Download the following files
0. Contents
| 1. Summary |
1-1 Model Shape and Summary 1-2 Detailed Model View 1-3 Load Cases |
|---|---|
| 2. File Opening and Preferences Setting |
2-1 Unit System Configuration |
| 3. Enter Material and Section Properties |
3-1 Define Material Properties 3-2 Define Section Properties |
| 4. Structural Modeling using Nodes and Elements |
4-1 Generate the Arch Ribs 4-2 Generate the Hangers 4-3 Generate the Main Girder and Duplicate the Arch Frame 4-4 Generate the Cross Beams 4-5 Generate the Bracings |
| 5. Enter Structure Boundary Conditions |
5-1 Input the Boundary Conditions at the Nodes 5-2 Boundary Conditions for Beam End Connections 5-3 Generate the Cross Beam Group |
| 6. Enter Moving Traffic Loads and Static Loads |
6-1 Define Load Cases 6-2 Define Static Loads 6-3 Moving Load Code 6-4 Enter the Lane Configuration 6-5 Define Moving Traffic Loads 6-6 Define Moving Load Cases 6-7 Define the Method of Analysis for the Moving Vehicle Load |
| 7. Perform Structural Analysis |
|
| 8. Verify and Interpret Analysis Results |
8-1 Load Combinations 8-2 Verify Deformed Shape 8-3 Shear Force and Bending Moment Diagrams 8-4 View Influence Lines Results |
1. Summary
1-1 Model Shape and Summary
This tutorial explains the modeling and analysis of a single-span arch bridge subjected to moving vehicle loads. The model shape of the arch bridge for this tutorial is as follows
Final Arch Bridge Model
The summary of the structure is as follows:
| Bridge Type | Arch Bridge |
|---|---|
| Bridge Class | First Class |
| Span Length | 50 m |
| Design Traffic Lanes | 2 Lanes |
| Bridge Width | 14m |
1-2 Detailed Model View
The following list describes the structural plan layout:
-
-
- The spacing of cross beams is 5 m
- Stringers are placed longitudinally along the axis of the bridge.
- Main girders and arch ribs are placed 7 m from the centerline on both sides.
-
Framing Plan
| No | Boundary Conditions |
|---|---|
| B1 | Full Restraint in All Directions |
| B2 | Restrained Displacement in the Y and Z Directions |
| B3 | Restrained Displacement in the X and Z Directions |
| B4 | Restrained Displacement in the Z Directions |
Front View Elevation
1-3 Load Cases
For simplicity, only the following 3 load cases are considered:
| No | Load condition |
|---|---|
| Load Case 1 | 90 kN/m Dead Load (applied only on the main girders) |
| Load Case 2 | 6 kN/m Sidewalk Load (applied only on the main girders) |
| Load Case 3 | Vehicle Loads (HL93-TRK, HL93-TDM) |
2. File Opening and Preferences Setting
Open a new file to model the bridge and save the file as “Arch BD3701” .
1. Click New Project
2. Click Save
3. Enter file name as 'Arch AASHTO LRFD'
4. Click on button
Save File
2-1 Unit System Configuration
In the modeling for this tutorial, we will use the unit system of meters (Length) and kilonewton (Force)
Main menu >[Tools] Tab > [Setting] Group > Unit System
1. Confirm 'm', in the Length, 'kN (ton)' in the Force (Mass)
2. Click on button
Unit system configuration
3. Enter Material and Section Properties
3-1 Define Material Properties
define the material for the members
| Material ID | Type | DB | |
|---|---|---|---|
| 1 | Steel | A36 | cross beam, bracing |
| 2 | Steel | A572-50 | main girder, arch rib, hanger |
Main menu > [Properties] Tab > [Material] Group > Material Properties
1. Click on button
2. Select “Steel” in the Type selection field
3. Select “ASTM(S)” in the Standard selection field of Steel.
4. Select “A36” in the DB selection field.
5. Click on button
6. Select “Steel” in the Type selection field.
7. Select “ASTM(S)” in the Standard selection field of Steel.
8. Select “A572-50” in the DB selection field.
9. Click on button
Material Properties Dialog Box
3-2 Define Section Properties
Input the cross-section of the members.
