1. WS16-1 MAR120, Workshop 16, December 2001 WORKSHOP 16 SPECTRUM RESPONSE ANALYSIS OF A TRANSMISSION TOWER 0.9751 2.5 3 4.5 2.56.6 2.258 210 1.1100 1.011000 0.29250.3 0.1950.2 0.009750.01 0.00048750.0005 0.00009750.0001 ValueFrequency

2. WS16-2 MAR120, Workshop 16, December 2001

3. WS16-3 MAR120, Workshop 16, December 2001 Model Description  This model represents a transmission tower such as those used to broadcast radio and television signals.  The model will be subjected initially to a response spectrum analysis in order to determine the maximum displacements due to an earthquake.  After the initial response spectrum analysis, the initial boundary conditions will be modified to provide for a preload in the structure. This preloaded structure will then be subjected to a second response spectrum analysis in order to determine the difference in response.

4. WS16-4 MAR120, Workshop 16, December 2001 n Objective u Set-up and solution of response spectrum analysis. Use the typical spectrum for rocklike material provided in the table (right). u Creation of preload step and response spectrum analysis with preloaded structure. u Comparison of results between analyses. n Required u The MSC.Patran Tower.ses is required. It should be provided together with this training material. This is a typical earthquake spectrum for rocklike material with a soil depth less than 200 ft, as provided by the UBC. 0.9751 2.5 3 4.5 2.56.6 2.258 210 1.1100 1.011000 0.29250.3 0.1950.2 0.009750.01 0.00048750.0005 0.00009750.0001 ValueFrequency

5. WS16-5 MAR120, Workshop 16, December 2001 n Suggested Exercise Steps 1. Read the Tower.ses file to create geometry. 2. Mesh the model using 1 element per curve. 3. Apply the model properties and boundary conditions. 4. Set-up and solve the initial response spectrum analysis. 5. Create the preload case, solve response spectrum with preloaded structure. 6. Compare results.

6. WS16-6 MAR120, Workshop 16, December 2001 d f CREATE NEW DATABASE Open a new database. Name it tower_spectrum.db. a.File: New b.Enter tower_spectrum as the file name. c.Click OK. d.Wait a few seconds until the New Model Preference opens. e.Select MSC.Marc as the Analysis Code. f.Click OK. a b c e

7. WS16-7 MAR120, Workshop 16, December 2001 g.File: Session / Play. h.Select tower.ses. i.Click –Apply-. g h i

8. WS16-8 MAR120, Workshop 16, December 2001 f Step 1. Elements: Create / Mesh Seed / Uniform Elements: Create the Mesh Seed. a.Elements: Create / Mesh Seed / Uniform. b.Select Number of Elements. c.Enter 1 as the Number. d.Click Curve List panel. e.Click Curve or Edge picking icon. f.Select all curves. There are 3 curves which do not exist in the range. If you input the range by hand, choose Yes to All for the error message e a b c d Curve 1:105 107:128 130:1

9. WS16-9 MAR120, Workshop 16, December 2001 e Step 2. Elements: Create / Mesh / Curve Create the Mesh for the tower. a.Create / Mesh / Curve. b.Select Bar2 as the Topology. c.Click Curve List panel. d.Click Curve or Edge picking icon. e.Select all curves. f.Click –Apply-. There are 3 curves which do not exist in the range. If you input the range by hand, choose Yes to All for the error message d a b c f

10. WS16-10 MAR120, Workshop 16, December 2001 Step 3. Elements: Equivalence / All / Tolerance Cube Equivalence for Tower. a.Equivalence / All / Tolerance Cube. b.Click –Apply-. a b

11. WS16-11 MAR120, Workshop 16, December 2001 Step 4. Materials: Create / Isotropic / Manual Input Create the material property for the tower. a.Materials: Create / Isotropic / Manual Input. b.Enter steel as the Material Name. c.Click Input Properties. d.Enter 30e6 as the Elastic Modulus. e.Enter 0.3 as the Poisson Ratio. f.Enter 7.45e-4 as the Density. g.Click OK. h.Click Apply. d e f g a b c h

12. WS16-12 MAR120, Workshop 16, December 2001 i.Group: Post. j.Click Select None. k.Select horizontal_members. l.Click Apply. i j k l

13. WS16-13 MAR120, Workshop 16, December 2001 d e f g h i Step 5. Properties: Create / 1D / Elastic Beam Create the element properties for the beams. a.Properties: Create / 1D / Elastic Beam. b.Enter horizontal_members as the Property Set Name. c.Click Input Properties. d.Enter steel as the Material. e.Enter as the XZ Plane Definition. f.Enter 0.3436 as the Cross Sectional Area. g.Enter 3.35e-2 as the Ixx. h.Enter 3.35e-2 as the Iyy. i.Click OK. These properties represent a 1” OD pipe with 0.125” wall thickness. The beam lies along the XY Vector, the resultant of XYxXZ is the orientation for the beam strong axis a b c

