Download the following file
0. Content
|
1. Overview |
1-1 Initial Cable Pretension Analysis Considering Construction Stages 1-2 Bridge Dimensions 1-3 Loading |
|---|---|
|
2. Work Environment Setting |
|
|
3. Definition of Properties |
3-1 Definition of Material Properties 3-2 Definition of Section Properties |
|
4. Modeling of Structure |
4-1 Input Nodes 4-2 Input Elements |
|
5. Input Boundary Conditions |
5-1 Input Supports 5-2 Input Beam End Offsets 5-3 Rigid Body Connection 5-4 Modeling Bridge Supports |
|
6. Input Loads |
6-1 Define Loading Conditions 6-2 Input Self Weight 6-3 Superimposed Dead Load 6-4 Self-Weight of Cross Beams 6-5 Input Pretension Loads 6-6 Perform Structural Analysis |
|
7. Calculate Initial Pretension |
7-1 Create Load Combinations 7-2 Calculate Unknown Load Factors |
| 8. Review Analysis Results |
8-1 Review Deformed Shape 8-2 Review Member Forces |
1. Overview
Cable-stayed bridges are structural systems effectively composed of cables, main girders and towers. This bridge form has a beautiful appearance and easily blends in with the surrounding environment due to the fact that various structural systems can be created by changing the tower shapes and cable arrangements.
Cable-stayed bridge is a bridge type where inclined cables transfer member forces induced in the girder. High compression is induced in the tower and main girder due to the structural system. Considering the above features, PC cable-stayed bridges using Prestressed Concrete material for the main girder, have following advantages:
- High buckling resistance compared to steel cable-stayed bridges because of the high stiffness of the tower and the main girder
- High wind and earthquake resistance compared to steel cable-stayed bridges because of the higher weight, stiffness, and damping ratio
- Concrete cable-stayed bridges are better than steel cable-stayed bridges in terms of serviceability as the stiffness of main girder is large, and thus the deflection due to live load is small (resulting in good control of noise/vibration).
- Low cost and easy maintenance compared to steel cable-stayed bridges
- Efficient constructability because it essentially consists of cantilevers, and can be built by constructing out from the towers.
- Economical because the minimized girder depth allows large space under the bridge and this type of bridge allows shorter approach length.
Cable-stayed bridge
1-1 Initial cable pretension analysis considering construction stages
The dominant issue of the design and build of a cable-stayed bridge is to compute and achieve the initial equilibrium configuration at the completed state. The initial equilibrium configuration of cable-stayed bridges is the equilibrium position due to dead load and tension forces in the stay cables. It is called “initial cable pretension analysis” to optimize the cable pretension in order to improve section forces in the main girders and towers and support reactions in the bridge.
In order to guide the construction of each erection stage, backward analysis is commonly adopted, in which the bridge is disassembled stage by stage from the completed state until just before the first pairs of cables are jacked. The forward analysis starting from any construction stage will predict the states in the successive stages by simulating the actual construction procedures.
This tutorial uses an example of non-symmetrical, cable-stayed bridges. Ideally in backward stage analysis, at key segment closure, shear force and bending moment should be close to 0. However, if backward analysis is applied in this case, non-zero shear force and bending moment occur due to non-symmetry. Thus, it is impossible to apply backward stage analysis in this case. In addition, with backward stage analysis, concrete material effect cannot be considered. Errors due to concrete construction with time can be eliminated by forward iteration analysis. Sequential tensioning and erection sequence, as shown in the first following figure, cannot be represented by backward analysis.
On the other hand, forward stage analysis follows the real erection sequence. It takes more time for the designer as he/she has to conduct trial-and-error analysis to determine the limiting member forces due to cable tension up to a certain range.
In this tutorial, forward stage analysis is used. In the forward stage analysis, it is necessary to know the cable pretensions at each construction stage, which give the initial equilibrium configuration at the completed state due to dead load.
The following second figure shows the sequence for initial cable pretension analysis with construction stages considered.
Construction Stage Cycle
Flow chart for the initial cable pretension analysis considering construction stages
1-2 Bridge Dimensions
This tutorial has been based on a real project of a PC cable-stayed bridge, and has been simplified since it will still suffice for educational purpose. We will learn how to calculate the initial force in the cable from this tutorial. Before performing initial cable pretension analysis with Construction Stages, initial cable forces due to the dead load at the final stage should be first calculated.
