ls-dyna碰撞例子

Exercise 5: Window Impact.In this exercise, we simulate the impact of a 2”x4” beam upon an impact resistant window. In coastal areas that are prone to hurricane damage, windows such as these are used to minimize possible damage from air-borne debris. The image below illustrates the analysis setup.A 2”x4” beam is given an initial velocity of 60mph and directed towards the window. Ideally, the beam will bounce off the window with little or no damage. However, as will be seen in this analysis, this is a difficult proposition that requires a great deal of engineering effort. There are many possible variations on the impact. The beam may be tumbling or rolling. It may also impact the window at a wide range of angles. A tool such as Ansys/LS-Dyna allows the analysis of a large combination of variables without resorting to expensive and time-consuming testing.It is important to remember that the proper design of these windows can greatly help prevent the loss of life or property during a hurricane.The mesh used in this example is illustrated below.Summary of Steps:1. Launch Ansys/LS-Dyna1.1. Launch ANSYS using your Start menu2. Setup2.1. Resume Database2.2. Set LS-Dyna Preferences2.3. Plotting Controls2.4. Define Element Types2.5. Define Real Constants3. Material Properties3.1. Linear Elastic Properties for Wall3.2. Plastic Kinematic Plasticity Model for Window Frame3.3. Plastic Kinematic Plasticity Model for Plexiglass3.4. Linear Elastic Properties for 2”x4” Wooden Beam3.5. Rigid Material Properties for Floor3.6. Rigid Material Properties for Crash Dummy4. Loads4.1. Define 2”x4” Wooden Beam Nodal Component4.2. Apply Initial Velocity to 2”x4” Wooden Beam5. Constraints5.1. Apply Constraints to Edges of Wall and Floor6. Contact Definition6.1. Define Automatic General Contact6.2. Define Wall Tie Surface Component6.3. Define Window Tie Surface Component6.4. Define Tied Surface-to-Surface Contact7. Solution Controls7.1. Time Controls7.2. Output Controls7.3. Analysis Controls7.4. Save Model7.5. Solution Monitoring7.6. Solve Model8. General Post-Processing8.1. Plot Setup8.2. Stress Plot9. Generate HTML Report9.1. Image Capture and Animation Generation9.2. Report Assembly10. Conclusions10.1. Exit AnsysStep-by-Step Instructions:Before we begin this problem, create a separate folder on your computer for this analysis and copy the ANSYS database window.db from the CD into this folder.1. Launch ANSYS/LS-Dyna1.1. Launch ANSYS using your Start MenuA. Browse to select the working directory were you placed thewindow.db file for this job.B. Enter window for the job name. All subsequent ANSYS files createdfor this problem will have a filename of window followed by a uniqueextension.C. Change the workspace and database sizes for this job to 384 and 128respectively.D. Click RUN to start ANSYS1.1.B1.1.C1.1.D2. Setup2.1. Resume DatabaseA. We are going to start with an ANSYS database that has already beenmeshed for you. This database contains the geometry of the window, wall, and beam as well as their constitutive elements and nodes. B. Resume Jobname.db ANSYS will read in the predefined databasewindow.db and plot the model in the graphics window.2.2. Set LS-Dyna PreferencesA. In the ANSYS main menu, pick Preferences…B. LS-Dyna ExplicitC. OK2.3. Plotting ControlsA. Use the Pan/Zoom/Rotate function to examine all parts of the modelas done in previous exercises. In the Utility menu, select PlotCtrlsB. Pan, Zoom, Rotate… This will activate the view control window.C. It is useful to keep this window active at all times.2.2.B2.2.CPan Zoom Rotate Functions:2.4. Define Element TypesThe wall and beam have been modeled using 8 noded bricks and the window, crash dummy, and floor have been modeled using shell elements. Thus, the SOLID164 (brick) and SHELL163 (shell) explicit element types are appropriate for this problem. As this example was pre-meshed, these element types are already defined. To review the element types in the modelA. In the Preprocessor menu, select Element TypeB. From this dialog box, it is possible to Add additional element types,Edit the existing types, or Delete defined types.C. For this case no modification is required. Click Close2.4.C2.5. Define Real ConstantsThe SOLID164 elements require no real constants. However, the SHELL163 elements require real