constraint’, ‘Enforced Motion Location’
· Select the node at the center of the rigid elements
· Set all 6 DOF to ‘Enforced;
· Change the default name if you wish
· Select ‘OK’
· This will fix the grid in all 6 degrees of freedom for the modal analysis via an SPC. It will also place the 6 degrees of freedom in the U2 USET, which will tell the solver to generate a constraint mode for each of the dof.
Define Solver Parameters
Prior to solving, the solution parameters need to be defined to tell the solver how many modes and/or what frequency range to solve for, as well as what output to recover.
When the Response Simulation solution was created, three subcases were automatically defined: one for Static Offset; a second for Stress Stiffening and a third for Dynamics. This analysis does not contain a Static offset or Stress Stiffening, so only the attributes for the Dynamics subcase need to be defined.
· Right click on ‘Subcase – Dynamics’ in the Simulation Navigator and select ‘Edit Attributes…’ to bring up the Edit Solution Step form
· Select the Open Manager button next to Output Requests (boxed in red above) to open the Modeling Objects Manager
· Select Create
· On the Stress tab, change the location from ‘CENTER’ to ‘CORNER’
· Cycle through all of the remaining tabs except for Displacement and SPC Forces and toggle off the ‘Enable XXXXX Request’ checkbox on each tab.
· Select ‘Preview’ and verify that the output requests match the following:
· Close the Preview window and select OK on the Structural Output Request form and Close on the Modeling Objects Manager form
· Select the Open Manager button next to Lanczos Method (boxed in magenta in the Edit Solution Step image above) to open the Modeling Objects Manager
· Select Create
· Define a frequency range of 0 to 1024 Hz
· Select OK on the Real Eigenvalues form and Close on the Modeling Objects Manager Form
· The objects just created should be selected in the drop down menus on the Edit Solution Step form:
· Hit OK
Solve for Modes UsingNX NastranSolver
Right click on the Response Simulation solution in the Simulation Navigator and select ‘Solve…’
· Hit OK
Post Process the Results to View the Mode Shapes
· When the solution is completed, a Results item will appear in the Simulation Navigator under the Response Simulation Solution. Double click on Results to switch to the Post Processing Navigator and load the results.
OR…
· Select the Post Processing
Navigator tab (
· You should see that there are 18 mode shapes from 20.25 Hz to 972.1 Hz.
· There are also 6 constraint modes, one for each enforced motion degree of freedom
· Expand the results list for
Mode 1 by clicking the ‘plus’ (
· Double click on the ‘Displacement – Nodal’ item (or right click and select PLOT) to plot the mode shape.
· Toggle on the Post-Processing toolbar (if it isn’t already on):
· Use the red arrow to animate the mode shape. Use the green arrows to activate different modes. Look at several modes to see if they look reasonable.
· Select ‘Return to Model’ (
Create Response Simulation
· Return to the Simulation Navigator tab on the Resource Bar
· Toggle on the Response Simulation toolbar (if it isn’t already on):
· Select the ‘Create Response Simulation’ icon
· On the Create Response Simulation form, enter a name if you wish and select the ‘Response Sim’ Response dynamic solution.
· Select OK
This will create a Response Simulation item in the Simulation Navigator:
Notice that the modal representation for this analysis consists of the 18 normal modes plus an additional 6 constraint modes (one constraint mode shape is stored for each enforced motion location that was defined in the Response Simulation solution).
· Mode shapes may also be plotted by right clicking on the Normal Modes or Constraint Modes items and selecting ‘Quick View’.
· For a summary of the Normal Modes, click on the ‘Response Simulation Details View’ tab at the bottom of the Simulation Navigator
o This summary includes modal mass, stiffness and damping for each mode
Define Random Excitation Function
Open the Function Manager (
This function will be created as a table in an .afu file
On the ID page of the XY Function Editor:
On the XY Axis Definition page:
On the XY Data page, select
Enter the following data points:
Frequency (Hz) |
Acceleration (g2/Hz) |
10 |
0.0065 |
40 |
0.0065 |
240 |
0.0002 |
241 |
0.003 |
400 |
0.003 |
480 |
0.0015 |
680 |
0.00003 |
1000 |
0.00015 |
1000 |
0.000001 |
Click ‘OK’ to create the function
Click ‘OK’ to close the XY Function Manager form
Plot the PSD excitation function
You can use the XY Graph toolbar (
Create Response Analysis Event for a Random Excitation
· Right click on the Response
Simulation item in the Simulation Navigator and select ‘Create Event’ or use
the Create Event icon (
· Set event type to ‘Random’
· Select OK
· This will create an event item in the Simulation Navigator
· Right click on the Excitations
item and select ‘Create Translational Nodal Excitation’ or use the (
· Set the type to Enforced Motion
· Using the List Selection or Graphic Selection method, select the independent grid of the RBE2 element
o This is the only node that had an enforced motion location defines in the Response Analysis solution. It is the only item in the selection list and the only node that is selectable in the graphic display.
