1. DYNAMICS for ANSYS 5.7 Workshop Supplement

2. January 30, 2001 Inventory #001448 WS-2 Table of Contents Introductory Workshop Galloping Gertie --------------------------------------------W-4 Modal Analysis Workshop Plate with a Hole --------------------------------------------W-14 Modal Analysis Workshop Model Airplane Wing --------------------------------------------W-19 Harmonic Analysis Workshop Fixed-Fixed Beam--------------------------------------------W-23 Transient Analysis Workshop Bouncing Block --------------------------------------------W-28 Restarting a Transient Workshop Bouncing Block-------------------------------------------- W-35 Response Spectrum Workshop Workbench Table-------------------------------------------- W-40 Random Vibration Workshop Model Airplane Wing --------------------------------------------W-43 Pre-stressed Modal Analysis Workshop Pre-Stressed Disc --------------------------------------------W-49 Modal Cyclic Symmetry Workshop Spiral Bevel Gear--------------------------------------------W-54

3. Introductory Workshop Galloping Gertie

4. Workshop Supplement January 30, 2001 Inventory #001448 WS-4 Introductory Workshop … Galloping Gertie Objective To get an idea of the steps involved in a typical dynamic analysis. The Tacoma Narrows bridge, also known as the Galloping Gertie is famous for its spectacular collapse in 1940. In this workshop, we will examine a model of the bridge and calculate its natural frequencies and mode shapes. We will then simulate the wind storm and vortex shedding that caused the bridge’s collapse by doing a harmonic analysis.

5. Workshop Supplement January 30, 2001 Inventory #001448 WS-5 Introductory Workshop … Galloping Gertie Instructions 1. Enter ANSYS in the working directory specified by your instructor. 2. Start by reading input from the file gallop.inp. Utility Menu > File > Read Input from… choose gallop.inp –This will create the model and perform a static analysis to prestress the bridge. –The next step is to do a modal analysis.

6. Workshop Supplement January 30, 2001 Inventory #001448 WS-6 Introductory Workshop … Galloping Gertie 3.Enter Solution and change analysis type to Modal: Solution > New Analysis… choose Modal. 4.Set the following analysis options. [Solution >] Analysis Options... accept the default (Block Lanczos) 10 modes to extract 10 modes to expand Calculate element stresses Include prestress effects… press OK Accept defaults on the next dialog 5.Solve. [Solution >] -Solve- Current LS

7. Workshop Supplement January 30, 2001 Inventory #001448 WS-7 6.Plot the first few mode shapes. General Postproc > Next Set [General Postproc >] Plot Results > Nodal Solution... Mode 1 - SX stress Mode 3 - SX stress Introductory Workshop … Galloping Gertie

8. Workshop Supplement January 30, 2001 Inventory #001448 WS-8 7.Enter Solution and choose harmonic analysis. Solution > New Analysis… 8.Set the following analysis options. [Solution >] Analysis Options... Mode superposition solution method Defaults for all others (including subsequent dialog box) 9.Set frequency and substep options: Solution > Time/Frequenc > Freq and Substeps... Harmonic frequency range = 0 to 0.4 Number of substeps = 40 Stepped boundary conditions Introductory Workshop … Galloping Gertie

9. Workshop Supplement January 30, 2001 Inventory #001448 WS-9 10.Set constant damping ratio = 0.01. Solution > Time/Frequenc > Damping… 11.Apply a load vector for mode superposition with a scale factor of 100. Solution > Apply > Load Vector > For Mode Super… (close the warning message window) 12.Solve -Solve- Current LS 13. Enter POST26 (TimeHist Postproc) and identify the results file name. TimeHist Postpro > Settings > File… Number of variables allowed = 10 File containing data = gallop.rfrq Introductory Workshop … Galloping Gertie

10. Workshop Supplement January 30, 2001 Inventory #001448 WS-10 14. Create a scalar parameter to represent the center node: At command line type in ncen = node(0,0,0) 15. Define a variable (a vector) containing UZ displacements of the center node: a. TimeHist Postpro > Define Variables > Add > Nodal DOF Result > OK b.Pick any arbitrary node and press OK in the picker dialog (Note: you will change this node number to NCEN in the next dialog box!) c.Reference number for variable = 2 d.Node Number = ncen e.Name (user-defined label) = umid f.Choose DOF Solution, Translation in UZ Introductory Workshop … Galloping Gertie