The figures and loadings for the bridge are as follows:
| Bridge type | PC cable-stayed bridge |
|---|---|
| Bridge length (L) | L=46.5+113.5+260+100 = 520.0 m |
| Main girder | Beam and slab type concrete section |
| Tower | Concrete section |
| Number of cables | 52x2 pair = 104 |
| Install 4 key blocks in 1, 2, 3, 4 spans | |
| Put 2 elastic bearings on PY1, PY2 |
General Layout of Bridge Structure
1-3 Loading
Self-Weight: Automatically calculated by the program
Superimposed dead load:
| Unit weight (kN/m) | Remark | |
|---|---|---|
| Pavement | 35.75 | 2.3 x 0.08 x 19.43 |
| Railing | 7.28 | |
| Parapet | 14.76 | |
| Sum | 57.75 |
Self-weight of cross beams: Enter the weight of cross beams, which were excluded in the modeling, using Nodal Loads.
2. Work Environment Setting
To perform the analysis of a PC cable-stayed bridge open a new file and save it under the name ‘PC.mcb’.
Assign ‘kN’ for Force (Mass) unit and ‘m’ for Length unit. This unit system can be changed any time during the modeling process as per the convenience of the user.
1. Click New Project
2. Click Save
3. Save file as 'PC'
Main menu >[Project] Tab > [Setting] Group > Unit System
The status Bar is located on the bottom of the screen and the units can be changed by clicking on it .
1. Confirm 'm' in the Length, 'kN (ton)' in the Force (Mass).
2. Click the button.
Unit system settings
3. Definition of Properties
3-1 Definition of Material Properties
Input material properties of cables and bridge deck in the Material Data dialog box.
| ID | Name | Type of Design | Standard | Modulus of Elasticity | Poisson's Ratio | Thermal Coefficient | Weight Density |
|---|---|---|---|---|---|---|---|
| 1 | Main | Concrete | None | 2.7389E+07 | 0.167 | 1.0E-05 | 24.52 |
| 2 | Sub | Concrete | None | 2.6063E+07 | 0.167 | 1.0E-05 | 24.52 |
| 3 | Cable | Steel | None | 2.0594E+08 | 0.3 | 1.2E-05 | 76.98 |
Main Menu > [Properties] Tab > [Material] group > Material Properties
1. Click the button
2. Enter 'Main Con'c' in the Name field
3. Select 'Conceret' in the Type of Design checkbox and select 'None' in Standard checkbox
4. In the Modulus of Elasticity field, enter '2.7389e+07'
5. In the Poisson's Ratio field, enter '0.167'
6. In the Thermal Coefficient field, enter '1.0e-05'
7. In the Weight Density field, enter '24.52'
8. Click the button
Refer to the table above and input the remaining materials for Sub Con'c and Cable in the same way as above.
Define Material Properties
3-2 Define Section Properties
With Section Property Calculator (SPC), section properties for irregular shape can be easily obtained and even the shape can be depicted in MIDAS CIVIL. Import the *.sec file drawn in SPC to define main girder sections (101, 102 and 103).
Main Menu > [Properties] Tab > [Section] Group > Section Properties
1. Click the button.
2. In PSC tab, Select 'PSC-Value' in drop-down menu.
3. Confirm '101' in the Section ID field.
4. Type 'D-Center' in the Name field.
5. Select 'Import from SPC' under button and invoke 'D_center.Sec'.
Referring to the guide diagram, enter the design parameters in the “Param. for Design Input” cell. These parameters are used for section capacity check, but not used for analysis. For sections 102 and 103, enter the same parameters.
Input dimensions for PC box section
PC Section
| ID | Type | Sub Type | Name | *.sec File Name | Remarks |
|---|---|---|---|---|---|
| 101 | PSC | PSC-Value |
D_center |
D_center.sec | Center part |
| 102 | PSC | PSC-Value | D_spt | D_support.sec | Support part |
| 103 | PSC | PSC-Value | D_py | D_py.sec | Tower part |
Tower Section
| ID | Type | Name |
|---|---|---|
| 201 | Value | PY1_head |
| 202 | Value | PY1_top |
| 203 | Value | PY1_down |
| 204 | DB/User | PY1_cross |
| 205 | DB/User | PY1_footing |
| 211 | Value | PY2_head |
| 212 | Value | PY2_top |
| 213 | Value | PY2_down |
| 214 | DB/User | PY2_cross |
| 215 | DB/User | PY2_footing |
Pier Section
Input 301~304 in Section ID in DB/User Type for modeling the pier section.