| Section ID | Name | Type | section type | section size |
|---|---|---|---|---|
| 1 | Main Girder | User | Box | 2.1 × 0.6 × 0.01/0.01 |
| 2 | cross Beam | User | I-Section | 1.54 × 0.5 × 0.014/0.027 |
| 3 | Arch Rib | User | Box | 0.6 × 0.6 × 0.016/0.014 |
| 4 | Hanger | User | I-Section | 0.6 × 0.4 × 0.012/0.016 |
| 5 | Truss Bracing and Struts | User | Box | 0.6 × 0.5 × 0.01/0.014 |
| 6 | Bracing & Stringer | DB | I-Section | W16x100 |
Main menu > [Properties] Tab > [Section] Group > Section Properties
1. Click on button
2. Confirm “1” in the Section ID field of the DB/User tab
3. Enter “Main Girder” in the Name field.
4. Select “Box” in the Section Shape selection field
5. Select “User” in User or DB.
6. Enter “2.1” in the H field
7. Enter “0.6” in the B field.
8. Enter “0.01” in the tw field.
9. Enter “0.01” in the tf1 field.
10. Click on button
11. Repeat steps 2 to 10 for Sections 2 to 5 (use I-section instead of Box section for sections 2 and 4)
12. Confirm “6” in the Section ID field.
13. Enter “Bracing & Stringer” in the Name field.
14. Select “I-Section” in the Section Shape selection field
15. Select “DB” in DB or User
16. Select “AISC” in the field to the right
17. Click the Sect. Name field and type “W16x100” or use "Scroll Bar" to select the type
18. Click on button
19. Click on button
Define section
Section Properties and Section Data Dialog Box
4. Structural Modeling using Nodes and Elements
4-1 Generate the Arch Ribs
Use Structure Wizard to generate the arch ribs
Main menu > [Structure] Tab > [Wizard] Group > Base Structures > Arch
1. Click Front View
2. Select “Parabola1” in the Type selection field of the Input & Edit tab
The arch shape (parabola/ellipse with equal/ equal-projected spacing) can be selected in the Type field of the Input & Edit tab. Considering the hangers at an equal spacing, select “Parabola1” to set the nodes on the arch rib at an equal spacing projected on a horizontal line.
3. Enter “10” in the Number of Segments field
4. Enter “50” in the L field
5. Enter “10” in the H field
6. Select “None” in the Boundary Condition selection field
7. Select “2 : A572-50” in the Material selection field
8. Select “3 : Arch Rib” in the Section selection field
9. . Enter “0, 0, 0” in the Insert Point field of the Insert tab
10. Click on button
Concept of Parabola1 format and Arch Wizard Dialog Box
4-2 Generate the Hangers
Use Extrude Elements to generate the hangers. Extend the nodes generated on the arch rib by projecting them perpendicularly downward
Main menu > [Node / Element] Tab > [Element] Group > Extrude
Extrude Elements generates geometrically 1-dimensional higher elements by following the moving path of the nodes or elements.
1. Display Node Numbers (Toggle on),
Auto Fitting
2. Input ‘2 to 10’ in the Select Nodes by Identifying
3. Select “Node->Line Elem.” in the Extrude Type selection field.
4. . Select “Beam” in Element Type of the Element Attribute selection field
5. Select “2 : A572-50” in the Material selection field
6. Select “4 : Hanger” in the Section selection field.
7. . Select “Project” in the Generation Type selection field.
8. Select “Project on a line” in the Projection Type selection field.
9. Click the P1 field of "Base Line definition". Once the background color turns to pale green, assign node 1 and then assign node 11 for P2 filed.
Base Line Definition requires 2 nodes of the line onto which it is projected.
10. Select “Normal” in the Direction selection field.
11. Click on button
Hanger Generation
Main menu > [Node / Element] Tab > [Element] Group > Change Element Parameters
1. Click Select Recent Entities
2. Select “Element Local Axis” in the Parameter Type selection field.
3. Select “Assign” in the Mode selection field.
4. Select “Beta Angle” in the Mode selection field.
The hanger web direction is modified to be perpendicular to the bridge longitudinal axis.
5. Enter “90” in the Beta Angle field.
6. Click on button
Modification of the Beta Angle for Hanger
4-3 Generate the Main Girder and Duplicate the Arch Frame
Create the main girder by connecting both ends of the arch. Duplicate the completed part of the arch frame including the main girder at the opposite side.
