Detailed Risk and Root Cause Analysis

Use SnRD to identify, evaluate, and eliminate squeak and rattle issues.

During the first S&R screening risk analysis, several input data were 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 analysed:
  • 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 search for and applied for relevant E-lines.
    • The stick slip data available in different sources (Ziegler data base, own data base etc.) can be imported into SnRD for update of existing model.
The objectives of this tutorial are:
  • Create FE model prepared for analyzing.
    • Create E-Lines using Auto & Manual methods-
      • 6 Rattle lines
      • 2 Squeak lines
  • 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. Import a Model.
  2. Click to open additional options.
    Figure 1.
  3. Using the file browser option, browse and select files for respective entries mentioned in the Detailed Risk and Root Cause Analysis.
  4. Click Import.
    The selected model, DTS, and material file are imported to the session.
    Figure 2.

Import Geometric Lines File

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

  1. From Setup group, select Define Interface > Import Geometry File.
    Figure 3.
    A file browser dialog opens.
  2. Browse and select the GeometricLines.stp file.
    The geometry lines file is imported into the session.
    Figure 4.

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 In plane 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 IP Substrate Control Panel Upper 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 Rattle In plane to Main Lower Control Panel IP Substrate IPsubstrate_To_Controlpanellower
Manual Squeak Normal to Main Speedometer Control Panel Upper Speedometer_To_ControlPanelUpper
Create E-Lines manually.
  1. From the Setup group, select the Create E-Line tool.
    Figure 5.
    A guide bar opens.
  2. Deactivate to manually create E-Lines.
  3. For Main Components, select IP Substrate.
  4. For Secondary, select Glove Box.
    Tip: Press Tab to toggle between selections.
  5. For Lines, 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 6.
  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 7.
Figure 7.

Realize E-Lines

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

  1. From the Setup group, select Manage E-Lines > Review E-Lines tool.
    Figure 8.
    The Review E-Line table 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 9.
    1. Optional: If an E-Line status is yellow, click to realize and update E-Lines.
  3. Go to the Material Mapping tab and 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.

Define Dynamic Loadcase

In this step, you will create a Dynamic loadcase.

  1. From Setup group, select Dynamic Event.
    Figure 10.
  2. From the graphics area, select the node shown in Figure 11.
    Figure 11.
    A microdialog opens.
    Figure 12.
  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. Click .
    A file browser dialog opens.
  7. 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.
  8. In the Curve Editor dialog, review the load curves and close the dialog.
    Figure 13.
    Figure 14.
    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 Analyze group, select Review All Loadcase.
    Figure 15.
    The Load Step Table dialog opens.
    Figure 16.
  2. Verify the Export checkbox is enabled for the SnRD_Dyn_Disp_#_XYZ entry.
  3. Click Close.
  4. From the Analyze group, select Export OptiStruct Solver File.
    Figure 17.
    The Model Export dialog opens.
    Figure 18.
  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.

Import Model and Results File

In this step, you will use the SnRD Post to post process the results.

  1. Open HyperView.
  2. From the menu bar, click File > Load > Preferences File.
    The Preferences dialog opens.
  3. In the Preferences dialog, select Squeak & Rattle and click Load.
    The SnRD menu is opened in the HyperView client.
  4. Select SnRD > SnRD-Post.
    The SnRD Post Processing tool opens.
    Figure 19.
  5. Using the file browse option , select the OptiStruct solver file which was exported in Export OptiStruct Solver File for Model File.
    Note: Pre output CSV file containing the E-Lines definition is sourced automatically.
  6. Click .
    A file browser dialog opens.
  7. Select the tutorial_ip_snr_model.pch file from the tutorials folder.
    A working status dialog opens while reading the PCH data.
    Figure 20.
  8. Enable the checkbox for the subcase in the Subcase selection table.
  9. Click in the Save Session File entry field.
  10. Browse and select the required folder where the post processing session and data will be stored.
    Once complete, your entries in the table should match Figure 21.
    Figure 21.

Post Process Results

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

  1. In the Post Processing tab, define the following parameters.
    1. For Analysis Type, select Rattle & Squeak.
    2. For Line(s) to Evaluate, select All.
    3. For % statistical evaluation, enter 0.
    4. For Session Type, select Full Analysis.
  2. Click Execute.
    Note: Execution of Full Analysis will take a considerable amount of time to chart histograms and plot contours based on the machine's performance.
    An execution success message opens.
    Figure 22.
  3. Click Close.
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
Summary for Squeak analysis can be found on Page nine.
Figure 24. 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 five to view the Rattle Detailed Dynamic - Line ID 19513009 details.
    Figure 25.
    The Relative Displacement of 1.85915 mm at the point 19513001. 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. Click the Sensitivity Analysis tab.
  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 19513009.
    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 26.
    Once complete, the relative displacement plots for all the points in the line are plotted.
    Figure 27.
  6. Under the Modal Contribution panel, click Analyze.
    A working dialog opens stating the process of plotting Relative Modal Contribution.
    Figure 28.
    Relative Modal Contribution - Line 19513009 - z is created with modes, contour and relative displacement plots for the line.
    Figure 29.
    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 30.
  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 31.
    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.