Workshop 1 Taylor Impact Test – Basic Simulation ANSYS Explicit Dynamics

Workshop Goal and Procedure Simulate the impact of rod into a plate (typically known as a “Taylor Test”) Procedure: Create an Explicit Dynamics (ANSYS) Analysis System Project Select the unit system and assign the material properties Create the rod and plate geometry in DesignModeler Mesh the two parts and set the initial velocity condition of the rod Define the analysis settings, boundary conditions, and applied 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 1 – Create the Project Schematic ... An alternate method to create the Project Schematic would have been to Drag and Drop the Explicit Dynamics (ANSYS) Analysis System onto the blank screen to the right as shown below. Please note that, throughout these Workshops, the procedures shown are not always the only way to accomplish the desired tasks, so feel free to investigate other methods via the documentation when outside of this course. D&D

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 Note: Engineering Data is native in Workbench, but DesignModeler and Mechanical are NOT currently (but will be in the future). Therefore, always check that the local units system is as desired.

Step 3 – Define Engineering Data Material 3.a Edit the Engineering Data cell to select pre-defined material models from one of the pre-defined material libraries. 3.b Select the General Non-linear Materials library. These materials have sufficient physical property data defined so that they can be used in both ANSYS implicit and explicit analyses. DC Note: The material models in the Explicit Materials library are generally more complicated and can only be used in explicit dynamic analyses. SC

Step 3 – Define Engineering Data Material ... 3.c Select the “+” sign to the right of the Aluminum Alloy NL material model to add it to the Engineering Data library. 3.d Likewise, select the “+” sign to the right of the Structural Steel NL material. Note the symbol of a book that appears indicating success. SC SC

Step 3 – Define Engineering Data Material ... 3.e Return to the Engineering Data cell and note the added materials. SC 3.f Return to the Project Schematic 3.g Save the Project by selecting the “Save As” icon and Browse to the directory indicated by your instructor. Enter “taylor_basic” for the Project name.

Step 4 – Create the Geometry 4.a To create new geometry, follow the procedure shown. Double Clicking on the “Geometry” cell will also work, since “New Geometry ...” is the default action for the Geometry cell when a geometry file is not already associated with the Project. RMB SC 4.b Select Meter as the desired length unit. 4.c Select “Always use project unit” to get around the problem of DesignModeler not currently being native in Workbench. When new geometry is created, the existing Project units will be used in DesignModeler. 4.d Select OK to enter DesignModeler (DM).

Step 4 – Create the Geometry ... 4.e Select the Sketching tab. SC 4.f Next select the Circle tool from the Draw Toolbox. This tool requires that the center point be entered first followed by a point on the circle’s circumference. SC SC 4.g Use the Left Mouse Button (LMB) and click on graph origin (a “P” will appear when the mouse is over the origin). With the LMB still depressed, slide the pointer away from the center until a circle is created. Then let go of the LMB, completing the circle operation.

Step 4 – Create the Geometry ... 4.h Select the General tool from the Dimensions Toolbox. RMB 4.i RMB select the Radius operation for the General Dimensions tool. This is a temporary selection of a dimension type. 4.j Select the circle, creating dimension “R1”. Then enter 0.010 meters in the Details View for the circle radius. Resize the graphics view, if desired.

Step 4 – Create the Geometry ... 4.k Select the Extrude icon, which brings up the Modeling mode. 4.l Enter a Fixed Depth of 0.030 meters in the Normal Direction via the Details View. 4.m Select the Generate icon to complete the extrusion operation.

Step 4 – Create the Geometry ... 4.n Return to the Sketching mode and create a new sketch (Sketch2) for the plate construction. 4.o Select the Rectangle tool from the Draw Toolbox and draw the rectangle shown by dragging the LMB, using the opposite corners of the rectangle to define it. 4.p The dimensions of the rectangle will be defined next, so now select the Dimensions Toolbox.

Step 4 – Create the Geometry ... 4.q Select the General tool under the Dimensions Toolbox and dimension the lines on the top and right side to be 0.040 meters long. Since the rectangle is no longer centered about the circle, additional dimensions will need to be defined. 4.r For the next two dimensions, use the RMB to select the Horizontal and then the Vertical options, respectively. RMB selections

Step 4 – Create the Geometry ... 4.s After specifying a Horizontal General dimension via the RMB, make sure that ONLY the Vertex filter is active. This will prevent lines from being accidentally selected, thereby simplifying the task. 4.t Select the origin, and while holding the Ctrl key down, select the top right corner of the rectangle to create dimension H4. Repeat this procedure (after specifying a Vertical General dimension via the RMB) with the same two points to create dimension V5. 4.u Enter 0.020 meters for both H4 and V5 in the Details View for these dimensions. The rectangle is now centered correctly.

