FREQUENCY RESPONSE ANALYSIS OF TRANSMISSION TOWER WORKSHOP 15 FREQUENCY RESPONSE ANALYSIS OF TRANSMISSION TOWER

Problem Description: This model represents a transmission tower such as those used to broadcast radio and television signals. The model will be pre-loaded to simulate the tensioning of the guy wires for the tower. After this pretensioning analysis, the model will be subjected to a frequency response analysis in order to determine its response to a load applied at the tip of the tower.

Suggested Exercise Steps: Objectives: Creation of preload static step. Set-up and solution of frequency response analysis. Interpretation of results from frequency response analysis. Required: Tower.ses is required. Suggested Exercise Steps: Read the Tower.ses file to create geometry. Mesh the model using 1 element per curve. Apply the model properties. Apply the model boundary conditions. Set-up and solve the complete frequency response analysis. Interpret results.

CREATE NEW DATABASE a d c e b Open a new database. Name it tower_freq.db File: New Type tower_freq as File name Click OK. Select MSC.Marc as the Analysis Code. tower_freq d MSC.Marc q c e b tower_freq

Step 1. File: Session / Play c b open_can.ses Opener Open the session file. File: Session / Play. Select tower.ses file. Click -Apply-.

Step 2. Elements: Create / Mesh Seed/ Uniform Create the mesh Elements: Create / Mesh Seed / Uniform. Select Number of Elements. Enter 1 as Number. Click Into Curve List panel. Select the Curve or Edge picking icon. Drag select all curves, or input: Curve 1:179. a f b c 1 d Curve 1:179 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

Step 3. Elements: Create / Mesh / Curve Select Bar2 for Topology. Click Into Curve List panel. Select the Curve or Edge picking icon. Input, or drag-select: Curves 1:179. Click –Apply-. a e b c Curve 1:179 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 f d

Step 4. Elements: Equivalence / All / Tolerance Cube Equivalence the nodes Equivalence / All / Tolerance Cube. Click -Apply-. b a

Step 5. Materials: Create / Isotropic / Manual Input Create the tower material Materials: Create / Isotropic / Manual Input. Enter steel as Material Name. Open Input Properties form. Select Elastic. Enter 30e6 as Modulus. Enter 0.3 as Poisson Ratio. Enter 7.45e-4 as Density. Click OK. Click -Apply-. steel b c a i 30e6 d e 0.3 7.45e-4 f g h

Step 6. Group: Post a b c Select appropriate beams Group: Post. Select horizontal_members. Click Apply. b c

Step 7. Properties: Create / 1D / Elastic Beam Create material properties Properties: Create / 1D / Elastic Beam. Enter horizontal_members as Property Set Name. Open Input Properties form. Enter steel as Material. Enter <0 0 1> as XZ Plane. Enter 0.3436 as Cross Sectional Area. Enter 3.35e-2 as Ixx and Iyy. Click OK to close form. h steel <0 0 1> 0.3436 3.35e-2 f g e d a b horizontal_members c 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

k i l j m Click in Select Members panel. Select Curve or Edge icon. Input or drag select: Curve 1:44. Click Add. Click -Apply- to create property. Curve 1:44 i l horizontal_members m k Repeat steps 6-7 to assign the following additional orientations: vertical_members: <1,0,0> cross_orient1: <1,-1,0> cross_orient2: <1,1,0> cross_orient3: <1,1,0> cross_orient4: <1,-1,0> j

Step 8. Group: Post a b c Open the cover group. Group: Post. Select Select All. Click Apply. b c

Step 9. Properties: Create / 1D / Truss Create the wire property Properties: Create / 1D / Truss. Enter wire as Property Set Name. Open Input Properties form. Enter steel as Material. Enter 0.049 as Cross-Sectional Area. Click OK to close form. a c wire b f m:steel 0.049 d e

i g j k h Click in Select Members panel. Select Curve or Edge icon. Input or select Curve 176:179. Click Add. Click -Apply-. i g Curve 176:179 j h k

Step 10. Load Case: Create a b c d Create the preload case loads for analysis Load Case: Create. Enter preload as Load Case Name. Select Time Dependent for Load Case Type. Click -Apply- to Create Case. a b preload c d

Step 11. Fields: Create / Non Spatial / Tabular Input Create a unit field for non-time varying loads Fields: Create / Non Spatial / Tabular Input. Enter constant_on as Field Name. Select Time as Independent Variable. Open the Input Data form. Input the following points for the Field: (0,1),(100,1) This is an always unity field. Click OK to close form. Click -Apply- to create field. a b c d g constant_on e f

Step 12. Loads/BCs: Create / Displacement / Nodal Create a wire boundary condition Loads/BCs: Create / Displacement / Nodal. Enter guy_wire as set name. Open Input Data form. Enter <0 0 0> as Translations <T1 T2 T3>. Select constant_on for Time/Freq. Dependence. Click OK to close form. a b guy_wire c d <o, o, o> constant_on f e As truss elements have no rotational degrees of freedom, we do not have to constrain them for this analysis.