11. Workshop Supplement January 30, 2001 Inventory #001448 WS-11 16. Graph variable number 2. TimeHist Postpro > Graph Variables… enter 2 in the top box. 17. Exit ANSYS or go to step 18 if time permits. Introductory Workshop … Galloping Gertie

12. Workshop Supplement January 30, 2001 Inventory #001448 WS-12 Optional: Continue with the following steps to review the deformed shape and stresses at 0.07 Hz frequency. 18. Read Input from… gallop_more.inp. 19. Enter POST1, read results for load step 1 substep 7, and plot the deformed shape and stress contours. Repeat for the imaginary part as well. 20. Exit ANSYS. Real Part Imaginary Part Introductory Workshop … Galloping Gertie

13. Modal Analysis Workshop Plate with a Hole

14. Workshop Supplement January 30, 2001 Inventory #001448 WS-14 Description: Determine the first 10 natural frequencies of the plate with a hole shown. Assume the plate to be radially constrained at the hole. The plate is made of aluminum, with the following properties: –Young’s modulus = 10 x 10 6 psi –Density = 2.4 x 10 -4 lbf-sec 2 /in 4 –Poisson’s ratio = 0.27 Modal Analysis Workshop … Plate with a Hole

15. Workshop Supplement January 30, 2001 Inventory #001448 WS-15 Instructions 1.Clear the database and read input from plate.inp to create the model geometry and mesh. Utility Menu: File > Clear & Start New… press OK, then answer Yes Utility Menu: File > Read Input from… choose plate.inp 2.Define material properties. Preprocessor > Material Props > Material Models… Double click through –… Structural … Linear … Elastic … Isotropic EX = 10e6(Young’s modulus in psi) PRXY = 0.27(Poisson’s ratio) [OK] –… Structural … Density DENS = 2.4e-4 (Density in lbf-sec 2 /in 4 ) [OK] Exit the material GUI Modal Analysis Workshop … Plate with a Hole

16. Workshop Supplement January 30, 2001 Inventory #001448 WS-16 3.Choose modal analysis. Solution > New Analysis… choose Modal, then OK 4.Specify analysis options. [Solution >] Analysis Options… Use Block Lanczos method (default) 10 modes to extract 10 modes to expand Yes to calculate element results… press OK Accept defaults on the next dialog box 5.Radially constrain the hole. Utility Menu: Plot > Lines [Solution >] -Loads- Apply > [Displacement >] > -Symmetry BC- On Lines + Pick the lines around the hole and press OK 6.Start the solution. [Solution >] -Solve- Current LS Check solution information in the /STAT window, then press OK Modal Analysis Workshop … Plate with a Hole

17. Workshop Supplement January 30, 2001 Inventory #001448 WS-17 7.Review results. Start by listing the frequencies. General Postproc > Results Summary 8.Plot the first mode shape. [General Postproc >] -Read Results- First Set [General Postproc >] Plot Results > Deformed Shape… Choose “Def and undef edge” and press OK 9.Plot and animate the next mode shape. [General Postproc >] -Read Results- Next Set Utility Menu: Plot > Replot Utility Menu: PlotCtrls > Animate > Mode Shape… 10 frames Time delay = 0.05 (accept all other defaults) 10. Repeat above step for subsequent mode shapes. Modal Analysis Workshop … Plate with a Hole MODE 6

18. Modal Analysis Workshop Model Airplane Wing

19. Workshop Supplement January 30, 2001 Inventory #001448 WS-19 Description: Determine the first five natural frequencies of the model airplane wing shown. Assume the wing to be fully fixed at Z=0. The wing has the following properties: –Young’s modulus = 38000 psi –Density = 1.033 x 10 -3 slugs/in 3 = 1.033E-3/12 lbf-sec 2 /in 4 Modal Analysis Workshop … Model Airplane Wing

20. Workshop Supplement January 30, 2001 Inventory #001448 WS-20 Instructions 1.Clear the database and read input from wing.inp to create the model geometry and mesh. 2.Define material properties. Remember to use British in -lb- sec units. 3.Apply boundary conditions. Hint: Choose Apply Displacements on Areas, pick the Z=0 area, and fix it in all DOF. Modal Analysis Workshop … Model Airplane Wing

21. Workshop Supplement January 30, 2001 Inventory #001448 WS-21 4.Extract (and expand) the first five natural frequencies using the Block Lanczos method. 5.Review all the mode shapes. Modal Analysis Workshop … Model Airplane Wing

22. Harmonic Analysis Workshop Fixed-Fixed Beam

23. Workshop Supplement January 30, 2001 Inventory #001448 WS-23 Harmonic Analysis Workshop … Fixed-Fixed Beam Description: Determine the harmonic response of a steel beam carrying two rotating machines which exert a maximum force of 70 lb at operating speeds of 300 to 1800 rpm. The beam, 10 feet long, is fully fixed at both ends, and the machines are mounted at its “one-third” points. Assume a damping ratio of 2%.