constant input.A. In the Preprocessor menu, select Real Constants…B. In the Real Constants dialog box, click on Add…C. In the Element Type for Real Constants , highlight Type 2 or 100.Note that it does not make a difference as both element type 2 and 100 reference Real constant set 1. Therefore, as this is set 1, the values input will be used by both element types. Click OK D. Input 5/6 for the Shear FactorE. Input 4 for the No. of integration pts.F. Input 0.125 for the Thickness at node 1G. Click OK. Note that ANSYS will default to using 0.125 for all fournodes if only the first value is input.H. Close the Real Constants dialog box by clicking Close2.5.G3. Material Properties3.1. Linear Elastic Properties for WallA. In the Preprocessor menu, select Material PropsB. Define MAT Model…C. In the Material Models dialog, click Add…D. Enter 1 for the Material NumberE. Highlight Linear Elastic and IsotropicF. Click OK3.1.D3.1.FG. In the Define Material Model dialog, enter 0.00031055 for DensityH. Enter 10e6 for Young’s modulusI. Enter 0.3 for the Poisson’s RatioJ. Click OK3.1.J3.2. Plastic Kinematic Plasticity Model for Window Frame A. Click Add…B. Enter 2 for the Material NumberC. Highlight Plasticity and Plastic KinematD. OKE. Enter 0.00022345 for DensityF. Enter 10e6 for Young’s modulusG. Enter 0.3 for Poisson’s RatioH. Enter 50000 for Yield StressI. Enter 200000 for Tangent ModulusJ. Enter 0.3 for Failure strainK. OK3.2.B3.2.C3.2.D3.2.K3.3. Plastic Kinematic Plasticity Model for Plexiglass A. Click Add…B. Enter 3 for the Material NumberC. Highlight Plasticity and Plastic KinematD. OKE. Enter 0.00024120 for DensityF. Enter 20e6 for Young’s modulusG. Enter 0.3 for Poisson’s RatioH. Enter 120000 for Yield StressI. Enter 280000 for Tangent ModulusJ. Enter 0.115 for Failure strainK. OK3.3.B3.3.C3.3.D3.3.K3.4. Linear Elastic Properties for 2”x4” Wooden Beam A. Click Add…B. Enter 4 for the Material NumberC. Highlight Linear Elastic and IsotropicD. Click OKE. In the Define Material Model dialog, enter 0.00032349 for DensityF. Enter 7e6 for Young’s modulusG. Enter 0.3 for the Poisson’s RatioH. Click OK3.4.B3.4.D3.4.H3.5. Rigid Material Properties for Floor A. Click Add…B. Enter 5 for the Material NumberC. Highlight Other and RigidD. Click OKE. In the Define Material Model dialog, enter 0.00038819 for DensityF. Enter 10e6 for Young’s modulusG. Enter 0.3 for the Poisson’s RatioH. Click OKI. Click Close to exit the Defing MAT Model dialog.3.5.B3.5.C 3.5.D3.5.H3.6. Rigid Material Properties for Crash Dummy A. Click Add…B. Enter 6 for the Material NumberC. Highlight Other and RigidD. Click OKE. In the Define Material Model dialog, enter 0.00038819 for DensityF. Enter 10e6 for Young’s modulusG. Enter 0.3 for the Poisson’s RatioH. Click OKI. Click Close to exit the Defing MAT Model dialog.3.6.B3.6.C 3.6.D3.6.H4. Loads4.1. Define 2”x4” Wooden Beam Nodal Component A. In the ANSYS Utility menu, pick Select B. Entities…C. In theSelect Entities dialog box, select Nodesand By Num/Pick D. Click OK4.1.DE. In the Pan-Zoom-Rotate dialog (discussed in section 2.3), select aRight view and Fit the view to the model.F. In the Select nodes dialog box, highlight the Box option.G. Draw a box around the wooden beam by clicking and dragging.H. Once all of the nodes in beam are selected, click OKI. Return to the ANSYS Utility menu and pick Select J. Comp/Assembly K. Create Component4.1.HL. Enter beam for the component name.M. Select Nodes as Entity component is made ofN. Click OKO. Return again to the ANSYS Utility menu and pick Select P. Everything4.2. Apply Initial Velocity to 2”x4” Wooden Beam Nodal ComponentA. In the Preprocessor menu, select LS-DYNA OptionsB. Initial VelocityC. w/Axial Rotate…D. In the Generate Velocity dialog, select the BEAM component to applythe initial velocity.E. Enter -10 for the VX Global X-componentF. Enter -10 for the VY Global Y-componentG. Enter –1056 for the VZ Global Z-componentH. Leave all other options set to 0I. Click OK4.2.D4.2.E-G 4.2.I5. Constraints5.1. Apply Constraints to Edges of Wall and FloorA. In the Pan-Zoom-Rotate dialog (discussed in section 2.3), select aFront view and Fit the view to the model B. In the Preprocessor menu, select LS-DYNA Options C. Constraints D. Apply E. On NodesF. In the Apply U,Rot on Nodes dialog, highlight the Box