h i j k g l Click Select Application Region…. Select the Geometric entity picking icon. Select or Input: Point 57:60. Click Add. Click OK to close form. Click -Apply- to create displacement. g l guy_wire j k i h

o p m q n Enter preload as New Set Name. Click Input Data…. Enter <0 0 1> as Translations <T1 T2 T3>. Select constant_on for Time/Freq. Dependence. Click OK. o <0, 0, 1> q constant_on p m preload n

s t u v r w Click Select Application Region…. Select the Geometric entity picking icon. Select or input point 45. Click Add. Click OK. Click -Apply-. w r preload guy_wire v u Point 45 t s

Step 13. Loads/BCs: Create / Force / Nodal Create a driving force for the tower Create / Force / Nodal. Enter nodal_force as New Set Name. Click Input Data…. Enter <0,1000,0> for Force <F1 F2 F3>. Select constant_on Time/Freq. Dependence. Click OK. b c a Nodal_force d e f <0, 1000, 0> constant_on

h i j k g l Click Select Application Region…. Select Geometric entity icon. Select or input point 56. Click Add. Click OK. Click -Apply-. l g i k j h

c a b d e Check load case for prestressed analysis Load Case: Modify. Select preload as Load Case. Verify that guy_wire, preload and nodal_force have been selected. Click OK. Click -Apply-. e preload a b c d

Step 14. Analysis: Analyze / Entire Model / Full Run Run the analysis Analysis: Analyze / Entire Model / Full Run. Enter prestressed_freq_job1 as Job Name. Click Translation Parameters…. Click Solver Options…. Select Non-Positive Definite. Click OK. Click Load Step Creation…. a e Entire Model q d Full Run q f b prestreessed_freq_job c h g

l m n q o i j k p r s u v t Enter prestress as Job Step Name. Select Static as Solution Type. Click Solution Parameters…. Click Load Increment Parameters…. Select Fixed for Increment Type. Enter 10 as Number of Increments Enter 1 as Total Time. Click OK. Click Select Load Case…. Choose preload as Load Case. Click Apply. Click Cancel. i k j r u prestress v p 10 1 n m o s t

aa bb cc dd x y ee z ff w gg ii hh Click Load Step Creation…. 1000 0.0 400 bb dd Click Load Step Creation…. Enter prestress_modal as Job Step Name. Select Normal Modes as Solution Type. Click Solution Parameters…. Select Lanczos for Extraction Method. Enter 1000 as Number of Modes. Enter 0.0 as Lowest Frequency. Enter 400 as Highest Frequency. Click OK. Click Select Load Case…. Choose preload as Load Case. Choose OK. Choose -Apply-. w x y z ff Prestress_modal ii cc gg hh

mm nn jj oo pp kk ll qq rr tt uu ss Input prestressed_freq as Job Step Name. Select Frequency Reponse for Solution Type. Click Solution Parameters…. Enter 0.0 as Lowest Excitation Freq. Enter 1 as Excitation Freq. Interval. Enter 400 as Number of Excitation Frequencies. Click OK. Click Select Load Case…. Select preload as Load Case. Click -Apply-. Click Cancel. kk prestressed_freq ll qq jj tt uu pp 0.0 1 400 mm oo nn rr ss

ww xx yy vv zz Open Load Step Selection form. Select prestress, prestress_modal and prestress_freq. Deselect the Default Static Step in Selected Job Steps panel. Click OK. Click Apply. vv zz ww xx yy

Step 15. Analysis: Read Results / Result Entities / Attach Read (Attach) results Read Results / Result Entities / Attach. Select prestressed_freq_job1. Click Apply. c a b

Step 16. Results: Read Results / Graph / Y vs. X Post-process the results Results: Create / Graph / Y vs. X. Select prestressed_freq as Result Case. Click Filter. Click -Apply-. Click Close. a b c d e

j l f g h i k m Select Displacement, Translation for Result. Select Magnitude for Quantity. Select Global Variable for X. Select Frequency for Variable. Click pick target icon. Select Node icon. Select Node 210. Click -Apply-. j g h i f m l k

The plot shows the tip’s deflection based on the frequency of the applied load. Per classical dynamics, the response to the load becomes zero as the frequency approaches infinity.

Step 17. Results: Create / Quick Plot Open the Results form Create / Quick Plot. Select prestress, A1; Dynamic Incr. 5. Select Stress, Global System for Select Fringe Result. Select Displacement, Translation for Select Deformation Result. Click -Apply-. d c b a e Frequency response analysis provides an efficient means of determining a structure’s response to harmonic excitations. The technique does not determine the transient response of the structure, so it is often non-conservative in its results. For instances where the transient response is known to be negligible, such as in machine vibration problems, the frequency response technique provides the most efficient means of analysis.