Main menu > [Node / Element] Tab > [Element] Group > Create Elements
1. Select “General beam/Tapered beam” in the Element Type selection field.
2. Select “2 : A572-50” in the Material selection field.
3. Select “1 : Main girder” in the Section selection field.
4. Select “0” in the Beta Angle field of Orientation.
5. Check on Node and Elem of the Intersect selection field.
6. Click the Nodal Connectivity field
7. Once the background color turns to pale green, assign nodes 1 to 11.
Create elements by specifying the node numbers in the correct order. Follow the order of the numbers in the table, specifying the front number first and the back number later. (For example, 1 -> 11)
Creation of main girder
Main menu > [Node / Element] Tab > [Element] Group > Translate
1. ISO View,
Activate all
2. Click Select All
3. Select “Copy” in the Mode selection field.
4. . Select “Equal Distance” in the Translation selection field
5. Enter “0, 14, 0” in the dx, dy, dz field.
6. Enter “1” in the Number of Times field
7. Click on button
Duplicate arch frame
4-4 Generate the Cross Beams
Use Extrude Elements to create the cross beams by extending the nodes on one of the main girders to the nodes on the opposite main girder.
Main menu > [Node / Elements] Tab > [Element] Group > Extrude
1. Input ‘1, 11 to 20’ in the Select Nodes by Identifying
Select the main girder before copying. Since the arch rib was created first and then the hanger was created, the node numbers may not be consecutive.
2. Select “Node->Line Element.” in the Extrude Type selection field
3. Select “Beam” in the Element Type selection field.
4. Select “1 : A36” in the Material selection field.
5. Select “2 : Cross beam” in the Section selection field.
6. Select “Project” in the Generation Type selection field.
7. Select “Project on a line” in the Projection Type selection field.
8. Click the P1 in the Base Line Definition field.
9. Once the background color turns to pale green, assign the nodes 21 and 31 consecutively.
10. Select “Normal” in the Direction selection field.
The Direction represents the Direction of Projection.
11. Click on button
Creation of Cross Beams
4-5 Generate the Bracings
Activate only the newly created cross beams. Use Element Snap in conjunction with Create Elements to create the stringers.
Main menu > [Node / Element] Tab > [Element] Group > Create Elements
1. Select Recent Entities
2. Activate,
Top View
3. Click Display Elements Numbers (Toggle on),
Display Node Numbers (Toggle off)
4. Select “General beam/Tapered beam” in the Element Type field.
5. Select “1 : A36” in the Material field.
6. Select “6 : Bracing & Stringer” in the Section field.
7. Enter “0” in the Beta Angle field of Orientation.
8. Confirm that the location of Element Snap in Status Bar is 1/2 (bottom right corner)
9. Check on ‘Node, Elem’ in the Intersect field
10. Click the Nodal Connectivity field
11. Once the background color turns to pale green, assign the middle of elements 59 and 60 consecutively.
12. Click Display Elements Numbers (Toggle off),
Display Node Numbers (Toggle on)
13. Click the Nodal Connectivity field. Once the background color turns to pale green, connect nodes 1 to 43 and nodes 43 to 21 to create two elements.
Completed Stringers
Main menu > [Node / Element] Tab> [Element] Group > Translate Elements
1. Click Select Single
2. Select the two braces generated in the previous step 13
3. Select “Copy” in the Mode selection field.
4. Select “Equal Distance” in the Translation selection field.
5. Enter “5, 0, 0” in the dx, dy, dz field.
6. Enter “4” in the Number of Times field
7. Click on button
Floor Plan
Main menu > [Node / Element] Tab > [Element] Group > Mirror Elements
8. Click Select Previous
9. Click Select Recent Entities to select all the diagonal bracings
To select all diagonal bracings, combine the elements selected in the previous step with the newly created elements.
10. Click "Yes" in the CVLw dialog box for the question "Append to Current Selection?"
11. Select “Copy” in the Mode selection field.
12. Select "y-z plane" in Reflection field
13. Click the x field. Once the background color turns to pale green, assign node 16 or enter “25”
14. Click on button
Completed Floor Plane
Create the bracings on the arch ribs located symmetrically on each side of the mid span.
