workbench材料属性

nullWorkshop 5 Circuit Board Drop TestWorkshop 5 Circuit Board Drop TestANSYS Explicit DynamicsWorkshop Goal and Procedure Workshop Goal and Procedure Goal: Simulate the bonded/breakable contacts in the drop test simulation of a circuit board Procedure: Create an Explicit Dynamics (ANSYS) Analysis System Project Select the units system and define the material properties Import, view, and mesh the circuit board geometry Define analysis settings, boundary condition, and initial condition Initiate the solution (AUTODYN - STR) and review the resultsStep 1 – Create the Project SchematicStep 1 – Create the Project SchematicStart ANSYS Workbench and follow the sequenced steps using the abbreviations shown below: DC = Double Click with Left Mouse Button SC = Single Click with Left Mouse Button CtrlSC = Single Click with Left Mouse Button while press Ctrl key RMB = Right Mouse Button SelectionDC1. Create an ANSYS Explicit Dynamics Analysis System ProjectStep 2 – Specify the Project UnitsStep 2 – Specify the Project Units2.a Select MKS for the Project Units from the Units List provided 2.b Request that Native Applications in Workbench have their values be Displayed in the Project Units 2.c Check those unit systems to Suppress from appearing in the Units List Note: Engineering Data is native in Workbench, but Mechanical is NOT at this time (but will be in the future).Step 3 – Define Engineering Data MaterialStep 3 – Define Engineering Data Material3.a Edit the Engineering Data cell to add materials to the current model. 3.b Select Engineering DataSC3.d Enter the material name: “PCB”DCSC3.c Select the last slot to define a new material. Step 3 – Define Engineering Data Material ...DCDCDCStep 3 – Define Engineering Data Material ...3.f Add the following Physical Properties to the material definition: Density Isotropic Elasticity Bilinear Isotropic Hardening Plastic Strain Failure 3.e Make sure the new material is active in order to define its properties DCStep 3 – Define Engineering Data Material ...Step 3 – Define Engineering Data Material ...3.g Enter the following values: Density = 1100 kg m^-3 Young’s Modulus = 2.21E9 Pa Poisson’s Ratio = 0.30 Yield Strength = 8.0E7 Pa Tangent Modulus = 2.21E8 Pa Maximum Plastic Strain = 0.5 Since the material is sufficiently defined, the blue question marks and yellow fields are no longer present in the data table. Note: The resulting stress-strain curve is elastic – plastic with linear strain-hardening. Step 3 – Define Engineering Data Material ...Step 3 – Define Engineering Data Material ...SC3.h Access material library “General Materials” 3.i Add the material Concrete to the model SCMaterial Overview Step 3 – Define Engineering Data Material ...Step 3 – Define Engineering Data Material ...3.j Return to the Project Schematic 3.k Save the Project by selecting the “Save As ...” icon and Browse to the directory indicated by your instructor. Use the name “Circuit_board_drop_test” for the Project name.Note: Saving the Project saves all of the important files. The Project may also be Archived, in which all of the supporting files are compressed and saved in one file.Step 4 – Import the GeometryStep 4 – Import the Geometry4.c Workbench has now identified the geometry file (note green checkmark in Geometry cell). RMBSC4.a Import the geometry by the procedure shown. Do NOT Double Click on the “Geometry” cell ...4.b Browse to the DesignModeler geometry file named: “circuit_board.agdb”Step 4 – Import the GeometryStep 4 – Import the Geometry4.e View the geometry. Find the spot welds. The total number of spot welds is 6. DC4.d Double Click on the “Geometry” cell to open the geometry of the circuit boardStep 5 – Edit the Model in MechanicalStep 5 – Edit the Model in Mechanical5.a Edit the model in Workbench Mechanical. Since Edit is the default action, double-clicking on the Model cell is also acceptable here.RMBSC5.b Select the MKS Units system Recall that Mechanical is not native in Workbench, so the Units here may not match the Project Units Note: Although the unit system used for data entry and post-processing is the MKS system, the actual unit system used by the AUTODYN solver is the mm-mg-ms system, because it provides higher accuracy. SCStep 5 – Edit the Model in Mechanical ...Step 5 – Edit the Model in Mechanical ...5.c Define PowerDiss properties: