Thermal Effects (Combined) Analysis

Evaluate squeak and rattle issues when exposed to thermal loading.

A typical challenge faced in the automotive industry is how does the vehicle interior perform under driving conditions while the vehicle has been parked in the sun for many hours?

To answer this question, vibration loads responses (Dynamics) need to be superposed to the temperature effect on parts (Thermal Expansion – Static), gaps are reduced for example. In this workflow, the user will evaluate the squeak and rattle issues in a dynamic condition where the vehicle, in this case, a parked under sunlight with a spike in internal temperature (Static loadcase). Later the car is driven, which is exposed to Dynamic Loading. Below is the illustration of the Driving Vehicle exposed to the Thermal Effects (Combined Loading) workflow.
Below is an illustration of the workflow that shall be covered in this usecase:
Figure 1.
Objective
  • Prepare the FE model for analyzing Squeak and Rattle issues.
  • Apply a static load of amplitude -5.55 to the certain node(s) on Lower Control Panel component. This simulates a touch point scenario.
  • Run analysis and post-process the results.
Starting Point

Choose the workflow according to your need and refer to sections mentioned above for the procedures.

Files Required

Files required to complete the usecase.

Use the solver deck exported from Detailed Risk and Root Cause Analysis usecase.
Once you import the Dynamic Loadcase solver deck, you can proceed with Thermal (Static) Loadcase setup.

Step 5: Thermal Event Definition and Export

Apply thermal loading on the top surface of the IP Substrate and Dashboard Panel.

Define Thermal Loadcase

Below are the steps to create thermal loadcase.

  1. From Setup group, select drop down arrow next to Dynamic > Thermal Event.
    Figure 2.
    A guide bar will appear.
  2. Select the nodes on the top surface of the IP Substrate and Dashboard Panel components.
    Figure 3.
  3. Enter 90 for the temperature value in the microdialog.
  4. Click .
    This creates the Thermal loadcase with the load collectors and other entities required for the simulation. Respective load collectors get created and are assigned to the loadstep.
    An user message will appear. Click OK to proceed.
    Figure 4.

Define Constraint

Below are the steps to define model constraints.
  1. In the Setup ribbon, select Static Event > Setup Constraints.
    Figure 5.
    A guide bar will appear.
  2. From the graphics area, select the node shown in the below image.
    Figure 6.
  3. In the microdialog, select SnRD_STATIC_Temperature_1 for the Loadstep option.
  4. Select all degrees of freedom.
    Figure 7.
  5. Click .
    This creates the Static loadcase with the load collectors and other entities required for the simulation. Respective load collectors get created and are assigned to the loadstep.

Export OptiStruct Solver File

  1. From Analyze group, select Export OptiStruct Solver File.
    Figure 8.
  2. Model Export window will appear.
    Figure 9.
  3. Click Export.
    A folder selection window will appear.
  4. Browse and select the required folder.
    This will export the OptiStruct solver deck file 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 6: Post Processing and Results Evaluation

In the workflow, you will first analyze the Squeak and Rattle issues for the Dynamic loading and then evaluate the thermal effect on the issues.

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.
    Figure 10.
  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 and Tutorial_IP_SNR_Model.h3d from tutorials folder.
    A working status window will appear while reading the H3D data.
  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 11.

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 12.
    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 13.
Full analysis creates 22 pages containing all the details. The summary for Dynamic Loadcase Rattle analysis is placed in Page 1.
Figure 14. Rattle Summary Dynamic
Summary for Dynamic Loadcase Squeak analysis is placed in Page 8.
Figure 15. Squeak Summary Dynamic
Summary for Thermal Loadcase Rattle analysis is placed in Page 12.
Figure 16. Rattle Summary Thermal
Summary for Thermal Loadcase Squeak analysis is placed in Page 19.
Figure 17. Squeak Summary Thermal

Combined Loading

Perform a Combined Loading study to understand the thermal effects on the squeak and rattle issues under Dynamic Loading condition.

  1. Select Combined Loadings tab.
    Figure 18.
  2. Select dynamic loadcase from Loading Type 1 drop down list.
    This disables the Affects Gap for loading type 1.
  3. Thermal loadcase selected by default for Loading Type 2.
  4. Select Summary Analysis radio button.
    Summary Analysis creates a summary for the combined loading effects on all E-Lines.
  5. Click Combine Results.
    The Combined Loading summary page is created.
    Figure 19.
    Considering the 19513009 E-Line, the following observation that can be made for the study-
    • The Relative Displacements has increased from 1.83 mm to 2.09 mm under thermal effect.
  6. Check Affects Gap against Loading Type 2 list.
  7. Select 19513009 from E-Line(s) Selection list.
  8. Select Full Analysis radio button.
  9. Click Combine Results.
    The combined effect on the selected interface is plotted in the results page.
    Figure 20.
    Below are the changes that can be observed from the plots-
    1. NewGap_Nominal_LC5_R2_Z and NewGap_Tolerance_LC5_R2_Z are introduced in the analysis. These are the changes in gap and tolerance due to thermal effects.
    2. It can also be observed that the relative displacement has reduced from 2.09 mm to 1.83 mm. This analysis states that the thermal effects has reduced the relative displacement, in turn leading to reduced rattle noise.