Workshop 2 Simulate the Crushing of an Empty Soda Can ANSYS Explicit Dynamics

Workshop Goal and Procedure Crush an aluminum beverage can and allow it to “springback” Procedure: Create an Explicit Dynamics (ANSYS) Analysis System Project Select the units system and define the material properties Import, modify, and mesh the soda can geometry Define analysis settings, boundary conditions, and external loads Initiate the solution (AUTODYN - STR) and review the results

Step 1 – Create the Project Schematic Start 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 RMB = Right Mouse Button Selection D&D = Drag and Drop = Hold Left Mouse Button down on item while dragging it to new location and then release it (i.e., Copy or Move) 1. Create an ANSYS Explicit Dynamics Analysis System Project DC

Step 2 – Specify the Project Units 2.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 Material 3.a Edit the Engineering Data cell to add a material to the default library. 3.b Select the last slot under Engineering Data to define a new material model. DC Note: An existing material model in the Explicit Materials library could have been selected, but there are restrictions on element types that can be used with certain material models, which will be discussed later. 3.c Enter material model name: “My_Aluminum” SC

Step 3 – Define Engineering Data Material ... 3.d Make sure the new material is active in order to define its properties SC 3.e Add the following Physical Properties to the material definition: Density Isotropic Elasticity Bilinear Isotropic Hardening DC DC DC

Step 3 – Define Engineering Data Material ... 3.f Enter the following values: Density = 2710 kg m^-3 Young’s Modulus = 7e10 Pa Poisson’s Ratio = 0.30 Yield Strength = 2.9e8 Pa Tangent Modulus = 0.0 Pa 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 – perfectly plastic. No strain hardening can develop.

Step 3 – Define Engineering Data Material ... 3.g Return to the Project Schematic 3.h Save the Project by selecting the “Save As ...” icon and Browse to the directory indicated by your instructor. Use the name “empty_soda_can” 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 and Modify the Geometry 4.a Import the geometry by the procedure shown. Do NOT Double Click on the “Geometry” cell ... RMB 4.b Browse to the DesignModeler 11.0 SP1 geometry file named: “soda_can_filled_110.agdb” SC 4.c Workbench has now identified the geometry file (note green checkmark in Geometry cell). It is now OK to Double Click on “Geometry”, as the new default action is to Edit the geometry. Default actions are shown in bold type after RMB selects. RMB SC

Step 4 – Import and Modify the Geometry ... 4.d Suppress the solid “Soda” and the surface body “Hole”. 4.e Generate the changes in the geometry. Although additional modifications could be made, but none are needed. 4.f Save the entire Project via the DM “Save” icon. RMB SC

Step 5 – Edit the Model in Mechanical 5.a Edit the model in Workbench Mechanical. Since Edit is the default action, double-clicking on the Model cell is also acceptable here. RMB SC 5.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. This will be shown later when the Analysis Settings are discussed.

Step 5 – Edit the Model in Mechanical ... 5.c Define the Aluminum Can properties: Stiffness Behavior = Flexible Thickness = 0.00025 meters Material Assignment = My_Aluminum 5.d Define the Punch and Die properties: Stiffness Behavior = Rigid Material Assignment = Structural Steel Rigid Steel Punch (moved downwards) Flexible Aluminum Soda Can (crushed) Rigid Steel Die (fixed)

Step 5 – Edit the Model in Mechanical ... 5.e Review the Contact specifications Keep contact definition defaults Note: There is no Save icon in Mechanical 5.f Save the Project

Step 6 – Set Sizing Controls and Mesh Model 6.a Select the Mesh branch 6.b Specify the Mesh Details: Physics Preference = Explicit Element Size = 0.010 meters 6.c Choose the Edge selection filter 6.d Orient the model to select the 8 edges that define the can circumferences (with the Left Mouse Button). Use the Ctrl key for multiple selections, as needed. RMB (anywhere) SC SC 6.e With the 8 edges still highlighted, Insert (RMB anywhere on graphics screen) an Edge Sizing

Step 6 – Set Sizing Controls and Mesh Model ... 6.f Specify the Edge Sizing Details: Type = Number of Divisions Number of Divisions = 36 Behavior = Hard 6.g Generate the Mesh (RMB on either Mesh branch or Edge Sizing branch) RMB SC Mesh view

Step 7 – Define the Analysis Settings 7.a Specify the Analysis Settings: End Time = 6.0e-4 seconds Automatic Mass Scaling = Yes Minimum CFL Time Step = 1.0e-7 sec SC 7.b Set the Solve Units = mm, mg, ms Note: The mm, mg, ms unit system is the most accurate in most simulations, so it is the only one currently available. Although more solver unit systems will be available in the future, any unit system in the drop-down list may be used to enter data and/or display the results.

Step 7 – Define the Analysis Settings ... 7.c Keep the remaining defaults Note: There are multiple ways to control the erosion of an element. In this case, the element will only fail when the geometric strain reaches 150%. 7.d Use the default number of data sets to save during the solution. Depending on the analysis, this number may need to be increased, but that requires additional disk space, so be judicious here.

