Workshop 1 Taylor Impact Test – Basic Simulation ANSYS Explicit Dynamics ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -1 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Workshop Goal and Procedure Training Manual Goal: 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 Design. Modeler 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 ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -2 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 1 – Create the Project Schematic Training Manual 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 ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -3 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 1 – Create the Project Schematic. . . Training Manual • 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 ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -4 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 2 – Specify the Project Units Training Manual 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 Design. Modeler and Mechanical are NOT currently (but will be in the future). Therefore, always check that the local units system is as desired. ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -5 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 3 – Define Engineering Data Material DC Training Manual 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. Note: The material models in the Explicit Materials library are generally more complicated and can only be used in explicit dynamic analyses. SC ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -6 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 3 – Define Engineering Data Material. . . Training Manual 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. ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. SC SC WS 1 -7 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 3 – Define Engineering Data Material. . . 3. e Return to the Engineering Data cell and note the added materials. Training Manual 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. ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -8 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 4 – Create the Geometry RMB SC Training Manual 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. 4. b Select Meter as the desired length unit. 4. c Select “Always use project unit” to get around the problem of Design. Modeler not currently being native in Workbench. When new geometry is created, the existing Project units will be used in Design. Modeler. 4. d Select OK to enter Design. Modeler (DM). ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -9 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 4 – Create the Geometry. . . SC Training Manual 4. e Select the Sketching tab. 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. ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -10 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 4 – Create the Geometry. . . Training Manual 4. h Select the General tool from the Dimensions Toolbox. RMB 4. j Select the circle, creating dimension “R 1”. Then enter 0. 010 meters in the Details View for the circle radius. 4. i RMB select the Radius operation for the General Dimensions tool. This is a temporary selection of a dimension type. Resize the graphics view, if desired. ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -11 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 4 – Create the Geometry. . . Training Manual 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. ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -12 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 4 – Create the Geometry. . . Training Manual 4. n Return to the Sketching mode and create a new sketch (Sketch 2) 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. ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -13 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 4 – Create the Geometry. . . Training Manual 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 ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -14 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 4 – Create the Geometry. . . Training Manual 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 H 4. Repeat this procedure (after specifying a Vertical General dimension via the RMB) with the same two points to create dimension V 5. 4. u Enter 0. 020 meters for both H 4 and V 5 in the Details View for these dimensions. The rectangle is now centered correctly. ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -15 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 4 – Create the Geometry. . . Training Manual 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 Sketch 2 via Generate. ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -16 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 4 – Create the Geometry. . . Training Manual 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 ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -17 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 5 – Edit the Model in Mechanical Training Manual 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 ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -18 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 5 – Edit the Model in Mechanical. . . Training Manual 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 ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -19 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation 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. Training Manual RMB Penalty-based Trajectory contact is the default interaction and the type is Frictionless. SC ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -20 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 6 – Set Sizing Controls and Mesh Model Training Manual 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 ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -21 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 7 – Define the Initial Conditions Training Manual 7. a Apply an Initial Velocity Condition to the Cylinder as shown. SC RMB ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -22 Note: If the Body selection filter is not automatically activated for the initial velocity condition, select it manually. February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 7 – Define the Initial Conditions. . . Training Manual 7. b Choose to define the Initial Velocity by Components: – X = 0 m/sec – Y = 0 m/sec – Z = -300 m/sec ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -23 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 8 – Define the Analysis Settings SC Training Manual 8. a Select Analysis Settings in the tree and set the End Time to be 2. 0 e-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. ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -24 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 9 – Apply Boundary Conditions Training Manual 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. ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -25 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 10 – Insert Result Items to Postprocess Training Manual 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 10. b Insert an Equivalent Plastic Strain plot request under the Solution branch. 10. c Save the Project. ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -26 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 11 – Run the AUTODYN Simulation Training Manual 11. a Select Solver Output under Solution Information and RMB Solve to start the simulation. RMB ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. 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. WS 1 -27 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 11 – Run the AUTODYN Simulation. . . Training Manual 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”. ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -28 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 12 – Review the Results Training Manual 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 Plasticity develops ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. Hourglass Energy WS 1 -29 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 12 – Review the Results. . . Training Manual 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 ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -30 February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 12 – Review the Results. . . Training Manual 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. Pick these 2 first Then pick this ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -31 Plastic strain constant after rod rebound from plate. February 27, 2009 Inventory #002665
Workshop 1. Taylor Impact Test – Basic Simulation Step 12 – Review the Results. . . Training Manual 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. . . ANSYS, Inc. Proprietary © 2009 ANSYS, Inc. All rights reserved. WS 1 -32 February 27, 2009 Inventory #002665
Скачать презентацию Workshop 1 Taylor Impact Test Basic Simulation
ANSYS_Explicit_Dynamics_120_Workshop_01.ppt