Cable Section
401~409 sections to be used for cables are defined by Value Type. Import *.sec file to define the main girder section. To define other sections, copy the data on the section tab of "12. PC Cable-stayed bridge Part I_Struc.xls" file and paste it into the section table. Classify Section Types into each tab as the type of data and the number of data are different from Section Type to Section Type.
Main Menu > [Properties] tab > [Tables] Group > Property Tables > Section
(using the provided excel file (12. PC Cable-stayed bridge Part I_Struc.xls), copy data accordingly)
Section table input
4. Modeling of Structure
4-1 Input Nodes
Input node data in "12. PC Cable-stayed bridge Part I_Struc.xls" file and copy the node information from the file into the Node Tables.
Main Menu > [Node/Element] Tab > [Node Detail] Group > Nodes Table
To copy and paste Node Data into Node Table, activate the Node Column as shown below. Right-click over the Node column and select “Enable Edit”. Now the Node column becomes enabled.
Copy the Node Data from the MS-Excel (12. PC Cable-stayed bridge Part I_Struc.xls) file and input it in the Table.
Node Information and Input Table
4-2 Input Elements
Likewise, enable the Element No. Column for pasting the data into the table. Copy the Element Data from Excel File and paste it into the table.
Main Menu > [Node/Element] Tab > [Element Detail] Group > Elements Table
Main girder
Main girder numbers are 101 ~ 317 from the left.
Cable
Cable numbers are 1001 ~ 1032, 2001 ~ 2052 from the left. Numbers in parentheses indicate the rear cables.
Tower and Pier
| Main tower | Small tower | Pier |
|---|---|---|
| 501to561 | 601to656 | 701to719 |
5. Input Boundary Conditions
5-1 Input Supports
Input the supports as shown in the figure below.
Main menu > [Boundary] Tab > [Supports] Group > Define Supports
1. Select nodes '389, 390, 397, 398, 2311, 2780, 3106' with Select Single.
2. Select 'Default' in the Boundary Group Name.
3. Select 'Add' in the Option.
4. Check on 'Dx, Dy, Dz, Rx, Ry, Rz' in the Supoort Type.
5. Click the button.
Input Supports
5-2 Input Beam End Offset
Input the width of Beam End Offset at the pier step.
Main Menu > [Boundary] Tab > [Release/Offset] Group > Beam End Offsets
| Elem | Type | RGDXi | RGDYi | RGDZi | RGDXj | RGDYj | RGDZj |
|---|---|---|---|---|---|---|---|
| 710 | Global | 0.0 | 1.72 | 0.0 | 0.0 | 0.0 | 0.0 |
| 715 | Global | 0.0 | 0.0 | 0.0 | 0.0 | -1.72 | 0.0 |
5-3 Rigid Body Connection
Enter rigid body connection between the main girder and cable anchorages, and between the tower and cable anchorages. Copy the data on Rigid Link tab of "12. PC Cable-stayed bridge Part I_Struc.xls" and paste it into Rigid Link Table.
Main Menu > [Boundary] Tab > [Tables] Group > Boundary Tables > Rigid Link
Later input the rigid body connection at the same location.
PC girder, tower and cable anchorages
Anchorage of cable with PC girder and Tower
5-4 Modeling Bridge Supports
Input Elastic Links at bridge supports connecting the bridge superstructure to the substructure.