Main menu > [View] Tab > [Activities] Group > Inverse Active
Inverse Active function deactivates the nodes and elements displayed in the current window and activates the formerly inactivated nodes and elements.
Main menu > [Node / Element] Tab > [Element] Group > Create Elements
1. ISO View
2. Select ‘General beam / Tapered beam’ in the Element Type
3. Select “1 : A36” in the Material selection field.
4. Select “5 : Strut” in the Section selection field.
5. Enter “0” in the Beta Angle field of Orientation.
6. Check on "Node" and "Elem"
7. Click the Nodal Connectivity field.
8. Click nodes ‘4, 24’ in order
9. Click nodes ‘5, 25’ in order
10. Click nodes ‘6, 26’ in order
11. Click nodes ‘7, 27’ in order
12. Click nodes ‘8, 28’ in order
Completed Struts
Main menu > [Node / Element] Tab > [Element] Group > Create Elements
1. Click Select Single
2. Select the 5 struts generated in the previous step.
3. Click on Activate,
Top View
When an undesirable location is selected during the data entry of elements, click the Esc key. Alternatively, right-click the mouse and select Cancel at the bottom of the Context Menu to cancel the entry.
4. Display Elements Numbers (Toggle on),
Display Node Numbers (Toggle off)
5. Select “General beam/Tapered beam” in Element Type.
6. Select “1 : A36” in the Material selection field
7. Select “6 : Bracing & Stringer” in the Section selection field
8. Enter “0” in the Beta Angle field of Orientation.
9. Check in Elem of the Intersect selection field
10. Click the Nodal Connectivity field.
11. Once the background color turns to pale green, connect successively the centers of elements 111 to 115 to create the bracings.
12. Display Elements Numbers (Toggle off),
Display Node Numbers (Toggle on)
13. Click the Nodal Connectivity field. Once the background color turns to pale green, connect separately nodes 4 and 53, 24 and 53, 5 and 54, 25 and 54, 54 and 7, 54 and 27, 55 and 8, and 55 and 28
To create the bracings in the central portion of the arches, selectively activate the elements that are connected to the elements being generated.
Completed Arch Bracings
5. Enter Structure Boundary Conditions
5-1 Input the Boundary Conditions at the Nodes
Enter Structure Boundary Conditions
Main menu > [Boundary] Tab> [Supports] Group > Define Supports
1. Click on Activate All,
ISO View
2. Select “Add/Replace” in the Options selection field.
3. Click Select Single
4. Check on ‘D-ALL’ in the Support Type (Local Direction)
5. Click joint ‘1’
6. Click on button
7. Check on ‘Dy’, ‘Dz’ in the Support Type (Local Direction)
8. Click joint ‘11’
9. Click on button
10. Check on ‘Dx’, ‘Dz’ in the Support Type (Local Direction)
11. Click Joint ‘21’
12. Click on button
13. Check on ‘Dz’ in the Support Type (Local Direction)
14. Click Joint ‘31’
15. Click on button
Enter Structure Boundary Conditions
5-2 Boundary Conditions for Beam End Connections
Input boundary conditions for the ends of the beam using the "Beam End Release" feature
- For the ends of the hangers: Specify pinned connection conditions along the z-axis of the element coordinate system.
- For the ends of the bracing member: Specify pinned connection conditions along the y-axis and z-axis of the element coordinate system.
- For the ends of the horizontal beam connected to the main structure: Specify pinned connection conditions along the y-axis and z-axis of the element coordinate system.