24. Workshop Supplement January 30, 2001 Inventory #001448 WS-24 Instructions 1.Clear the database and read input from beam.inp to create the beam model. 2.Specify harmonic analysis (full method). 3.Fix the two ends of the beam and apply the two in-phase harmonic forces of FY=70 lbs each at the 40-inch and 80-inch points along the beam. 4. Specify a damping ratio of 0.02 (i.e. 2%) ( Solution > -Load Step Opts- Time/Frequency > Damping ) 5.Specify 25 solutions between 5 and 30 Hz (300-1800 rpm). Remember to step apply the loading ( Solution > -Load Step Opts- Time/Frequency > Freq and Substps … ). Harmonic Analysis Workshop … Fixed-Fixed Beam

25. Workshop Supplement January 30, 2001 Inventory #001448 WS-25 6.Obtain the harmonic solution. 7.In Time history post processor plot UY displacements versus frequency for the two nodes at which the forces were applied. NOTE: Use ( Utility menu > PlotCtrls > Style > Graphs ) for changing graph style / settings. 8.In General Post processor review the deformed shape of the beam at the critical frequency and phase angle. Harmonic Analysis Workshop … Fixed-Fixed Beam

26. Workshop Supplement January 30, 2001 Inventory #001448 WS-26 9.If time permits, repeat the analysis with forces that are 180° out of phase. Harmonic Analysis Workshop … Fixed-Fixed Beam

27. Transient Analysis Workshop Bouncing Block

28. Workshop Supplement January 30, 2001 Inventory #001448 WS-28 Description: A 6x6x1-inch block is dropped on a 100- inch long beam from a height of 100 inches. Obtain a graph of the motion of the block as it bounces on the beam. Assume a gap stiffness of 2000 lb/in. The beam is fully fixed at both ends, and the only load is gravity, 386 in/sec 2. The beam and the block are made of the same material: –Young’s modulus = 1,000,000 psi –Density = 0.001 lbf-sec 2 /in 4 –Poisson’s ratio = 0.3 Transient Analysis Workshop … Bouncing Block

29. Workshop Supplement January 30, 2001 Inventory #001448 WS-29 Instructions 1.Clear the database and read input from bounce.inp to build the model. 2.Define a transient analysis (full method) 3.Fix the two ends of the beam in all directions. 4.Use APDL to calculate the integration time step (ITS): kgap = 2000- gap stiffness mgap = 6*6*0.001 = 0.036- mass of block pi = acos(-1) fgap = sqrt(kgap/mgap)/(2*pi) - gap frequency its = 1/(fgap*30) - integration time step Transient Analysis Workshop … Bouncing Block

30. Workshop Supplement January 30, 2001 Inventory #001448 WS-30 5.Solve using two load steps. Load Step 1 (for non-zero initial acceleration): –Fix all nodes of the block in all dofs. –Apply an acceleration of 386 in/sec 2 In Solution Control menu, –Set analysis to “large displacement transient”. –Set time=0.001. –2 substeps –Request output of all results for all substeps on the results file –Static solution (time integration effects off) with Step applied load. –Set beta damping of.0003183. SOLVE Transient Analysis Workshop … Bouncing Block

31. Workshop Supplement January 30, 2001 Inventory #001448 WS-31 Load Step 2 ( transient): Go back to solution control menu and –Time=1.5 –Automatic time stepping on, with starting ITS = 0.02, minimum ITS = its (from step 4) and maximum ITS = 0.02 –Transient solution (time integration effects “on”) –Release the block –SOLVE Transient Analysis Workshop … Bouncing Block

32. Workshop Supplement January 30, 2001 Inventory #001448 WS-32 6.Review results: –Plot the UY displacements of the beam mid-point and the block versus time. –Plot the FY reaction force at one of the constraints versus time. –Animate results over time. Note: To store all the frames needed for animation, you may need to reduce the size of the graphics window. Transient Analysis Workshop … Bouncing Block

33. Workshop Supplement January 30, 2001 Inventory #001448 WS-33 7.Do not exit ANSYS: –You will continue this workshop with a restart later on. Transient Analysis Workshop … Bouncing Block