· Toggle off the checkbox for the
X and Z excitation functions. Using the
· Select OK
Next, apply damping to the modes of the event.
· Right click on the Normal Modes item and select ‘Edit Damping Factor’
· Specify 3% viscous damping on all modes
· Select OK
· Note: For more detailed control (activate/deactivate individual modes, specify different damping values for different modes, etc.) use the ‘Response Simulation Details View’. One or more modes can be selected using standard <Ctrl>/<Shift> list selection. Right click to modify.
Compute Response Functions for the Random Solution
· In the Simulation Navigator, right click on the event and select ‘Solve for Modal Response’.
o This will generate an event evaluation file (.eef) containing the modal response of the model to the defined input.
o Note that this step is “optional”. The Modal Response will be solved for automatically the first time you evaluate a response if this step is skipped.
· Right click on the event, then on Evaluate Function Response and pick ‘Nodal Function’.
· Set the Result Type to ‘Acceleration’
· Select the grid on the –X end of the fender at the vertex shared by 3 edges as shown below
· Set the Data Component to Y
· Toggle on Store to AFU to permanently store the response function in an external AFU file.
· Select OK
· Plot the generated response function together with the input function
· The result should look like:
Now, generate functions for elemental results such as stress.
· Right click on the event, then on Evaluate Function Response and pick ‘Elemental Function’.
· Set the Result Type to Stress
· Select an element near the center of the strut as shown below
· Set the Data Component to Von Mises
· Toggle on Store to AFU to permanently store the response function in an external AFU file.
· Select OK
A totalof 5 functions are computed and are written to the same AFU file as the nodal result. The first is the Von Mises stress at the element centroid. Each of the other four is the Von Mises stress at one of the corner nodes of the quad element.
Compute Full Field RMS Stresses for the Random Solution
The results computed previously show the response at one location over the entire frequency range. Another way to view random results is to look at the RMS response of the full structure. This is called a full field response.
· Select the Evaluate Contour
Results icon (
· Set the Result Type to Stress
· Set Selection Method to ‘By Mesh’ and click on the shell mesh to select all of the shell elements.
· Toggle on the VonMises response request
· Select OK
The RMS stress for all elements is computed at this time. The results listed in the Simulation Navigator under the Contour Results item and are written to an external .rs2 file. Right click on the RMS Stress item and select Post to view the result shown in the figure below.
Generate Equivalent Time Domain Solution
NX 5 includes a Java based palette of
Function Tools. These tools run outside of the NX environment and can operate
directly on the data in AFU files. To start the tools through NX, select
Function Tools for Response Simulation (
Select ‘PSD -> Time on the Transient or Random PSD tab
The XY function Navigator in NX now shows two functions in the fender_PSD afu file
Plot the transient function
Next, check to see if the transient function adequately captures the content of the original PSD
Note that the RMS values of both functions are very close. This indicates that the transient function has captured the content of the original PSD function
Evaluate Transient Response
Return to the Simulation Navigator and create a new transient event on the response simulation
Create a new translational nodal excitation on the enforced motion grid
Evaluate the nodal acceleration response in the Y direction at the same grid as the PSD excitation was evaluated at above.
Finally, use the Function Tools to convert this transient response back to PSD and compare to the original response.
Select the original PSD response and the TransientToPSD record and plot them together
Adjust the X axis range to 10 to 1000 Hz.
Compare the RMS values of the original PSD response and the PSD response calculated from the transient response
SHAPE\* MERGEFORMAT
AFU File Name:
fender_sim-response_simulation_1-event_1.afu
Record Number: 1
Record Name:1_(,1387Y+)_1
Function Type: Power
Spectral Density (PSD)
Max= 1.67936e+008@ Frequency =
283.63 Hz
RMS= 84214.5
Spacing:UnEven
Data Format:Real Only
Abscissa Type:
Frequency (Hz)
Ordinate Type:
Acceleration^2 (mm/sec^2)^2/Hz
Total Point Count:
276
AFU File Name:
fender_sim-response_simulation_1-event_2.afu
Record Number: 2
Record Name:ConvertedToPSD
Function Type: Power
Spectral Density (PSD)
Max= 1.70174e+008@ Frequency =
283.813 Hz
RMS= 82964.4
Spacing:Even
Data Format:Real Only
Abscissa Type:
Frequency (Hz)
Ordinate Type:
Acceleration^2 (mm/sec^2)^2/Hz
Total Point Count:
4097
The calculated PSD can be “cleaned up” by using function math operations to generate a moving average
This will create a new function (appended to the same afu file as the input) where each point is the moving average of the previous 5 points.
Plot the original PSD response and the function generated by the moving average operation
Finish
This concludes the workshop.