Main menu > [Boundary] Tab > [Release / Offset] Group > Beam End Release
1. Click on Select Elements by Identifying
2. Select ‘Section’ in the Select Type
3. Select ‘4 : Hanger’ and Click on button
4. Click on button
5. Select ‘Add / Replace’ in the Options
6. Select ‘Relative’ in the General Types and Partial Fixity
7. Check on i-node ‘Mz’ and input ‘0’
8. Check on j-node ‘Mz’ and input ‘0’
9. Click on button
Inputting boundary conditions for the ends of the hanger member
Main menu > [Boundary] Tab > [Release / Offset] Group > Beam End Release
1. Click Select Elements by Identifying
2. In the Select Type dropdown menu of the Identify dialog box, select 'Section'
3. Select “6 : Bracing & Stringer” in the Section selection field
4. Click on button
5. Click on button
6. Click on button in the General Types and Partial Fixity
7. Click on button
8. Click Select Elements by Identifying
9. In the Select Type dropdown menu of the Identify dialog box, select 'Section'
10. Select “2 : Cross Beam” in the Section field.
11. Click on button
12. Click on button
13. Click Activate
14. Display Elements Numbers (Toggle on),
Display Node Numbers (Toggle off)
15. Click Select by Intersecting to select elements 59 to 69.
16. Click on button in the General Types and Partial Fixity
17. Click on button
18. Input ‘80 to 90’ in the Select Elements by Identifying
19. Click on button in the General Types and Partial Fixity
20. Click on button
Complete Beam End Release
5-3 Generate the Cross Beam Group
Generate the Cross Beam Group, which will be used to enter the moving loads.
To consider precise moving load distribution, automatically generate lane elements
1. Display Elements Numbers (Toggle off),
Active all,
ISO View
2. Click Select Identity-Elements
3. Select "Section" in the Select Type field
4. Select "2: Cross Beam" in the Section field
5. Click on button
6. Click on button in the Select Identity-Element dialog box
Tree menu > Group
7. Click on Active all,
Top View in the Icon Menu
8. Right-click the mouse in the Structure Group and then select New to enter “Cross Beam 1”.
9. From the Structure Group drag "Cross Beam 1" with the mouse and drop to the model window.
10. Click on Active all,
ISO View in the Icon Menu
Generate the Cross Beam Group
6. Enter Moving Traffic Loads and Static Loads
6-1 Define Load Cases
Define Static Load Case before specifying Static loads.
Main menu > [Load] Tab > [Create Load Cases] Group > Static Load Cases
1. Enter "Dead Load" in the Name field.
2. Select “Dead Load” in the Type selection field.
3. Click on button
4. Enter “Sidewalk Load” in the Name field.
5. Click on button
6. Click on button
Define load cases
6-2 Define Static Loads
Specify the static load cases. The dead and sidewalk loadings are assumed to be applied only on the main girders for simplicity.
Main menu > [Load] Tab > [Beam Load] Group > Element Beam Loads
1. Click Select Elements by Identifying
2. . Select “Section” in the Select Type field
3. Select “1 : Main Girder” in the Section selection field.
4. Click on button
5. Click on button
6. Select “Dead Load” in the Load Case Name selection field
7. Select “Add” in the Options selection field.
8. Select “Uniform Loads” in the Load Type selection field.
9. Select “Global Z” in the Direction selection field
10. Enter “0”, “1” and “-90” in the x1, x2 and w fields, respectively
11. Click on button
12. Click Select Previous
13. Select “Sidewalk Load” in the Load Case Name field
14. Enter “0”, “1” and “-6” in the x1, x2 and w fields, respectively.
15. Click on button
Input Static Loads
6-3 Moving Load Code
To perform moving load analysis, you need to set up the moving load code. In this tutorial, let's set the Moving Load Case to "AASHTO LRFD"
Main menu > [Load] Tab > [Load Type] Group > Moving Load
Main menu > [Load] Tab > [Moving Load Code] Group > Moving Load Code
1. ISO View,
Activate all
2. Select ‘AASHTO LRFD’ in the Moving Load Code
Moving load code
6-4 Enter the Lane Configuration
Define the traffic line lanes
Change the unit system to the English system (kips and ft)
Main menu > [Load] Tab > [Moving Load Analysis Data] Group > Traffic Line Lanes
1. ISO View,
Display Node Numbers (Toggle on)
2. Click on button
3. Enter “Lane 1” in the Lane Name field.
4. Enter “-11.5” in the Eccentricity field.
5. Enter "6.0" in the Wheel Spacing field.
6. Select “Cross Beam” in the Vehicle Load Distribution field
7. Select “Cross Beam 1” in the Cross Beam Group field.
8. Select "Both" in the Moving Direction field
9. Select 2 Points among the options of 2 Points, Picking and Element Number within Selection by, and then click the field below it. Once the background color turns to pale green, assign nodes 1 and 11.