Step 8 – Apply BCs and External Loads RMB SC 8.a Fix the Steel Die (base): Select the Body filter Insert a Fixed Support under Explicit Dynamics Select the steel die Apply the selection SC

Step 8 – Apply BCs and External Loads ... RMB SC SC 8.b Displace the Steel Punch Insert a Displacement under Explicit Dynamics Select the steel die Apply the selection

Step 8 – Apply BCs and External Loads ... 8.c Specify the vertical (Y) displacement to be a Tabular load and set both the X and Z displacements to be zero. 8.d Ramp the Y displacement as follows: Time = 0.0 sec Y = 0.0 meters Time = 5e-4 sec Y = -0.060 meters Time = 6e-4 sec Y = -0.030 meters Note: The punch speed and abrupt change in direction are unrealistic, but sufficient for demonstration purposes. Normally, the movement would be prescribed according to a SINE wave function.

Step 9 – Insert Result Items to Postprocess 9.a Insert a Total Deformation plot request under the Solution branch. 9.b Insert an Equivalent (von-Mises) Stress plot request under the Solution branch. The rigid bodies (i.e., the punch and die) will not show stress. RMB SC SC SC RMB SC SC SC

Step 9 – Insert Result Items to Postprocess ... 9.c Insert an Equivalent Plastic Strain plot request under the Solution branch. RMB SC 9.d Save the Project again. SC SC Note: Even though a single time point (at the end of the run) is specified, the complete set of results can be viewed, including animations. Recall that the default output controls (20 equally spaced time points) was retained under the Analysis Settings branch.

Step 10 – Run the AUTODYN Simulation 10.a Select Solver Output under Solution Information and Solve the simulation. SC The Solver Output shows the run statistics, including the estimated clock time to completion. Any errors or warnings are also noted. Termination due to “wrapup time reached” is expected here.

Step 10 – Run the AUTODYN Simulation ... 10.b Select Energy Summary under Solution Information to review the global statistics. Note the abrupt changes in kinetic energy due to the unrealistic loading scenario ... TIME = 5.0e-4 seconds occurs around 3200 cycles into run Constant velocity after starting from rest

Step 11 – Review the Results 11.a Select Total Deformation and Show the Elements under True Scale. The maximum deformation (-0.060 m) exceeds the punch value due to the momentum involved (i.e., an excessive punch speed was used to reduce the required computer run time). SC

Step 11 – Review the Results ... 11.b Animate the results by setting the controls as shown below and then pressing the Animation button. For transient dynamics, the default Distributed mode is inadequate, as it linearly interpolates between saved results. The Result Sets mode is optimal, as it uses the actual saved data. To review a static result, just click on the desired Time or Value from the Tabular Data and use the RMB to pick Retrieve This Result. The given state will then be shown. Pick these 2 first Pick this to save the animation Then pick this To retrieve a given result ... RMB

Step 11 – Review the Results ... 11.c Repeat the procedure, if desired, for the von-Mises equivalent stress results. Note: No stress can develop in a rigid body. The punch and die are each condensed out to a mass at their respective centers of gravity with six DOFs active. SC Contact is based on the exterior surface, so a six DOF body can have a complicated contact surface.

Step 11 – Review the Results ... 11.d Repeat the procedure one last time for the equivalent plastic strain results. 11.e. Hide the Punch and Die for a better view of the results. Per the Analysis Settings, erosion does not occur until the geometric strain is 1.50 SC RMB SC

Step 12 – Review the Output Files 12.a Pick Files under the View menu to access the Project files 12.b Select Open Containing Folder via the RMB option for the AUTODYN print file (admodel.prt). RMB

Step 12 – Review the Output Files ... 12.c Double click on the file admodel.prt 12.d As noted earlier, the solver units system was mm-mg-ms in order to maximize the accuracy. After the Simulation is done, the results are converted back into the current Mechanical units system.

Step 12 – Review the Output Files ... 12.e The AUTODYN print file also contains the Material Summary information and run statistics. The Energy and Momentum are shown on both a material basis and a Part basis (shown here).

Step 12 – Review the Output Files ... 12.f The Energy and Momentum Balance, Mass Scaling, and Run Times are also included in the admodel.prt file. 12.g No mass was added to the model, since the time steps were all above the Minimum CFL Time Step of 1.0e-7 sec set in Step 7.a under Analysis Settings

Step 12 – Review the Output Files ... 12.h Close the admodel.prt file and review the setup.log file in the same directory (F:\exp_dyn\soda_can\empty_soda_can_files\dp0\SYS\MECH). 12.i The setup.log file contains the information pertaining to the transfer of data from the Explicit Dynamics (ANSYS) Analysis System to the AUTODYN Cycle Zero file, which is then run by the AUTODYN solver. 12.j Close the file and return to the Mechanical window (i.e., view the model itself again).

Step 13 – Generate a Report 13.a Click on the Solution branch in the Project tree and then click on the Report Preview tab at the bottom of graphics window. ANSYS does the rest! It will now automatically generate a report by going through the entire tree and summarizing the model and the results.

Step 13 – Generate a Report ... 13.b The model properties are summarized, including volume, mass, centroid, and moment of inertia properties. 13.c Loading information is also shown in clear table format.

Step 13 – Generate a Report ... 13.d Even the energy plots are conveniently assembled into the report.

Step 13 – Generate a Report ... 13.e The results data is shown. 13.f Finally, SAVE the model and exit ANSYS.