Process Automation for Static Analysis of Truck Chassis Assembly

Transcription

1 Process Automation for Static Analysis of Truck Chassis Assembly Haridas P.T AGM - CAE Ashok Leyland Ltd Technical Centre, Velliyoyal Chavadi Chennai Balakrishnan.M Senior Manager-CAE Ashok Leyland Ltd Technical Centre, Velliyoyal Chavadi Chennai Shashidhar.D Senior Manager-CAE Ashok Leyland Ltd Technical Centre, Velliyoyal Chavadi Chennai Selva Karunakar.S Manager-CAE Ashok Leyland Ltd Technical Centre, Velliyoyal Chavadi Chennai Abbreviations: CAE (Computer Aided Engineering), CAD (Computer Aided Design), TCL (Tool Command Language), FEA (Finite Element Analysis), CG (Centre of gravity), FAW (Front Axle Weight), RAW (Rear Axle Weight), GVW (Gross Vehicle weight), BC (Boundary Condition) Keywords: Chassis, Process automation, Macros, Solver templates, Time reduction Abstract In today s competitive world, the customer expects better products than the existing one. To meet this, there is a need to adopt fast, responsive, adaptive and innovative product development processes. Computer Aided Engineering (CAE) is one such a tool, which aids in this. This paper explains the process automation techniques employed from pre-processing stage to report generation stage during the static analysis of truck chassis assembly in CAE. These automations resulted in the reduction of cycle time, elimination of possible mistakes and result variation due to manual post processing. Introduction Frame assemblies of most heavy commercial vehicles are ladder shaped structure with side frame rails interconnected with cross members at critical locations where frame stresses are expected to be higher. These primary load carrying frame side members and cross members form an integral structure to support payload, cab, load body, power train and other chassis mounted components such as fuel tank, battery, spare wheel carrier, Air tank, Air cleaner, silencer, etc., Pre-processing and post-processing are major time consuming activities in a chassis analysis. Time reduction in pre-processing and post-processing will help us to reduce the overall analysis duration and thereby the project duration. Hence, the following improvements are made to automate the chassis analysis process. 1. Organizing of CAD model. 2. Mid surface extraction and assigning thickness using macro 3. Meshing of thin shell components & Automatic bolt creation using macro 4. Renaming of components with specific name with thickness details (for checking FE model and post processing). 5. Renumbering of specific nodes to apply Loads, Boundary conditions & extraction of output. 6. Lumped mass creation at respective CG locations using Excel worksheet and macro 7. Leaf spring suspension modeling using macro. 8. Using solver template file with include files. 9. Automatic post processing of results using advanced option in HyperView 10. Comparison of results between two chassis results using excel macro Flow chart for static analysis of truck chassis assembly The following flow chart explains the list of activities involved in static analysis of truck chassis assembly and process automations are made in the activity which is filled with "Green" colour.

2 Start Import CAD model in Hypermesh Organize the CAD parts with specific name Extract mid-surface & assign thickness using macro Meshing using macro Re-mesh NO Is the mesh quality O.K? Check the quality of the mesh YES Bolt connection using macro Assign material Renumbering of specific nodes & elements to apply Loads & BCs and to extract desired output Free - Freee normal mode analysis using Solver templatee files with include files (Mesh data) Correct the element connectivity NO Is the element connectivity O.K? Check the element connectivity by viewing the mode shapes in Hyperview A A YES Lumped mass creation using macro

3 Suspension modeling using macro Apply Loads & BC s for Vertical_1G using Solver template file with include files (Mesh data file & input variable file) Calculate FE model mass Adjust missing mass in the payload with the consent of customer NO Is that matching with GVW? Compare the FE model mass with GVW YES Solve for Vertical_1G Modify the payload CG location to match the reaction forces Extract the FEA reaction forces at ground points for Vertical_1G NO Is that matching with FAW & RAW? Compare the FEA reaction forces at ground points with FAW & RAW (given in the input sheet) YES B B

4 Apply Loads & BC s for other load cases (Vertical_3G, Braking, and Cornering & Articulation) Solve for other load cases using solver template file Extract the FEA reaction forces for other load cases Check the reaction forces for Braking, Cornering and Articulation load case Post processing using "Advanced option" in Hyperview Comparison of results between two chassis assembly using excel macro Report preparation End 1. Organizing the CAD model Organizing the CAD model with specific name will help us in checking of FE processing. Sample CAD model of chassis assembly is shown in Figure 1. model and aid in post-