14. WS16-14 MAR120, Workshop 16, December 2001 j.Click Select Members panel. k.Click Curve or Edge picking icon. l.Enter or drag select all curves. m.Click Add. n.Click –Apply-. o.Create the other Properties using the information provided below. Cross Section Area and Moments of Inertia are the same as entered above. Only the XZ Plane Definition changes. k j l m n Post other groups, one at a time, and then repeat steps a-n to assign the properties. Change the Property Set Name and XZ Plane Definition according to the table on the right: o

15. WS16-15 MAR120, Workshop 16, December 2001 Create the element properties guy wires. a.Group: Post. b.Click Select All. c.Click Apply. Step 6. Properties: Post a b c

16. WS16-16 MAR120, Workshop 16, December 2001 Step 7. Properties: Create / 1D / Truss Create the truss. a.Create / 1D / Truss. b.Enter wire as the Property Set Name. c.Click Input Properties. d.Enter steel as the Material Name. e.Enter 0.049 as the Cross- Sectional Area. f.Click OK. a b c d e f

17. WS16-17 MAR120, Workshop 16, December 2001 g.Click Select Members. h.Click Curve or Edge picking icon. i.Enter or select Curve 176:179. j.Click Add k.Click –Apply-. h i g j k

18. WS16-18 MAR120, Workshop 16, December 2001 Step 8. Load Cases: Create Create a base constraints load case for analysis. a.Load Cases: Create. b.Enter base as the Load Case Name. c.Select Static as the Load Case Type. d.Click –Apply-. a b c d

19. WS16-19 MAR120, Workshop 16, December 2001 Step 9. Fields: Create / Non Spatial / Tabular Input Create an input spectrum for the base excitation. a.Fields: Create / Non Spatial / Tabular Input. b.Enter Spectrum as the Field Name. c.Select Frequency from the Active Independent Variable. d.Click Input Data. e.Enter the following table for the Field that is in the Next Page. f.Click OK. g.Click –Apply-. f a b c d g 0.9751 2.5 3 4.5 2.56.6 2.258 210 1.1100 1.011000 0.29250.3 0.1950.2 0.009750.01 0.00048750.0005 0.00009750.0001 ValueFrequency This is a typical earthquake spectrum for rocklike material with a soil depth less than 200 ft, as provided by the UBC. The analyst should check for local codes which are relevant prior to conducting the analysis. e

20. WS16-20 MAR120, Workshop 16, December 2001 d e Step 10. Loads/BCs: Create / Displacement / Nodal Create a fixed the guy wire boundary condition. a.Load/BCs: Create / Displacement / Nodal. b.Enter guy_wire as the New Set Name. c.Click Input Data. d.Enter as the Translation vector. e.Click OK. As truss elements have no rotational degrees of freedom, we do not have to constrain them for this analysis. a b c

21. WS16-21 MAR120, Workshop 16, December 2001 f.Click Select Application Region. g.Click Geometry entity picking icon. h.Enter or Select Point 57:60. i.Click Add. j.Click OK. k.Click –Apply-. g h i j f k

22. WS16-22 MAR120, Workshop 16, December 2001 d e Step 11. Loads/BCs: Create / Displacement / Nodal Create a fixed boundary condition at the base of the tower. a.Create / Displacement / Nodal. b.Enter base as the New Set Name. c.Click Input Data. d.Enter as the Translation vector. e.Click OK. Do not constrain the rotational degrees of freedom at the base so that the guy wires must prevent tipping. a b c

23. WS16-23 MAR120, Workshop 16, December 2001 f.Click Select Application Region. g.Click Geometry entity picking icon. h.Enter or select Point 45. i.Click Add. j.Click OK. k.Click –Apply-. g h i j f k

24. WS16-24 MAR120, Workshop 16, December 2001 Step 12. Load Cases: Modify Create load case for unstressed analysis. a.Modify. b.Select base from the Select Load Case to Modify. c.Verify that: Displ_base, Displ_guy_wire have been selected. d.Click OK. e.Click –Apply-. c d a b e

25. WS16-25 MAR120, Workshop 16, December 2001 d g Step 13. Analysis: Analyze / Entire Model / Full Run Setup and run a unstressed spectrum response analysis. a.Analysis: Analyze / Entire Model / Full Run. b.Enter unstressed_spec as the Job Name. c.Click Translation Parameters. d.Click Solver Options. e.Select Non-Positive Definite. f.Click OK. g.Click OK. a b c e f

26. WS16-26 MAR120, Workshop 16, December 2001 h.Click Load Step Creation. i.Enter nostress_modal as the Job Step Name. j.Select Normal Modes as the Solution Type. k.Click Solution Parameters. l.Select Inverse Power Sweep as the Extraction Method. m.Enter 1000 as the Number of Modes. n.Enter 40,000 as the Max # of Iteration per Mode. o.Enter 1e-005 as the Convergence Tolerance. p.Enter 0 as the Initial Frequency. q.Enter 400 as the Highest Frequency. r.Click OK. h i j k l m n o p q r