10. Click on button
11. Click on button
12. Enter “Lane 2” in the Lane Name field.
13. Enter “-35” in the Eccentricity field
14. Enter "6.0" in the Wheel Spacing field.
15. Select “Cross Beam” in the Vehicle Load Distribution field
16. Select “Cross Beam 1” in the Cross Beam Group field.
17. Select "Both" in the Moving Direction field
18. Repeat step 9 for Lane 2 case
19. Click on button
20. Click on button
Traffic Line Lanes Dialog Box
6-5 Define Moving Traffic Loads
The method for defining the moving traffic loads, HL93-TRK and HL93-TDM is explained below.
Main menu > [Load] Tab > [Moving Load Analysis Data] Group > Vehicles
1. Click on button
2. Select ‘AASHTO LRFD Load’ in the Standard Name field
3. Select ‘HL-93 TRK’ in the Vehicle Load Name and Vehicle Load Type fields
4. Enter "33" in the Dynamic Load Allowance Field
5. Click on button
6. Select ‘HL-93 TDM" in the Vehicle Load Name and Vehicle Load Type fields
7. Enter "33" in the Dynamic Load Allowance Field
8. Click on button
9. Click on button
Input Vehicle Loads
6-6 Define Moving Load Cases
Using the Moving Load Case feature, define the lane on which the vehicle load will be applied, along with the maximum and minimum number of lanes that can be simultaneously loaded. Specify the specific vehicle load conditions as well.
Main menu > [Load] Tab > [Moving Load Analysis Data] Group > Moving Load Cases
1. Click on button
2. Enter “MVL” in the Load Case Name field of the Moving Load Case dialog box
3. Keep default values of "Scale Factor" in Multiple Presence Factor
4. Select ‘Independent’ in the Loading Effect from Sub-Load Cases
By selecting "Independent" in the Loading Effect, when specifying multiple Sub-Load Cases, the maximum and minimum values from the results of each Sub-Load Case are calculated and presented. Therefore, in this example, it will be easy to check the envelope results of the results caused by the vehicles.
5. Click on button in the Sub-Load Cases
6. Select ‘VL : HL93-TDM’ in the Vehicle Class field from Load Case Data
7. Enter “1” in the Scale Factor field.
8. Enter “1” in the Min. Number of Loaded Lanes field
9. Enter “2” in the Max. Number of Loaded Lanes field.
10. Select “Lane 1” and “Lane 2” in List of Lanes of Assignment Lanes
11. Click to move and Click on
button in the Sub-Load Cases field
Use the Moving Load Cases Function to define the vehicle loading conditions, i.e. which vehicle loads are applied on which traffic lanes. Also define the maximum and minimum numbers of traffic lanes that can be loaded with vehicle loads simultaneously
12. Click on button in the Sub-Load Cases field
13. Select ‘VL : HL93-TRK’ in the Vehicle Class field from Load Case Data
14. Repeat steps "7 to 11"
15. Click on button in the Define Moving Load Case dialog box
16. Click on button in the Moving Load Cases dialog box
Define the vehicle load group
6-7 Define the Method of Analysis for the Moving Vehicle Load
Main menu > [Analysis] Tab > [Analysis Control] Group > Moving Load
1. Select “Exact” in the Analysis Method field.
To specify the method for deriving various design values from the analyzed influence lines, you can use the Moving Load Analysis Control feature. In the Analysis Method selection, 'Exact' sequentially moves the concentrated wheel load along the lanes, 'Pivot' selects the axle with the most significant influence from the concentrated wheel loads and moves it, while 'Quick' only applies the concentrated wheel load at positions where the maximum/minimum influence line values occur.
2. Select "All Points" in the Analysis Method field
3. Enter “5” for the field of Numer/Line Element within the Influence Generating Points.
Use Moving Load Analysis Control to input the number of points on each line element where influence lines should be generated. For example, if “5” is inputted in Influence Generating Point No./Line Element field, it means that the concentrated axle load is applied successively at 5 equally spaced points on each line element, along the direction of the traffic lane. (Also refer to the Structural Analysis functions in the Online Manual for details).
4. Select “Normal” in Frame in the Analysis Results field.
5. Select “All” in Reactions, Displacements and Forces/Moments within Calculation Filters.
Calculation Filter in Moving Load Analysis Control Data groups only the desired part of the results for review. The grouping reduces the computation time and the size of Results file for large structures.