34. Restarting a Transient Workshop Bouncing Block

35. Workshop Supplement January 30, 2001 Inventory #001448 WS-35 Description: Continue the bouncing block analysis from the previous exercise. That analysis was stopped at time=1.5. In this exercise we will continue to follow the block’s motion up to time=3.0. The restart files needed (.r001 /.ldhi /.rdb ) are available from the previous workshop. The results file from the previous transient analysis is also available. ANSYS will append the new results to this RST file as load step 3. Restarting a Transient Workshop … Bouncing Block

36. Workshop Supplement January 30, 2001 Inventory #001448 WS-36 Instructions: 1.Continue the ANSYS session from the previous workshop. 2. Solution > -Analysis- Restart This will bring up a lister window showing a summary of the restart files available. Choose the load step and substep number from this summary. 3. In Solution Control menu change TIME to 3.0. 4. Solve. Restarting a Transient Workshop … Bouncing Block

37. Workshop Supplement January 30, 2001 Inventory #001448 WS-37 In Time History postprocessor graph the UY displacement of a node on the block and a node on the beam again. Restarting a Transient Workshop … Bouncing Block

38. Workshop Supplement January 30, 2001 Inventory #001448 WS-38 In the general postprocessor animate the bouncing of the block again. –Animate results over time. Note: To store all the frames needed for animation, you may need to reduce the size of the graphics window. Restarting a Transient Workshop … Bouncing Block

39. Response Spectrum Workshop Workbench Table

40. Workshop Supplement January 30, 2001 Inventory #001448 WS-40 Description: Determine the displacements and stresses in a workbench table due to the acceleration spectrum shown below. Acceleration Frequency 2080200300 217 79.5 150.2 Response Spectrum Workshop … Workbench Table

41. Workshop Supplement January 30, 2001 Inventory #001448 WS-41 Instructions 1.Clear the database and read input from table.inp to create the model geometry and mesh. 2.Obtain a modal solution (15 modes) and view the first few mode shapes. Be sure to request element stress calculations. 3.Do a spectrum analysis for the given acceleration spectrum applied in the global X direction. Use the SRSS method of mode combination. 4.Review displacements and table top stresses for each load step. 5.If time permits, repeat the analysis with the spectrum applied in the Y direction, then in the Z direction. Response Spectrum Workshop … Workbench Table

42. Random Vibration (PSD) Workshop Model Airplane Wing

43. Workshop Supplement January 30, 2001 Inventory #001448 WS-43 Description: Determine the displacements and stresses of the model airplane wing due to an acceleration PSD applied to the base of the wing in Y direction. Assume the wing to be fully fixed at Z=0. Random Vibrations Workshop … Model Airplane Wing Acceleration(G 2 /Hz) Frequency (Hz) 20100400600 0.1 0.025 0.075

44. Workshop Supplement January 30, 2001 Inventory #001448 WS-44 Instructions 1.Clear the database and read input from wing.inp to create the model geometry and mesh. 2.Define material properties. Young’s modulus = 38000 psi Density = 1.033E-3/12 lbf-sec2/in4 3.Apply boundary conditions. Hint: Choose Apply Displacements on Areas, pick the Z=0 area, and fix it in all DOF. 4.Extract (and expand) the first 15 natural frequencies using the Block Lanczos method. Random Vibrations Workshop … Model Airplane Wing

45. Workshop Supplement January 30, 2001 Inventory #001448 WS-45 5.Review mode shapes. 6. Perform a PSD Spectrum analysis using the acceleration PSD shown. Hint: Be sure to use G 2 /Hz as the units of the PSD. 7. Specify excitation in the Y direction (by applying unit displacements in the Y direction at the base nodes). 8. Compute Participation factors. 9. Use PSD mode combination method and SOLVE. Random Vibrations Workshop … Model Airplane Wing

46. Workshop Supplement January 30, 2001 Inventory #001448 WS-46 10. In the general postprocessor look at the relative displacements/ stresses ( Load step 3). –Can you directly use stress contours for, say SZ, to compare to yield stress? –What is in load step 1? –Are equivalent/principal stresses derived from 1 sigma component stresses valid? Random Vibrations Workshop … Model Airplane Wing

47. Workshop Supplement January 30, 2001 Inventory #001448 WS-47 11. In Time History Postprocessor create the response PSD for UY at one of the nodes of the wingtip. Plot on log-log scale. –Hint: When you get into time history postprocessor first issue ‘Store Data’ and accept the default. This is required for computing Response PSD. Random Vibrations Workshop … Model Airplane Wing

