Detailed Risk and Root Cause Analysis

In this tutorial, you will use SnRD to identify, evaluate, and eliminate squeak and rattle issues.

During the first squeak and rattle screening risk analysis, input data was lacking for the different interfaces. At that time, no gap or material properties were defined yet. Now, the design team has more information for each of the E-Lines that have been analyzed:
  • Rattle lines:
    • The gap and tolerances are now defined from the styling and engineering departments.
    • These dimensions can now be imported into SnRD and used for updating the existing model.
  • Squeak lines:
    • Material choices are more mature, therefore the stick slip testing data can be searched for and applied for relevant E-Lines.
    • The stick slip data available in different sources (Ziegler data base, own data base, and so on) can be imported into SnRD for updating an existing model.
The objectives of this tutorial are:
  • Create FE model prepared for analyzing.
    • Create E-Lines using automatic and manual methods: six rattle lines and two squeak lines.
  • Create a dynamic loadcase, with user defined multi direction loading data.
  • Run analysis, post process, and perform sensitivity study.
Before you begin, copy the file(s) used in this tutorial to your working directory:
Contains the model and geometric lines file.
Contains the DTS and material data file.
Contains the load definition files.

Import Model, DTS, and Material File

In this step, you will use the Import tool to import the required files.

  1. From the HyperMesh NVH menu bar, select Squeak and Rattle.
    The SnRPre and SnRPost ribbons open.
  2. From the SnRPre ribbon, select the Import tool.
    Figure 1.


  3. Click to open additional options.
    Figure 2.
  4. Using the file browser option, browse and select files for respective entries.
  5. Click Import.
    The selected model, DTS, and material file are imported to the session.
    Figure 3.

Import Geometric Lines File

In this step, you will import the geometric lines file.

  1. From SnRPre ribbon, select the Import Geometry tool from the Define Interface tool group.
    Figure 4.
    A file browser dialog opens.
  2. Browse and select the GeometricLines.stp file.
    The geometry lines file is imported into the session.
    Figure 5.

Create E-Lines

In this step, you will use the Create E-Lines tool to create E-Lines at the interfaces.

Below are the E-Lines you will create in this step.
Table 1.
Method Line Type Gap Direction Main Component Secondary Component Interface Name
Manual Rattle Normal to Main IP Substrate Glove Box GloveBox_To_IPsubstrate
Manual Squeak In plane to Main IP Substrate Dashboard Panel Ipsubstrate_To_Dashboardpanel
Manual Rattle In plane to Main Control Panel Upper IP substrate IPsubstrate_To_ControlpanelUpper
Manual Rattle Normal to Main Radio Panel Lower Control Panel Radiopanel_To_ControlPanelLower
Manual Rattle In plane to Main Driver Side Panel Lower Control Panel DriverSidepanel_To_Controlpanellower
Manual Rattle In plane to Main Driver Side Panel IP Substrate DriverSidepanel_To_IPsubstrate
Manual Squeak Normal to Main Speedometer Control Panel Upper Speedometer_To_ControlPanelUpper
Create E-Lines manually.
  1. From the SnRPre ribbon, select the Create E-Line tool.
    Figure 6.
    A guide bar opens.
  2. From the guide bar, select Manual.
    By selecting the manual method, more options to create E-Lines in a more controlled manner become available on the guide bar, see Figure 7. You must select the Main and Secondary components based on the interface, and in which direction the local z-axis will be oriented. However, you can select only one geometric line at a time, based on the interface of interest.
    Figure 7.


  3. For Main, select IP Substrate.
  4. For Secondary, select Glove Box.
    Tip: Press Tab to toggle between selections.
  5. For Line, select the geometric line present at the edge of the Glove Box component.
  6. Click .
    E-Lines are created at the interface and will be highlighted in yellow.
    Figure 8.
  7. Repeat the substeps above to create a squeak line between the IP Substrate and Dashboard Panel.
Once all E-Lines are created, your model should look like Figure 9.
Figure 9.

Realize E-Lines

In this step, you will use the Manage E-Lines tool to realize all E-Lines.

  1. From the SnRPre ribbon, select the Review E-Lines tool from the Manage E-Line tool group.
    Figure 10.
    The Review E-Line dialog opens.
  2. Map the correct interface from the DTS file to the created E-Lines and ensure all other options, like Gap direction, are correct.
    Figure 11.


    Note: The E-Line status is represented using three colors:
    • Red indicates a failed E-Line.
    • Yellow indicates an unrealized E-Line.
    • Green indicates a fully realized E-Line.
    1. Optional: If an E-Line status is yellow, click to realize and update E-Lines.
  3. From the Material Mapping tab, select the following materials for the two squeak E-Lines.
    1. IPSubstrate_To_Dashboardpanel
      • For Main Material, select PPTD_20.
      • For Secondary Material, select PPTD_20.
    2. Speedometer_To_ControlPanelUpper
      • For Main Material, select PPTD_20.
      • For Secondary Material, select ABS.
    Tip: In the Review E-Line dialog, click to connect to Ziegler Database and map materials. See Ziegler PEM Material Database for more information.
    Figure 12.


Define Dynamic Loadcase

In this step, you will create a Dynamic loadcase.