6. Click on button
7. Click Display Node Numbers (Toggle off)
Moving Load Analysis Control Dialog Box
7. Perform Structural Analysis
Perform the structural analysis of the structure attributed to boundary conditions and load cases.
Main menu > [Analysis] Tab > [Perform] Group > Perform Analysis
8. Verify and Interpret Analysis Results
8-1 Load Combinations
We will now examine the Linear Load Combination method of the 3 load cases (dead load, sidewalk load and moving load) for which structural analyses have been completed.
In this example, we specify only one load combination as noted below, and check its results. The load combination case has been arbitrarily chosen and, as such, it may be irrelevant for any practical design application.
Load Combinations
- Load Combinations 1 (LCB 1): 1.0 (Dead Load + Sidewalk Load + MVL)
Main menu > [Results] Tab > [Combination] Group > Load Combination
1. Select General Tab
2. Enter “LCB1” in the Name field from Load Combination List.
Selecting Active under Active in the Load Combinations dialog box prompts the load combination used by the design function of the program. (Refer to the Online Manual for details)
3. Select "Add" in the Type selection field
4. Select ‘Dead Load (ST)’ in the Load Case from Load Cases and Factors and enter "1.0" in Factor field
5. Select ‘Sidewalk Load (ST)’ in the Load Case from Load Cases and Factors and enter "1.0" in Factor field
6. Select ‘MLV (MV)’ in the Load Case from Load Cases and Factors and enter "1.0" in Factor field
7. Click on button
Load Combinations Dialog Box
8-2 Verify Deformed Shape
Use the following procedure to check the deformed shape
Main menu > [Results] Tab > [Results] Group > Deformations > Deformed Shape
1. Select ‘CBmin : LCB 1’ in the Load Cases / Combinations
2. Select ‘DXYZ’ in the Components
3. Check “Undeformed” and “Legend” in the Type of Display selection field.
4. Click in the Deform from Type of Display
5. Select ‘Real Deform’ in the Deformation
6. Check ‘Apply upon OK’
7. Click on button
8. Click on button
9. Click Hidden (Toggle on)
Deformed Shape
8-3 Shear Force and Bending Moment Diagrams
The method for reviewing the shear force and bending moment diagrams are quite similar. Therefore, only the method for displaying the bending moment diagram is reviewed in this case. This method is not intended to capture the bending moment diagram of the entire structure. The purpose is to display only the results related to a specific part of the structure. For instance, the following steps illustrate the procedure to display the bending moment diagram in the X-Z plane
Quite often, analysis results for the structural behavior of specific parts are required in practice. Use the Select Plane to separately extract the results at the desired planar section
1. Click Front View
2. Click Hidden (Toggle off)
3. Click Initial View in the Icon Menu
4. Click Select by Plane
5. Select “XZ Plane” in the Plane tab.
6. Click in the Y Position field and select a point with the mouse, which defines the desired X-Z plane (the color of the selected plane changes). For convenience to follow the given instruction, choose y = 0.
7. Click on button
8. Click Activate and
Front View
Main menu > [Results] Tab > [Results] Group > Forces > Beam Diagrams
1. Select “MVall: MVL” in Load Cases/Combinations selection field
MVmin: The minimum member force resulting from the vehicle load applied to the structure.
MVmax: The maximum member force resulting from the vehicle load applied to the structure.
2. Select “My” in the Components selection field.
3. Select “5 Points” and “Line Fill” in Display Options selection field
4. Enter “1.0” in the Scale field.
5. Check “Contour” and “Legend” in the Type of Display selection field
6. Click on button
BMD check (XZ Plane)
8-4 View Influence Lines Results
First, we will examine the influence lines for a support reaction. it is the results for support B1 (node 1).
Main menu > [Results] Tab> [Moving Load] Group > Influ. Lines > Reaction Forces / Moments
1. Click Hidden (Toggle off),
Front View
2. Select “Lane 1” in the Line/Surface Lanes field.
3. Enter “1” in the Key Node field.
4. Enter “1.0” in the Scale Factor field.
5. Select “FZ” in the Components field.
6. Check “Legend” in the Type of Display field.
7. Click on button
Reaction Influence Line
Result of the deflection influence line.