Main Menu > [Boundary] Tab > [Links] Group > Elastic Link
Locations for installing bridge support
Input the data for elastic links at the bridge supports as shown in the table below [Unit: kN, m]:
| No. | Node1 | Node2 | Type | SDx | SDy | SDz | Remarks |
|---|---|---|---|---|---|---|---|
| 1 | 390 | 392 | GEN | 1E+11 | 1E+11 | 0 | Pot support |
| 2 | 389 | 391 | GEN | 1E+11 | 1E+11 | 0 | Pot support |
| 3 | 567 | 394 | GEN | 25230100 | 20670 | 20670 | Elastic support |
| 4 | 561 | 393 | GEN | 25230100 | 20670 | 20670 | Elastic support |
| 5 | 667 | 396 | GEN | 23870000 | 19810 | 19810 | Elastic support |
| 6 | 661 | 395 | GEN | 23870000 | 19810 | 19810 | Elastic support |
| 7 | 398 | 400 | GEN | 1E+11 | 1E+11 | 0 | Pot support |
| 8 | 397 | 399 | GEN | 1E+11 | 1E+11 | 0 | Pot support |
| 9 | 1009 | 168 | GEN | 0 | 7808220 | 0 | Wind Shoe |
| 10 | 1010 | 275 | GEN | 0 | 7808220 | 0 | Wind Shoe |
| 11 | 3013 | 3015 | GEN | 1E+11 | 1E+11 | 0 | Pot support |
| 12 | 3012 | 3014 | GEN | 1E+11 | 1E+11 | 0 | Pot support |
6. Input Loads
6-1 Define Loading Conditions
The loading conditions used in the analysis are defined.
Main menu > [Load] Tab > [Load Type] Group > Static Loads
[Create Load Cases] Group > Static Load Cases
1. Enter 'Self' in the Name.
2. Select 'Dead Load' in the Type.
3. Click the button.
4. Enter '2nd Dead' in the Name.
5. Select 'Dead Load' in the Type.
6. Click the button.
7. Enter 'Cross W't' in the Name.
8. Select 'Dead Load' in the Type.
9. Click the button.
10. Enter 'Pre01' in the Name.
11. Select 'Prestress' in the Type.
12. Click the button.
Input the loading cases repeatedly from Name (Pre02) to Name (Pre52).
Define Load Case Dialog Box
6-2 Input Self-Weight
Input the self weight as follows.
Main menu > [Load] Tab > [Load Type] Group > Static Loads > [Static Loads] Group > Self Weight
1. Select 'Self' in the Load Case Name.
2. Select 'Default' in the Load Group Name.
3. Enter '-1' in the Z of the Self Weight Factor.
4. Click the button.
Input self weight
6-3 Input Superimposed Dead Load
Apply the 2nd dead load by inputting it as Element Beam Load.
Main menu > [Load] Tab > [Load Type] Group > Static Loads > [Static Loads] Group > Beam Loads > Element
1. Click Select Elements by Identifying...
2. Select 'Section' in the Select Type.
3. Select 'D_center, D_spt, D_py' in the Section field.
4. Click the button and Click the
button.
5. Select '2nd Dead' in the Load Case Name.
6. Select 'Default' in the Load Group Name.
7. Confirm 'Add' in the Option.
8. Select 'Uniform Loads' on the Load Type.
9. Select 'Global Z' in the Direction.
10. Confirm 'Relative' in the Value.
11. Enter '0' in the x1, '1' in the x2, '-56.633' in the w field.
12. Click the button.
Apply 2nd Dead Load
6-4 Input Self Weight of Cross Beams
Enter the weight of cross beams, which was excluded from the modeling, using nodal loads. Copy the loading information from the Load tab in "12. PC Cable-stayed bridge Part I_Struc.xls" and paste it into Nodal Load Table.
Main menu > [Load] Tab > [Load Type] Group > Static Loads > [Structure Loads] Group > Nodal Loads
6-5 Input Pretension Loads
For the case of a symmetric cable-stayed bridge, as is the case in this tutorial, identical initial pretension in the cables will be introduced to each of the corresponding cable symmetric to the bridge center. Therefore, we will input identical loading conditions to the cable pairs that form the symmetry.
Main menu > [Load] Tab > [Load Type] Group > Prestress
[Prestress Loads] Group > Pretension Loads
1. Click Select Intersect and select elements '1001, 2001'
2. Select 'Pre01' in the Load Case Name.
3. Select 'Default' in the Load Group Name.
4. Confirm 'Add' in the Options.
5. Enter '1' in the Pretension Load.
6. Click the button.
7. Click Select Intersect and select elements '1002, 2002'
8. Select 'Pre02' in the Load Case Name.
9. Select 'Default' in the Load Group Name.
10. Confirm 'Add' in the Options.
11. Enter '1' in the Pretension Load.
12. Click the button.
Input the unit pretension loads for all the cables repeatedly from 'Pre03' to 'Pre52' and select elements in sequence from '1003, 2003' to '1052, 2052' respectively.
Input Pretension Loads
6-6 Perform Structural Analysis
After completing all the processes for modeling and load input, structural analysis is performed.