optionG. Draw boxes on each side of the wall and floor to select the edge nodes. See the following elment plot figure. H. Click OKI. In the Apply U,ROT on Nodes dialog, highlight the UX, UY, and UZDOFs to be constrainedJ. Select Constant Value for the Apply as option and enter 0 as a Value K. OK5.1 G5.1.I5.1.J5.1.K6. Contact Definition6.1. Define Automatic General ContactA. In the LS-Dyna Options menu, select ContactB. Define ContactC. Highlight Single Surface and Auto Gen’l (AG)D. Click OK6.1.DE. Click OK again.6.2. Define Wall Tie Surface Component A. In the ANSYS Utility Menu, click Select B. Entities…C. In the Select Entities dialog, highlight Elements , By Attributes , andMaterial num6.1.ED. Enter 1,1,1 for Min, Max, IncE. Click ApplyF. In the Select Entities dialog, highlight Nodes , Attached to , andElements G. Click Plot H. Click OKI. In the Pan-Zoom-Rotate dialog, select a Front view and FitJ. Return to the Select menu in the ANSYS utility menu and click Entities… K. In the Select Entities dialog, highlight Nodes , By Num/Pick , andReselect and click OK L. In the Select Node dialog, enable Polygon picking and select the nodes in the window frame. M. Click OK6.2.GN. In the ANSYS Utility menu, click Select O. Comp/Assembly P. Create Component…Q. Enter Wallfrm for the Component Name R. Click OK6.3. Create the Window Frame Tie Surface Component A. In the ANSYS Utility Menu, click Select B. Entities…C. In the Select Entities dialog, highlight Elements , By Attributes , andMaterial num D. Enter 2,2,1 for Min, Max, Inc E. Click ApplyF. In the Select Entities dialog, highlight Nodes , Attached to , andElementsG. Click Plot H. Click OKI. In the Pan-Zoom-Rotate dialog, select a Front view and Fit6.3.GJ. Return to the Select menu in the ANSYS utility menu and click Entities…K. In the Select Entities dialog, highlight Nodes, By Num/Pick, and Reselect and click OKL. In the Select Node dialog, enable Polygon picking and select the nodes in the window frame. M. Click OKN. In the ANSYS Utility menu, click Select O. Comp/AssemblyP. Create Component…Q. Enter Winfrm for the Component Name R. Click OK6.3.R6.4. Create Tied Surface-to-Surface ContactA. In the Preprocessor menu, click on LS-DYNA OptionsB. Define ContactC. In the Contact Parameter Definitions dialog, highlight Surface to Surf and TiedD. Click OK6.4.DE. In the Contact Options dialog, select Winfram for ContactComponent and Wallfram for the Target ComponentF. Click OKG. In the ANSYS Utility menu, click Select and Everything6.4.F7. Solution Controls7.1. Time ControlsA. Under the Ansys Main Menu, select SolutionB. Time ControlsC. Solution Time…D. For the termination time, enter 0.5E. OK7.2. Output ControlsA. In the Solution menu, click Output ControlsB. File Output FreqC. Time Step Size…7.1.D7.1.ED. Enter 1e-02 for Result File Output Interval and Time-History OutputInterval E. Enter 1.0 for Restart Dump Output Interval F. OK7.3. Analysis OptionsNo modifications to default ANSYS analysis options are required for this analysis. 7.4. Save ModelA. In the Ansys Utility menu, select FileB. Save as Jobname.db 7.5. Solution InstructionsA. In the Solution menu, select SolveB. OKC. Click Yesin the verification dialog7.2.D7.2.E 7.2.F7.6. Solution MonitoringA. LS-Dyna will open a window to run the analysis. In this window bypressing Ctrl+C, it is possible to monitor the solution process. After hitting Ctrl+C and entering sw1, sw2, sw3, or sw4, LS-Dyna will respond according to the table below. B. Sw2 is particularly useful. Hitting Ctrl+C and entering sw2 will causeLS-Dyna to respond with time, energy, and remaining solution time. C. Sw1 allows an analysis to be terminated. LS-Dyna will write results atthe time point at which it stops.7.5.B7.5.C8. General Post-Processing8.1. Plot SetupA. Now that we have completed the analysis, it is necessary topostprocess the results. This is accomplished by going into the Ansys General Postprocessing module. Pick General Postproc from the Ansys Main menu. B. Once in the Postprocessor module, we need to tell Ansys what file topostprocess. Click Data and File Opts… C. All Items D. window.rst E. Click OK8.1.C 8.1.D 8.1.EF. Now we need to specify a results set to read into Ansys. SelectResults Summary from the General Postproc menu. G. Highlight step 12 H. Read I. Close8.1.H8.1.I。