5 Figure 1: Sample CAD model of Chassis assembly 2. Mid surface extraction and assigning thickness using macro This macro extracts the mid surface and assigns thickness to the components and the name of the component will look like "MID_COMPOENT-NAME_THICKNESS" as shown in Figure 2. Figure 2: Mid surface extraction and assigning thickness

6 3. Meshing of thin shell components & Automatic bolt creation using macro This macro will mesh the components with specified meshing criteria and create bolt connection between the components where there is a matching hole. Sample mesh pattern around the hole is shown in Figure 3. Sample rigid spider and beam element creation is shown in Figure 4. Figure 3: Sample mesh pattern around the hole Figure 4: Sample Rigid spider & Beam element creation

7 4. Renaming of components with specific name Once the meshing is completed, we have to rename the components with specific name for checking FE model and post processing of results. Sample component naming format is shown in Figure 5. 1 FSM 2 Internal Flitch 2 External Flitch 3 Front cross member Conventional Naming 5. Renumbering of specific nodes and elements Specific Naming Format 01_FSM_*T 02_Flitch_Int_Front_*T 02_Flitch_Int_Middle_*T 02_Flitch_Int_Rear_*T 02_Flitch_Ext_Middle_*T 02_Flitch_Ext_Rear_*T 03_Front_Xmem_Channel *T 03_Front_Xmem_Gusset_* *T 03_Front_Xmem_Stiffener *T Figure 5: Specific component naming format Standard node and element numbers are being employed to apply Loads, Boundary conditions and to extract desired outputs using solver template file. Standard nodes and elements numbering at front suspension is shown in Figure 6 and rear suspension is shown in Figure 7. NODE IDS Ground : 2 Spring Seat : 102 Bump stop : 202 Spring Bkt front : 302 Spring Bkt rear : 402 NODE IDS Ground : 4 Spring Seat : 104 Bump stop : 204 Spring Bkt front : 304 Spring Bkt rear : 404 FA1_RH FA2_RH FRONT Power train ( Engine + Gear box) NODE ID: 1001 Ram point NODE ID: 1002 FA1_LH NODE IDS Ground : 1 Spring Seat : 101 Bump stop : 201 Spring Bkt front : 301 Spring Bkt rear : 401 FA2_LH NODE IDS Ground : 3 Spring Seat : 103 Bump stop : 203 Spring Bkt front : 303 Spring Bkt rear : 403 Y-Axis X-Axis Figure 6: Node numbering at front suspension

8 NODE IDS Ground : 6 Spring Seat : 106 Bump stop : 206 Spring Bkt front : 306 Spring Bkt rear :406 RA1_RH NODE IDS Ground : 8 Spring Seat : 108 Helper spring mid node : 208 Spring Bkt front : 308 Spring Bkt rear : 408 FSM Bump Stop Spring Bottom node1 : 508 FSM Bump Stop Spring Bottom node2 : 708 FSM Bump Stop Spring Bottom node3 : 808 Bump stop node on Axle : 608 ELEMENT IDS Helper spring Bush : 2008 (F), 3008 (R) FSM Bump stop Spring1 : 5008 FSM Bump stop Spring2 : 7008 FSM Bump stop Spring3 : 8008 RA2_RH Hinge_RH NODE ID: 1004 NODE ID: 1003 Hinge_LH RA1_LH NODE IDS Ground : 5 Spring Seat : 105 Bump stop : 205 Spring Bkt front : 305 Spring Bkt rear : 405 RA2_LH NODE IDS Ground : 7 Spring Seat : 107 Helper spring mid node : 207 Spring Bkt front : 307 Spring Bkt rear :407 FSM Bump Stop Spring Bottom node1 :507 FSM Bump Stop Spring Bottom node2 :707 FSM Bump Stop Spring Bottom node3 :807 Bump stop node on Axle : 607 ELEMENT IDS Helper spring Bush: 2007 (F), 3007 (R) FSM Bump stop Spring1: 5007 FSM Bump stop Spring2: 7007 FSM Bump stop Spring3: 8007 Figure 7: Node numbering at rear suspension