27. WS16-27 MAR120, Workshop 16, December 2001 s.Click Select Load Case. t.Select base from the Available Load Cases. u.Click OK. v.Click Apply. w.Click Cancel. t u s v w

28. WS16-28 MAR120, Workshop 16, December 2001 x.Click Load Step Creation. y.Enter nostress_spec as the Job Step Name. z.Select Spectrum Response as the Solution Type. aa.Click Solution Parameters. bb.Enter 100 as the # of Modes for Response. cc.Select default translation and rotation parameters. dd.Select spectrum from the Displacement Response Spectrum. ee.Click OK. x y z aa bb cc dd ee

29. WS16-29 MAR120, Workshop 16, December 2001 ff.Click Select Load Case. gg.Select base from the Available Load Cases. hh.Click OK. ii.Click Apply. jj.Click Cancel. gg hh ff ii jj

30. WS16-30 MAR120, Workshop 16, December 2001 kk.Click Load Step Selection. ll.Select nostress_modal, nostress_spec from the Existing Job Steps. mm.Unselect Default_Static_Step to remove from analysis. nn.Click OK. oo.Click Apply. ll mm nn kk oo

31. WS16-31 MAR120, Workshop 16, December 2001 Step 14. Analysis: Read Results / Result Entities / Attach Read in the results from the spectrum response analysis. a.Read Results / Result Entities / Attach. b.Make sure that the Job Name is unstressd_spec. c.Click Apply. a b c

32. WS16-32 MAR120, Workshop 16, December 2001 Step 15. Results: Create / Quick Plot Post-process the results from the spectrum response. a.Results: Create / Quick Plot. b.Select nostress_spec, inc.1 from the Select Result Cases. c.Select Displacement, Translation from the Select Fringe Result. d.Select Displacement, Translation from the Select Deformation Result. e.Click Apply. The maximum displacement on the unloaded structure due to the spectrum input is 4.47”. a b c d e

33. WS16-33 MAR120, Workshop 16, December 2001 Step 16. Loads/BCs: Modify / Displacement / Nodal Modify the base constraint to provide a preload for the structure. a.Modify / Displacement / Nodal. b.Select base from the Select Set to Modify. c.Click Modify Data. d.Enter as the Translation vector. e.Click OK. f.Click –Apply-. The base point of the tower is deflected upwards 1” to preload the guy wires. This was done for simplicity in creating the load case. For a complete analysis, a pretensioning load case which considers the actual steps used during erection should be used to obtain the most accurate results. d e a b c f

34. WS16-34 MAR120, Workshop 16, December 2001 Step 17. Analysis: Analyze / Entire Model / Full Run Setup and run a prestressed spectrum response analysis. a.Analyze / Entire Model / Full Run. b.Enter prestressed_spec as the Job Name. c.Click Load Step Creation. d.Enter static as the Job Step Name. e.Click Solution Parameters. f.Select NonLinear as the Linearity. g.Select Large Displ. (Total Lagr.)/ Small Strains as the Nonlinear Geometric Effects. a b c d e f g

35. WS16-35 MAR120, Workshop 16, December 2001 h.Click Load Increment Parameters. i.Enter 10 as the # of Cutbacks. j.Enter 0.1 as the Trial Time Step Size. k.Enter 1.2 as the Time Step Scale Factor. l.Enter 0.0001 as the Minimum Time Step. m.Enter 0.2 as the Maximum Time Step. n.Enter 1000 as the Maximum # of Steps. o.Enter 1 as the Total Time. p.Enter 25 as the # of Steps of Output. q.Click OK. r.Click OK. i j k l m n o p q h r

36. WS16-36 MAR120, Workshop 16, December 2001 s.Click Select Load Case. t.Select base from the Available Load Cases. u.Click OK. v.Click Apply. w.Click Cancel. t u s v w

37. WS16-37 MAR120, Workshop 16, December 2001 x.Click Load Step Selection. y.Select static, nostress_modal, nostress_spec from the Existing Job Steps. z.Unselect Default_static_Step. aa.Click OK. bb.Click Apply. bb x aa y z

38. WS16-38 MAR120, Workshop 16, December 2001 Step 18. Analysis: Read Results / Result Entities / Attach. Read in the results from the spectrum response analysis. a.Read Results / Result Entities / Attach. b.Make sure that the Job Name is prestressd_spec. c.Click Apply. a b c

39. WS16-39 MAR120, Workshop 16, December 2001 Step 19. Results: Create / Quick Plot Post-process the results from the spectrum response analysis. a.Create / Quick Plot. b.Select nostress_spec, inc.1 from the Select Result Cases. c.Select Displacement, Translation from the Select Fringe Result. d.Select Displacement, Translation from the Select Deformation Result. e.Click Apply. The maximum displacement on the preloaded structure due to the spectrum input is 4.51”. This indicates that the compressive forces in the tower provide a stress softening effect. It should be noted that spectrum response analyses can be performed at any time during a linear or nonlinear solution cycle in order to determine the response of the deflected structure a b c d e

40. WS16-40 MAR120, Workshop 16, December 2001