Step 4 – Create the Geometry ... 4.v Select the Extrude icon, which accesses the Modeling mode, and set the Operation to Add Frozen to prevent merging of the bodies. 4.w Enter a Fixed Depth of 0.010 m in the Reversed Direction. 4. x Extrude Sketch2 via Generate.

Step 4 – Create the Geometry ... 4.y Rename the two solids to be Cylinder and Plate, respectively. Use the RMB after selecting the body in the tree to access the Rename function. The Cylinder is not frozen, but the Plate is frozen. Since the bodies touch each other, they would be merged into one body if both bodies were unfrozen. RMB 4.z Save the Project

Step 5 – Edit the Model in Mechanical 5.a Edit the model in Workbench Mechanical. 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

Step 5 – Edit the Model in Mechanical ... 5.c Assign the material Aluminum Alloy NL to the Cylinder and the material Structural Steel NL to the Plate. To access the materials stored in the Engineering Data library, click on the default material currently assigned to the part, and a small fly-out arrow will appear. Clicking on that arrow lists the materials available for use. SC SC SC

Step 5 – Edit the Model in Mechanical ... 5.d Delete the automatically defined Contact Region. Alternatively, it can be changed from Type Bonded to Frictionless, but the existing Body Interactions are sufficient as shown below. Penalty-based Trajectory contact is the default interaction and the type is Frictionless. RMB SC

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 = 0.003 meters 6.c Generate the mesh RMB

Step 7 – Define the Initial Conditions 7.a Apply an Initial Velocity Condition to the Cylinder as shown. Note: If the Body selection filter is not automatically activated for the initial velocity condition, select it manually. SC RMB

Step 7 – Define the Initial Conditions ... 7.b Choose to define the Initial Velocity by Components: X = 0 m/sec Y = 0 m/sec Z = -300 m/sec

Step 8 – Define the Analysis Settings SC 8.a Select Analysis Settings in the tree and set the End Time to be 2.0e-4 seconds in the Details View. 8.b Keep the remaining default settings. 8.c Twenty equally-spaced results sets should be sufficient for the animations.

Step 9 – Apply Boundary Conditions 9.a Pick the Face selection filter. RMB 9.b Insert a Fixed Support on the back face of the Plate. Rotate the geometry, as needed.

Step 10 – Insert Result Items to Postprocess 10.a Insert a Directional Deformation plot request under the Solution branch and set the Orientation to the Z Axis in the Details View. RMB RMB 10.b Insert an Equivalent Plastic Strain plot request under the Solution branch. 10.c Save the Project.

Step 11 – Run the AUTODYN Simulation 11.a Select Solver Output under Solution Information and RMB Solve to start the simulation. 11.b Note: The model is converted to an AUTODYN Cycle Zero database and submitted to the AUTODYN solver. The results are written to the standard AUTODYN files, but are also available in this product for review. RMB

Step 11 – Run the AUTODYN Simulation ... 11.c The Solver Output shows the run statistics. This problem will only take a few minutes to solve and should terminate due to the condition “wrapup time reached”.

Step 12 – Review the Results 12.a Select Energy Summary under Solution Information to view the global statistics. Note how the Kinetic Energy of the projectile is converted into Internal Energy during impact. Also, the Hourglass Energy is sufficiently small (less than 10% of the Internal Energy). Internal Energy Kinetic Energy Hourglass Energy Plasticity develops

Step 12 – Review the Results ... 12.b Select Directional Deformation (Z Axis) and Show the Elements under True Scale. The maximum displacement (-0.0024 m) is in the negative Z direction, so it appears as a minimum value. SC

Step 12 – Review the Results ... 12.c Likewise, select Equivalent Plastic Strain. 12.d Animate the results by setting the controls as shown below and then pressing the Animation button. For transient dynamics, the default Distributed mode is often inadequate, as it just linearly interpolates between saved results and not enough data sets may have been saved for good interpolation. The Result Sets mode is usually best, as only actual saved data is used. Plastic strain constant after rod rebound from plate. Pick these 2 first Then pick this

Step 12 – Review the Results ... 12.e If desired, hide the Plate (or even the Cylinder) to get a better view of the remaining body. Reorient the animation as needed. RMB 12.f Finally, Save the model and then Exit ANSYS ...