Select all PowerDiss parts Thickness = 0.005m Material Assignment = PCBCtrlSCStep 5 – Edit the Model in Mechanical ...5.d Define Concrete properties: Select Concrete part Material Assignment = Concrete 5.e Define Heat Sink and Chips properties: Select Heat Sink and Chips parts Material Assignment = PCB Step 5 – Edit the Model in Mechanical ...SCCtrlSCStep 5 – Edit the Model in Mechanical ...Step 5 – Edit the Model in Mechanical ...5.f Define PCB properties: Select PCB part Thickness = 0.002m Material Assignment = PCBSCStep 5 – Edit the Model in Mechanical ...Step 5 – Edit the Model in Mechanical ...5.g Define contact properties: Select all contact regions RMB the selections Rename contact regionsRMBCtrlSCSCStep 5 – Edit the Model in Mechanical ...Step 5 – Edit the Model in Mechanical ...5.h Define Heat Sink/CPU breakable contact: Select Heat Sink/CPU bonded contact Breakable = Stress Criteria Normal Stress Limit = 5.0E7 Pa Shear Stress Limit = 2.5E7 PaCtrlSCStep 5 – Edit the Model in Mechanical ...Step 5 – Edit the Model in Mechanical ...5.i Define PowerDiss/PCB spot weld contacts: Select PowerDiss to PCB weld contacts Breakable = Force Criteria Normal Force Limit = 10 N Shear Force Limit = 5 NCtrlSCStep 5 – Edit the Model in Mechanical ...Step 5 – Edit the Model in Mechanical ...5.j Define Body Interactions: Select Body Interactions Shell Thickness Factor = 1.0 Body Self Contact = No Element Self Contact = NoSCStep 5 – Edit the Model in Mechanical ...Step 5 – Edit the Model in Mechanical ...5.k Define Body Interactions: Make sure All Bodies are selected Step 6 – Mesh the GeometryStep 6 – Mesh the Geometry6.a Select the Mesh branch 6.b Specify the Mesh Details: Physics Preference = Explicit Element Size = 0.002 meters 6.c Generate mesh by RMB on Mesh SCRMBSCStep 6 – Mesh the GeometryStep 6 – Mesh the GeometryMesh viewStep 7 – Define Initial ConditionStep 7 – Define Initial ConditionRMBSC7.a Define the Initial Condition: RMB Initial Conditions Select Insert -> Velocity Select all parts of the circuit board. Do not include the concrete ground Step 7 – Define Initial ConditionStep 7 – Define Initial ConditionSC7.b Click on Apply to specify the geometry: 7.c Specify the initial velocity Define By = Components X Component = 5.0 m/s Z Component = -1.71 m/sFinal view of the circuit board and its velocityStep 8 – Define the Analysis Settings Step 8 – Define the Analysis Settings 8.a Specify the Analysis Settings: End Time = 0.004 secondsSC8.b Set the Erosion Controls Geometric Strain Limit = 1E+20 On Geometric Strain Limit = No On Material Failure = Yes Final view of the Erosion ControlsStep 9 – Apply Boundary ConditionStep 9 – Apply Boundary Condition9.a Fix the Concrete (base): Select the Face filter Insert a Fixed Support under Analysis Settings Select the concrete bottom face Apply the selectionRMBSCSCStep 10 – Insert Result Items to PostprocessStep 10 – Insert Result Items to Postprocess10.a Insert a Contact Force plot request under the Solution Information branchRMBSCStep 10 – Insert Result Items to PostprocessStep 10 – Insert Result Items to Postprocess10.b Select the body filter 10.c Select the concrete part and then click on Apply Orientation = X Axis 10.d Repeat a-b to insert another Contact Force Orientation = Z Axis SCSCStep 10 – Insert Result Items to PostprocessStep 10 – Insert Result Items to Postprocess10.e Insert an Equivalent (von-Mises) Stress plot request under the Solution branch. RMBSCStep 11 – Run the AUTODYN SimulationStep 11 – Run the AUTODYN Simulation11.a Select Solution Information 11.b If click on Solve, the simulation will start. The simulation will run in hours You can view the pre-calculated solutions by following the instructions in the next 3 slides. SCSCStep 12 – Review the ResultsStep 12 – Review the Results12.a Start a new project 12.b Restore the archive “circuit_board_drop_test_run” and then save it to your directorySCSCSCStep 12 – Review the ResultsStep 12 – Review the Results12.c Plot the time history of Contact Force (X Axis) 12.d Plot the time history of Contact Force (Z Axis)SCSCStep 12 – Review the Results ...Step 12 – Review the Results ...12.e View the animation of Equivalent (von-Mises) StressSC12.f PowerDisss/PCB bonded weld contacts are broken. Thus PowerDiss parts are fallen off from the circuit board. The rest contact are still bonded.