Main menu > [Analysis] Tab > [Perform] Group > Perform Analysis
7. Calculate Initial Pretension
7-1 Create Load Combination
Create a load combination from the 52 unit pretension load cases introduced to each cable, self weight load case, and superimposed dead load case and cross beam self weight load case.
Main menu > [Results] Tab > [Result Type] Group > Analysis Result > [Combination] Group > Load Combination
1. In General tab, Enter 'LCB 1' in the Name of the Load Combination.
2. Select 'Active' in the Active.
3. Select 'Add' in the Type.
4. Select 'Self (ST)' in the LoadCase and enter '1.0' in the Factor.
5. Select '2nd Dead (ST)' in the LoadCase and enter '1.0' in the Factor.
6. Select 'Pre01 (ST)' in the LoadCase and enter '1.0' in the Factor.
7. Select 'Pre02 (ST)' to 'Pre15 (ST)' in the LoadCase and enter '1.0' in the Factor.
8. Select 'Pre16 (ST)' in the LoadCase and enter '250' in the Factor.
9. Select 'Pre17 (ST)' in the LoadCase and enter '250' in the Factor.
10. Select 'Pre18 (ST)' to 'Pre52 (ST)' in the LoadCase and enter '1.0' in the Factor.
11. Click the button.
Input Load Combinations
7-2 Calculate Unknown Load Factors
Calculate unknown load factors that satisfy the boundary conditions by the Unknown Load Factor function for LCB 1, which was generated through load combination. The constraints are specified to limit the deflection of the tower and the main girders.
Specify the load condition, constraints and method of forming the object function in Unknown Load Factor. First, we define the cable unit loading conditions as unknown loads.
Main menu > [Results] Tab > [Result Type] Group > Bridge Specialization > [Cable Bridge] Group > Cable Control > Unknown Load Factor
1. Click the [Add New] button.
2. Enter 'Unknown' in the Item Name.
3. Select 'LCB 1' in the Load Comb.
4. Confirm 'Square' in the Object function type.
5. Confirm 'Both' in the Sign of unknowns.
6. Check off 'Self', '2nd Dead', 'CrossW't' in LCase.
Unknown Load Factors
Specify the constraining conditions, which restrict the displacement of the tower and the main girders by using the Constraints function.
Input Constraint Conditions
The boundary conditions for the Unknown Load Factors can also be applied through the MCT Command Shell.
Refer to the table below for inputting the constraint conditions for calculating the unknown load factors.
| Name | Node | Node ID | Type | Upper | Lower |
|---|---|---|---|---|---|
| py101 | 554 | RY | Inequality | 1.00E-06 | -1.00E-06 |
| py201 | 645 | RY | Inequality | 1.00E-06 | -1.00E-06 |
| sp02 | 107 | DZ | Inequality | 0.001 | -0.001 |
| sp03 | 111 | DZ | Inequality | 0.001 | -0.001 |
| sp04 | 115 | DZ | Inequality | 0.001 | -0.001 |
| sp05 | 119 | DZ | Inequality | 0.001 | -0.001 |
| sp06 | 123 | DZ | Inequality | 0.001 | -0.001 |
| sp07 | 127 | DZ | Inequality | 0.001 | -0.001 |
| sp08 | 131 | DZ | Inequality | 0.001 | -0.001 |
| sp09 | 135 | DZ | Inequality | 0.001 | -0.001 |
| sp10 | 139 | DZ | Inequality | 0.001 | -0.001 |
| sp11 | 143 | DZ | Inequality | 0.001 | -0.001 |
| sp12 | 147 | DZ | Inequality | 0.001 | -0.001 |
| sp13 | 151 | DZ | Inequality | 0.001 | -0.001 |
| sp14 | 155 | DZ | Inequality | 0 | -0.001 |
| sp15 | 159 | DZ | Inequality | 0 | -0.001 |
| sp16 | 163 | DZ | Inequality | 0.001 | -0.001 |
| sp17 | 173 | DZ | Inequality | 0.001 | -0.001 |
| sp18 | 177 | DZ | Inequality | 0 | -0.001 |
| sp19 | 181 | DZ | Inequality | 0 | -0.001 |
| sp20 | 185 | DZ | Inequality | 0.001 | -0.001 |
| sp21 | 189 | DZ | Inequality | 0.001 | -0.001 |
| sp22 | 193 | DZ | Inequality | 0.001 | -0.001 |
