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

3. 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.

4. 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.

5. 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

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

7. 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

8. 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

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

10. 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

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

12. 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 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

13. 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

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

15. 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 as Cross-Sectional Area.
Click OK to close form. a c
wire b f
m:steel
0.049 d e

16. 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

17. 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

18. 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

19. 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.

20. 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

21. 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

22. 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

23. 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

24. 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

25. 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

26. 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

27. 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

28. 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

29. 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

30. 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

31. 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

32. 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

33. 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

34. 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.

35. 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.