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 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 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.
Objective
  • 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.
Starting Point
  • Clean FE model- no SnRD information.
Below is an illustration of the workflow-
Figure 1.
In this usecase, you will perform the following steps-
  1. Import tutorial model, user defined DTS, material and geometric lines definition file,
  2. Create and realize E-Lines.
  3. Create Dynamic event and export solver deck.
    • Solve the .FEM solver deck to obtain results and files.
  4. Use the solver deck, E-Lines definition file and to post process results.
    • Generate histograms, contour plots, etc.
  5. Evaluate and eliminate Squeak and Rattle issues at the interfaces.
    • Perform sensitivity analysis and modal participation study.

Files Required

Files required to complete the usecase.

You will use below set of files for the following usecase:
  1. ...\hwdesktop\demos\snr\001_model- contains the model and geometric lines file,
  2. ...\hwdesktop\demos\snr\002_dts_and_material_data- contains the DTS and material data file,
  3. ...\hwdesktop\demos\snr\003_loads- contains the load definition files.

Step 1: Import Model, DTS and Material File

Use Import to import files to begin.

Using the Import task, you will import the required set of files.

Below are the steps to import files model, DTS and material files-

  1. Import a Model.
  2. Click to open additional options.
    Figure 2.
  3. Using the file browser option, browse and select files for respective entries mentioned in the Files required section.
  4. Click Import.
    This will import the selected model, DTS and material file to the session.
    Figure 3.

Step 2: Import Geometric Lines File

Below are the steps to import geometric lines file.

  1. From Setup group, select Define Interface > Import Geometry File.
    Figure 4.
  2. A file browser window will appear. Browse and select GeometricLines.stp file.
    This will import the geometry lines file into the session.
    Figure 5.

Step 3: Create, Manage and Review E-Lines

Create E-Lines at the interfaces of the imported geometry lines file.

Create E-Lines

Use Create E-Lines tool to create E-Lines at the interfaces. Tabulated below are the E-Lines that you will create in this step-

Method Line Type Gap Direction Master Component Slave Component Interface Name
Fast Rattle In plane to master IP Substrate Glove Box GloveBox_To_IPsubstrate
Fast Squeak In plane to master IP Substrate Dashboard Panel Ipsubstrate_To_Dashboardpanel
Manual Rattle In plane to master IP Substrate Control Panel Upper IPsubstrate_To_ControlpanelUpper
Manual Rattle Normal to Master Radio Panel Lower Control Panel Radiopanel_To_ControlPanelLower
Manual Rattle In plane to Master Driver Side Panel Lower Control Panel DriverSidepanel_To_Controlpanellower
Manual Rattle In plane to Master Driver Side Panel IP Substrate DriverSidepanel_To_IPsubstrate
Manual Rattle In plane to Master Lower Control Panel IP Substrate IPsubstrate_To_Controlpanellower
Manual Squeak Normal to Master Speedometer Control Panel Upper Speedometer_To_ControlPanelUpper

Fast Create

  1. From Setup group, select Create E-Line tool.
    Figure 6.
    A guide bar will appear.
  2. Select IP Substrate and Glove Box for Components option.
    Tip: Use Tab button to toggle options.
  3. Select the geometric line present at the edge of the Glove Box component for Lines option.
  4. Click .
    This will create the E-Linesat the interface and same will be highlighted in yellow color.
    Figure 7.
  5. Repeat the above step to create Squeak line between IP Substrate and Dashboard Panel.

Manual Create

  1. Deactivate to manually create E-Lines.
  2. Select In Plane to Master.
  3. Select IP Substrate and Control Panel Upper for Master and Slave options.
  4. Select the geometric line at the edge of Control Panel Upper component for Lines option.
  5. Click .
    This will create the E-Lines at the interface and same will be highlighted in yellow color.
  6. Repeat the above steps to create the remaining E-Lines tabulated above.
    Your model should be as shown below after creating all the E-Lines.
    Figure 8.

Realize E-Lines

Use Manage E-Lines tool to realize all the E-Lines.

  1. From Setup group, select Manage E-Lines tool.
    Figure 9.
  2. Click .
    Note: Components between which the interfaces are defined are only isolated in the graphics area.
    This will realize all the E-Lines in the model.
    Figure 10.
  3. From Setup group, select Manage E-Lines > Review E-Lines tool.
    Figure 11.
    Review E-Line table will appear.
    Figure 12.
  4. For the squeak lines, select following materials for master and slave materials-
    1. Master Material
      PPTD_20
      Slave Material
      PPTD_20
    2. Master Material
      PPTD_20
      Slave Material
      ABS

Step 4: Dynamic Event Definition and Export

Create a Dynamic event at the prescribed node.

Define Dynamic Loadcase

Below are the steps to create a Dynamic loadcase.