  1. From SnRPre ribbon, select the Dynamic Event tool.
    Figure 13.
  2. In the modeling window, select the node shown in Figure 14.
    Figure 14.
    A microdialog opens.
    Figure 15.
  3. Verify Displacement (D) is selected as load type.
  4. For Load Curve, select From File.
  5. For load directions, select X, Y, and Z.
  6. Select Constrain all Dofs to constrain the excitation nodes in all the other directions.
  7. Click .
    A file browser dialog opens.
  8. Browse and select the Excitation_XYZ.csv file from the 003_loads folder.
    The required load collectors and other entities required for the simulation are created. The newly created loads are displayed in the Curve Editor dialog.
  9. In the Curve Editor dialog, review the load curves and close the dialog.
    Figure 16.
    Figure 17.
    Tip: You can use the Model Browser to view the new entities.

Review Loadcase and Export Solver Deck

Review the Dynamic Loadcase.

  1. From the SnRPre ribbon, Analyze group, select the Review Loadcases tool.
    Figure 18.
    The Load Step Table dialog opens.
    Figure 19.
  2. Verify the Export checkbox is enabled for the SnRD_Dyn_Disp_#_XYZ entry.
  3. Close the dialog.
  4. From the SnRPre ribbon, Analyze group, select the Export tool.
    Figure 20.
    The Model Export dialog opens.
    Figure 21.
  5. Click Export.
    A folder selection dialog opens.
  6. Browse and select the required folder.
    The OptiStruct solver deck is exported to the selected folder.
  7. Click Close to close the Model Export dialog.
Use the exported .FEM solver deck to solve in the OptiStruct solver. Once completed, two output files are generated: .H3D and .PCH. These files will be used in the Post Processing of results.

Post Process Results

In this step, you will perform a Full Analysis to understand the squeak and rattle risks in the model.

  1. From the SnRPost ribbon, select the Risk Assessment tool.
    Figure 22.


    The SnR Risk Assessment Browser opens.
  2. For Result File, select the .pch file.
    Note: Prior to selecting the .pch file, the .fem and .csv file must already be loaded in the SnRPre ribbon.
  3. Under Subcase Selection, select the subcase.
    The rattle and squeak lines are segregated into separate tabs.
  4. Select the line Ids required to perform post-processing.
  5. For SEP, enter 0.
  6. Verify Full Analysis is selected to see the line-level plots and to continue to next steps of post-processing.
    Important: You must perform full analysis to access Sensitivity Analysis and combined loading capabilities.
    Note: If Full Analysis is not selected, only a summary analysis is generated. Full Analysis is selected by default.
  7. Click Plot.
Seven pages are created containing the details and summary for rattle analysis. You must switch to the squeak tab and select the lines for squeak results.
Full analysis creates 11 pages containing all the details. The summary for rattle analysis can be found on page one.
Figure 23. Rattle Summary Dynamic

To access squeak results, you must click on the squeak tab and click Plot. The plots in sequence are as shown below:

Maximum Peak-to-peak Displacement plot:

Minimum Peak-to-peak Displacement plot:

Maximum P-P Displacement bar plot.

To visualize P-P displacement in comparison with the Impulse rate data from testing, you should access advanced squeak capabilities.
Figure 24.


Figure 25. Squeak Summary Dynamic

Evaluate Results

In this step, you will study the histograms and contour plots to understand results and complete squeak and rattle risk evaluation.

From page one of the Rattle Summary Dynamic, you can see the Rattle line ID 19513009 has the maximum relative displacement. You will perform Sensitivity Analysis to evaluate the effects of modes on the relative displacements.
  1. Navigate to page six to view the Rattle Detailed Dynamic - Line ID 70009 details.
    Figure 26.
    The Relative Displacement of 0.86 mm at the point 70001. This is higher than the Gap and (Gap - Tolerance) values. This indicates a risk of rattle at this particular interface of Driver Side Panel - Lower Control Panel.
  2. From the SnRPost ribbon, select the Sensitivity Analsysis tool.
    Figure 27.


    The SnR Sensitivity Analysis Browser opens.
    Figure 28.


  3. Define the following parameters.
    1. For Result File, select Tutorial_IP_SNR_Model.pch.
    2. For Subcase Name, select Subcase 4 (SnRD_MTRAN_EnforcedDisplacement_1_XYZ).
    3. For Modal Result File (.H3D), select Tutorial_IP_SNR_Model.h3d.
  4. In the E-Line Selection section, define the following parameters.
    1. For E-Lines, select 70009.
    2. For Select Pair, select Line check box.
    3. For Select Direction, select Z.
  5. Click Load Time History.
    A working window opens stating the process of plotting relative displacement.
    Figure 29.
    Once complete, the relative displacement plots for all the points in the line are plotted.
    Figure 30.
  6. Under the Modal Contribution panel, click Analyze.
    A working dialog opens stating the process of plotting Relative Modal Contribution.
    Figure 31.
    Relative Modal Contribution - Line 70009 - z is created with modes, contour and relative displacement plots for the line.
    Figure 32.


    Figure 33.
    From the Modes plot, the Mode-4 of value 26.5 Hz is the highest contributing factor for the rattle issue.
  7. Click Modal Sensitivity under the Modal Sensitivity Studies panel.
    Figure 34.
  8. Select Exclude from the Select Contributor(s) to list.
  9. Enter 50 for % to Exclude value.
  10. Enable the checkbox for mode 4 under the Mode # column.
  11. Click Analyze.
    The Modal Sensitivity for Line (MSL) - Line ID 19513009 -z page is created in the session with the Max Relative Displacement (mm) values plotted against all the interface points.
    Figure 35.
    The relative displacement is reduced when the mode 4 is excluded by 50%.
  12. Repeat the above steps to study the remaining lines in the model.