9 6. Lumped mass creation at respective CG locations using Excel worksheet and macro This macro will create lumped mass of Payload and other aggregates at respective CG locations. FE model after lumped mass creation is shown in Figure 9. STEPS TO USE THE MACRO 1) Enter X, Y, Z coordinates of reference point in respective cells as shown in Figure 8. 2) Enter the description of each aggregate in Column B 3) Enter mass of each aggregate (in Tonnes) in column C 4) Enter X, Y, Z coordinates (in mm) of the aggregates in respective cells. 5) Press button "Run. A new *.tcl file will be created in C drive (C:\CGmass.tcl) 6) Execute C:\CGmass.tcl in HM to create lumped masses and corresponding tags. Figure 8: Lumped mass creation data from inputs Figure 9: FE model after lumped mass creation

10 7. Leaf spring suspension modeling using macro This macro will create beam element representation of leaf springs with shackle at specified locations. FE model after leaf spring modeling using macro is shown in Figure 11. Figure 10: Inputs for Leaf spring modeling Figure 11: FE model after Leaf spring modeling

11 8. Using solver template file with include files Solver template will help the analyst to apply loads, boundary conditions and to extract desired outputs (Displacements, Stress, SPC forces, MPC forces, BUSH element forces, etc.,). Using the template files will reduce mistakes due to manual application of loads & BC's and also reduces FE model review time. Figure 12: Portion of sample solver template file 9. Automatic post processing of results using advanced option in HyperView This option will help the analyst to post process the desired results. Steps for advanced post processing are explained below 1. Click the icon Contours to view the stress and displacements. 2. Select Stress [t] and vonmises options under Result type to view the vonmises stress results. 3. Select the Elements or Components under selection icon. 4. Click Apply. 5. Select Query Results to extract the plots in h3d format

12 On Clicking Query Results option, the following window will open. Click the Advanced option The html file will be having component wise results with a hyperlink to respective h3d files for all the loading conditions. Sample view of html file which comes out of the above mentioned post-processing option is shown in Figure 13.

13 Figure 13: Sample view of results HTML file 10. Comparison of results between two chassis results using excel macro Steps to be followed to compare follows. the results between two frames using Excel spreadsheet macro is as 1. Open the excel spreadsheet for comparing the results between two frames as shown in Figure Update the name of vehicle1 and vehicle2 in the Nomenclature tab 3. Enter the number of load cases to be compared. 4. Open the html file of Vehicle-1,copy all the contents and paste it in VEH1_RES sheet. 5. Open the html file of Vehicle-2,copy all the contents and paste it in VEH2_RES sheet. 6. Go to Nomenclature sheet and execute "Vehicle 1","Vehicle 2" and "Summary" macros to get the consolidated and summary results as shown in Figure 15.

14 Figure 14: Comparison of results - Nomenclature Figure 15: Comparison of results - Summary

15 Benefits Summary Pre-processing time reduction and elimination of manual errors using macros Extraction of mid surface and assigning thickness (Time reduction: 4 hrs to 10 min) Meshing of thin shell components (Time reduction: 56 hrs to 24 hrs) Automatic bolt creation (Time reduction: 8 hrs to 15 min) Lumped mass creation at respective CG locations (Time reduction: 2 hrs to 5 min) Leaf spring suspension modeling (Time reduction: 10 hrs to 30 min) Pre-processing technical review (Time reduction: 8 hrs to 3 hour) Solver template file (Time reduction: 4 hrs to 5 min) Post-processing and comparison of results using macros (Time reduction: 16 hrs to 3 hour) Challenges Time reduction in overall Chassis analysis without compromising on the quality of results Standardization of component names, analysis deck and output requests Comparison of results between two chassis assemblies with hyperlink to result plots. Conclusions Major time consuming activity in chassis analysis process has been automated using macros which helped us to reduce the overall analysis duration by 70%. Macros created during this process automation exercise has been deployed horizontally across all the Truck chassis analysis carried out in AL, which has helped the designer to carry out many iterations and to get consistent results. ACKNOWLEDGEMENTS The authors thank the management of Ashok Leyland, Head-CAE and ALTAIR for having provided opportunity to present the work reported in this paper. The authors also thank our CAE team members at Ashok Leyland Technical centre for their continuous support in executing this process automation. Hyper Mesh User Manual, Altair Engineering Practical Programming in TCL and TK, Brent Welch REFERENCES