  1. From Setup group, select Dynamic Event.
    Figure 13.
  2. From the graphics area, select the node shown in the below image.
    Figure 14.
    A microdialog will appear.
    Figure 15.
  3. Select D- displacement.
  4. Select From File for Load Curve.
  5. Select X, Y and Z for load directions.
  6. Click .
    A file browser window will appear. Browse and select the Excitation_XYZ.csv file from003_loads folder.
    This will create the required load collectors and other entities required for the simulation. You can view the model browser for the new entities that are created.
    Figure 16.
  7. The newly created loads are displayed in the Curve Editor. Review the load curves and close the window.
    Figure 17.

Review Loadcase and Export Solver Deck

Review the Dynamic Loadcase.

  1. From Analyze group, select Review All Loadcase.
    Figure 18.
    Load Step Table will appear.
    Figure 19.
  2. Make sure Export box is checked against SnRD_MTRAN_EnforcedDisplacement_1_XYZ entry. Click Close.

Export Solver Deck

  1. From Analyze group, select Export OptiStruct Solver File.
    Figure 20.
  2. Model Export window will appear.
    Figure 21.
  3. Click Export.
    A folder selection window will appear.
  4. Browse and select the required folder.
    This will export the OptiStruct solver deck to the selected folder. Click Close to close the model export option.
Use the exported .FEM solver deck to solve on OptiStruct solver. Once done, two output files are generated: .H3D and .PCH. These files will be used in the Post Processing of results.

Step 5: Post Process results

Results post processing.

Import model and results file

Use the SnRD Post to post process the results.

Launch HyperWorks X, switch to HyperView client. Select File > Load > Preferences File. Preferences window will appear. Select Squeak & Rattle and click Load. This creates SnRD menu in the HyperView window.

  1. Select SnRD > SnRD-Post.
    SnRD Post Processing tool is launched.
  2. Using the file browse option , select the OptiStruct solver file which was exported in Step 4 for Model File.
    Note: Pre output CSV file containing the E-Lines definition is sourced automatically.
  3. Click .
    A file browser window will appear. Select tutorial_ip_snr_model.pch from tutorials folder.
    A working status window will appear while reading the PCH data.
    Figure 22.
  4. Check the box against the subcase in Subcase selection table.
  5. Click in the Save Session File entry field.
    Browse and select the required folder where the post processing session and data will be stored.
    Once done, your entries in the tab should be as below-
    Figure 23.

Post Process

Perform Full Analysis to understand the Squeak and Rattle risks in the model.

  1. In the Post Processing tab, define the following-
    Analysis Type
    Rattle & Squeak
    Line(s) to Evaluate
    All
    % statistical evaluation
    0
    Session Type
    Full Analysis
  2. Click Execute.
    A working window will appear stating the Compose batch execution.
    Figure 24.
    Note: Execution of Full Analysis will take considerable time to chart histograms and plot contours based on the machine's performance.
    Execution success message will appear once done. Click Close to close the window.
    Figure 25.
Full analysis creates 11 pages containing all the details. The summary for Rattle analysis is placed in Page 1.
Figure 26. Rattle Summary Dynamic
Summary for Squeak analysis is placed in Page 9.
Figure 27. Squeak Summary Dynamic

Step 6: Result analysis and evaluation

Study the histograms and contour plots to understand results.

Results Evaluation

Squeak and Rattle risk evaluation.

From the Page 1 Rattle Summary Dynamic, it can be observed that the Rattle line ID 19513009 has the maximum relative displacement. You will perform the Sensitivity Analysis to evaluate the effects of modes on the relative displacements.
  1. Navigate to Page 5to view the Rattle Detailed Dynamic - Line ID 19513009 details.
    Figure 28.
    It can be observed that 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 on Sensitivity Analysis tab.
  3. Define the following in the tab-
    Result File
    Tutorial_IP_SNR_Model.pch
    Subcase Name
    Subcase 4 (SnRD_MTRAN_EnforcedDisplacement_1_XYZ)
    Modal Result File (.H3D)
    Tutorial_IP_SNR_Model.h3d
  4. Define the following in E-Line Selection section-
    E-Lines
    19513009
    Select Pair
    Line check box
    Select Direction
    Z
  5. Click Load Time History.
    A working window will appear stating the process of plotting relative displacement.
    Figure 29.
    Once done, the relative displacement plots for all the points in the line are plotted.
    Figure 30.
  6. Under Modal Contribution panel, keeping the default values, click Analyze.
    A working window will appear stating the process of plotting Relative Modal Contribution.
    Figure 31.
    Relative Modal Contribution - Line 19513009 - z will be created with modes, contour and relative displacement plots for the line.
    Figure 32.
    From the Modes plot, it can be observed that the Mode-4 of value 26.5 Hz is the highest contributing factor for the rattle issue.
  7. Click Modal Sensitivity nuder Modal Sensitivity Studies panel.
    Figure 33.
  8. Select Exclude from Select Contributor(s) to list.
  9. Enter 50 for % to Exclude value.
  10. Check the box against mode 4 under Mode # column.
  11. Click Analyze.
    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 34.
    It can be observed that the relative displacement is reduced when the mode 4 is excluded by 50%.
    Repeat above steps to study the remaining lines in the model.
This concludes the Advanced or Expert Analysis usecase.