| sp23 | 197 | DZ | Inequality | 0.001 | -0.001 |
| sp24 | 201 | DZ | Inequality | 0.001 | -0.001 |
| sp25 | 205 | DZ | Inequality | 0.001 | -0.001 |
| sp26 | 209 | DZ | Inequality | 0.001 | -0.001 |
| sp27 | 213 | DZ | Inequality | 0.001 | -0.001 |
| sp28 | 217 | DZ | Inequality | 0.001 | -0.001 |
| sp29 | 221 | DZ | Inequality | 0.001 | -0.001 |
| sp30 | 225 | DZ | Inequality | 0.001 | -0.001 |
| sp31 | 229 | DZ | Inequality | 0.001 | -0.001 |
| sp32 | 233 | DZ | Inequality | 0.001 | -0.001 |
| sp33 | 234 | DZ | Inequality | 0.001 | -0.001 |
| sp34 | 238 | DZ | Inequality | 0.001 | -0.001 |
| sp35 | 242 | DZ | Inequality | 0.001 | -0.001 |
| sp36 | 246 | DZ | Inequality | 0.001 | -0.001 |
| sp37 | 250 | DZ | Inequality | 0.001 | -0.001 |
| sp38 | 254 | DZ | Inequality | 0.001 | -0.001 |
| sp39 | 258 | DZ | Inequality | 0 | -0.001 |
| sp40 | 262 | DZ | Inequality | 0 | -0.001 |
| sp41 | 266 | DZ | Inequality | 0 | -0.001 |
| sp42 | 270 | DZ | Inequality | 0.001 | -0.001 |
| sp43 | 280 | DZ | Inequality | 0.001 | -0.001 |
| sp44 | 284 | DZ | Inequality | 0 | -0.001 |
| sp45 | 288 | DZ | Inequality | 0 | -0.001 |
| sp46 | 292 | DZ | Inequality | 0 | -0.001 |
| sp47 | 296 | DZ | Inequality | 0.001 | -0.001 |
| sp48 | 300 | DZ | Inequality | 0.001 | -0.001 |
| sp49 | 304 | DZ | Inequality | 0.001 | -0.001 |
| sp50 | 308 | DZ | Inequality | 0.001 | -0.001 |
| sp51 | 312 | DZ | Inequality | 0.001 | -0.001 |
We now check the constraints used to calculate the cable initial pretension and unknown load factors in Unknown Load Factor Result.
Make Load Combination using the Unknown Load Factors which are automatically created for the Load Combination.
Generate the Influence Matrix as a MS-Excel File from the calculation results of Unknown Load Factors.
Unknown Load Factors.
1. Click the [Get Unknown Load Factors] button.
The following figure shows the analysis results for calculating the Unknown Load Factors.
Unknown Load Factor Calculation Results
We will now check whether the calculation results satisfy the constraints by auto-generating a new load combination using the unknown load factors in the Make Load Combination function.
Automatic generation of “ULF” load combination using the unknown load factors
Confirm the results of the load combination that is automatically generated using the unknown load factors.
Main menu > [Results] Tab > [Result Type] Group > Analysis Result > [Combination] Group > Load Combination
Automatic Generation of “ULF” Load Combination that uses the Unknown Load Factor
8. Review Analysis Results
8-1 Review Deformed Shape
Review the deformed shape for the “ULF” load combination, which includes the Unknown Load Factors calculated for the initial tension.
Main menu > [Results] Tab > [Result Type] Group > Analysis Result > [Result Display] Group > Deformations > Deformed Shape
1. Select 'CB : ULF' in the Load Cases/Combinations.
2. Confirm 'DZ' in the Components.
3. Check on 'Undeformed', 'Legend' in the Type of Display.
4. Click the button.
Deformed Shape Results
8-2 Review Member Forces
Review the member forces for the “ULF” load combination.
Main Menu > [Results] Tab > [Result Type] Group > Analysis Result > [Result Display] Group > Forces > Beam Diagrams
1. Select 'CB:ULF' in the Load Cases/Combinations.
3. Confirm 'My' in the Components.
4. Confirm '5 Points', 'Line Fill' in the Display Options.
5. Enter '1.0' in the Scale.
6. Check on 'Undeformed', 'Legend' in the Type of Display.
7. Check off 'Deform' in the Type of Display.
8. Click the button.
Review Member Forces