48. Pre-stressed Modal Workshop Pre-Stressed Disc

49. Workshop Supplement January 30, 2001 Inventory #001448 WS-49 Modal Analysis Workshop … Pre-stressed Disc Description: Determine the first ten natural frequencies and mode shapes of the perforated aluminum disc shown. The disc is constrained at the central hole both in the radial and out-of-plane directions. A pre-stress exists due to a radial pressure load of -20 lbs/inch at the perimeter. Properties of the disc are as follows: –Young’s modulus = 10 x 106 psi –Density = 2.3 x 10-4 lbf-sec2/in4 –Poisson’s ratio = 0.27

50. Workshop Supplement January 30, 2001 Inventory #001448 WS-50 Instructions 1.Clear the database and read input from disc.inp to create the model geometry and mesh. 2.Apply displacement constraints: UZ=0 and symmetry b.c. (for radial constraints) at the central hole. Hint: You will need to use two menus: Solution > Apply > Displacement > On Lines + for the UZ constraint [Solution > Apply > Displacement >] -Symmetry B.C.- On Lines + for symmetry b.c. To pick the lines easily, switch to front view and use Circle picking. Modal Analysis Workshop … Pre-stressed Disc

51. Workshop Supplement January 30, 2001 Inventory #001448 WS-51 3.Apply the radial load as pressure on the lines at the perimeter : -20 pounds/inch on the outer edges of the disc. Hint: Stay with the front view, use Circle picking to pick the entire disc, then use Circle unpicking to unpick all except the outer edges. 4.Activate pre-stress effects (using the Analysis Options dialog box), obtain a static solution, and review results. 5.Switch to modal analysis, activate pre-stress effects (again), and extract the first 10 modes of the pre-stressed disc using the Block Lanczos method. Modal Analysis Workshop … Pre-stressed Disc

52. Workshop Supplement January 30, 2001 Inventory #001448 WS-52 6.Review the mode shapes. 7.If time permits, do a second, stress-free modal analysis (with pre-stress effects off) and compare results. Shown below is the first mode shape for each case. Can you guess which one is pre-stressed? Modal Analysis Workshop … Pre-stressed Disc

53. Modal Cyclic Symmetry Workshop Spiral Bevel Gear

54. Workshop Supplement January 30, 2001 Inventory #001448 WS-54 Description: Determine the first two natural frequencies of nodal diameter 2 for the spiral bevel gear shown. Assume a free-free condition (i.e., no displacement constraints). Material properties of the gear are as follows: –Young’s modulus = 2.9 x 10 7 psi –Density = 7.32 x 10 -4 lbf-sec 2 /in 4 –Poisson’s ratio = 0.32 Modal Cyclic Symmetry Workshop … Spiral Bevel Gear Courtesy: Sikorsky Aircraft

55. Workshop Supplement January 30, 2001 Inventory #001448 WS-55 Instructions 1.Clear the database and read input from bevel.inp to create the basic sector. 2.Identify one of the cyclic symmetry planes as node component RIGHT. Hint: First select the predefined area component A_RIGHT ( Utility menu > Select > Comp/Assembly > Select Comp/Assembly ). Then select all nodes attached to selected areas and define the node component RIGHT. 3. Make all nodes active ( Utility menu > Select > Everything ) Modal Cyclic Symmetry Workshop … Spiral Bevel Gear

56. Workshop Supplement January 30, 2001 Inventory #001448 WS-56 4.Save the database, then generate a copy of the basic sector. Preprocessor > Cyclic Sector... 5. Define a modal analysis with these options: –Block Lanczos method –Extract two modes in the frequency range 100 to 10,000 –Use accurate Lagrange method for constraint equation processing 6.Solve using the CYCSOL command for nodal diameter range 2 to 2, with 53 sectors. Use RIGHT as the Low component name. ( Solution > Modal Cyclic Sym … ) Modal Cyclic Symmetry Workshop … Spiral Bevel Gear

57. Workshop Supplement January 30, 2001 Inventory #001448 WS-57 7.Expand results to all 53 sectors ( Specify 53 in General Postproc > Modal Cyclic Sym … ). Then read in the results of the first mode shape ( - Read Results- First set ). NOTE: The EXPAND command actually creates new elements and nodes for all 53 sectors. Modal Cyclic Symmetry Workshop … Spiral Bevel Gear