Main menu > [Results] Tab > [Moving Load] Group > Influ. Lines > Displacements
1. Confirm “Lane 1” in the Line/Surface Lanes selection field.
2. Enter “15” in the Key Node field.
3. Enter “2.0” in the Scale Factor field.
4. Select “DZ” in the Components selection field
5. Check “Legend” in the Type of Display selection field.
6. Click on button
Deflection Influence Line
Result of the moment influence line.
Main menu > [Results] Tab > [Moving Load] Group > Influ. Lines > Beam Forces / Moments
1. Confirm “Lane 1” in the Line/Surface Lanes selection field.
2. Enter “23” in the Key Element field
3. Enter “2.0” in the Scale Factor field
4. Select “i” in the Parts selection field
5. Select “My” in the Components selection field
6. Check “Legend” in the Type of Display selection field.
7. Click on button
Moment Influence Line
Use Moving Load Tracer to check the reactions on the structure resulting from the movement of vehicular traffic.
Moving Load Tracer can be applied to the results obtained from the structural analysis related to Moving Vehicle Load. It displays the results similar to an influence line or influence surface diagram by tracking the location of the vehicle loading.
Main menu > [Result] Tab> [Moving Load] Group > Moving Tracer > Reactions
1. Click ISO View,
Initial View.
2. Click Select by Plane
3. Select “XY Plane” in the Plane tab, click in the Z Position field, and select node 1 with the mouse.
4. Click
5. Click Activate
6. Select “MVmax: MVL” in the Moving Load Cases selection field.
Moving Load Tracer generates a particular loading condition, which produces specific results due to moving vehicle load. The traced moving load condition is expressed in terms of an influence line or surface.
7. Input ‘1’ in the Key Node
8. Input ‘1.0’ in the Scale Factor
9. Select ‘FZ’ in the Components
10. Select ‘Contour’, ‘Legend’, 'Applied Loads' in the Type of Display
11. Click on button
Checking the loading points of a Vehicle using Moving Load Trace
Use the Moving Load Tracer feature to determine the position of the vehicle load that induces the moment at the i-th span of element 28.
Main menu > [Results] Tab > [Moving Load] Group > Moving Tracer > Beam Forces / Moments
1. ISO View,
Active all
2. Select ‘MVmax: MVL’ in the Moving Load Cases selection field
3. Input ‘28’ in the Key Element
4. Input ‘1.0’ in the Scale Factor
5. Select ‘i’ in the Parts
6. Select ‘My’ in the Components
7. Select ‘Contour’, ‘Legend’, ‘Applied Loads’ in the Type of Display
8. Click on button
Confirming the load position that induces moment using the Moving Tracer
Having determined the moving load location by the Moving Load Tracer, we will now examine the method of converting the live load into a static load. If we click the button of the Moving Load Tracer Function, the converted static load is saved in an MCT file. When we execute the MCT file using the MCT Command Shell in the model file already generated, the static load will be entered in the model. (For details on MCT Command Shell, refer to the Online Manual).
1. Click on button
2. Click on button in Moving Load Converted to Static Load dialog box.
3. Select File>Exit in the MIDAS/Text Editor.
4. In the Main menu, select Tools>MCT Command Shell>Open > File Name (MVmaxMVLMy28.mct) >open
5. Click in the MCT Command Shell dialog box.
6. Click "Yes" when prompted for “Analysis/design results will be deleted; Continue?” in the CVLw dialog box.
7. Click in the MCT Command Shell dialog box.
8. Select Load>Static Load Cases in the Main Menu.
9. Confirm that “MVmaxMVLMy28.mct” is generated under the Name column in the Static Load Cases dialog box.
10. Click in the Static Load Cases dialog box.
11. Click Analysis.
Substituting load using MCT Command Shell
Generated static load case using Moving Load Tracer
We can now check the bending moment due to the static load that was generated from the live load which caused the movement at the ith end of element 28.
Main menu > [Results] Tab > [Results] Group > Forces > Beam Diagrams
1. Select "ST:MVmaxMVLMy28” in Load Cases/Combinations selection field
2. Select “My” in the Components selection field.
3. Select “5 Points” and “Line Fill” in Display Options selection field
4. Enter “1.0” in the Scale field.
5. Check “Contour” and “Legend” in the Type of Display selection field
6. Click on button
My beam diagrams for the live load converted into static load