[CIVIL NX] Construction Stage Analysis of an I-Girder Bridge Using Composite Section

Download the following files

Steel I-Girder Composite Bridge.rar

0. Contents

1. Overview

For members composed of two or more materials, structural analysis must be performed considering the composite effect. Moreover, composite sections containing concrete when used, creep and drying shrinkage must be considered.
In this example, a bridge consisting of a composite cross-section of a concrete deck and a steel I-girder is constructed. Model using the Composite Section Wizard and construction stage method and check the results.
The type and span configuration of the bridge used in this example are as follows.

Interpretation model

MIDAS CIVIL NX provides the Composite Section for Construction Stage command for performing the construction stage analysis of a composite section. Through this example, we will learn how to perform structural analysis including the concepts of construction stages and composite sections.

The procedure for performing construction stage analysis of composite cross-section bridges is as follows.

1-1 Cross Section

[Unit: mm]

Section view

 In this example, the same cross-section is used for all girders and cross-beams to simplify the model.

1-2 Materials Used

1-3 Load

1-4 Composition of Construction Stage 

• Define load cases and load groups

Construction sequence for the deck and each part of the deck section

Now that the slab has an inflection point at 0.2L from the interior support when casting new concrete upon old concrete, make it happen at the inflection point where no stress occurs.

• Define boundary condition group

• Define construction stages

• SGroup represents a Structure Group including all members (girders, cross beams).
• One element group is enough since the geometry of the structure does not vary with construction stages.
• Using the Composite Section for Construction Stage command, define a composite/non-composite section in accordance with the construction sequence for the deck.
• Assume that it takes 25 days to manufacture formwork and concrete slab obtains the initial strength at 5 days. Accordingly, it would take 30 days to finish the construction.
• The self-weight of the slab to be entered into Element Beam Loads will be activated at 25 days when formwork will have been completed.

Slab weight and additional dead loads loaded at each construction stage

2. Setting up the Work Environment and Defining Cross-Sections and Materials

New file to model plate girder bridges ( Open New Project ) and save it with the name ‘I-Girder Composite’ (  Save).

Main menu > File >  New Project

Main menu > File >  Save

1. Enter ‘I-Girder Composite’ in the file name and Click the button

Save file

2-1 Setting up the Work Environment 

 Set the unit system for modeling plate girder bridges.

Main menu >[Project] Tab > [Setting] Group >  Unit System

1. In the Length checkbox, select ‘m’, in the Force (Mass) checkbox, Select ‘kN (ton)’

2. Click the  button

Unit system settings

2-2 Material Definition

 Define the materials of girders, crossbeams, and floor plates using the built-in DB in MIDAS CIVIL NX.

Main menu > [Properties] Tab > [Material Properties] Group >  Material Properties

1. Click the  button

2. Check ‘1’ in the Material ID field of General.

3. Select ‘Steel’ in the Type of Design selection box.

4. Select ‘ASTM(S)’ in the Standard selection box of Steel.

5. Select ‘A53’ in the DB selection box.

6. Click the  button

7. Check ‘2’ in the Material ID field of General.

8. Enter ‘A36’ in the DB selection box.

9. Click the  button

10. Check ‘3’ in the Material ID field of General.

11. Select ‘Concrete’ in the Type of Design selection box.

12. Select ‘ASTM (RC)’ in the Standard selection box of Steel.

13. Select ‘C6000’ in the DB selection box.

15. Click the  button

Material definition

2-3 Section Definition

With the construction sequence considered, girders will have different section names from construction stage to stage. For this particular tutorial, assume that all girder sections are the same; in such case, girders will have identical section properties but different section names (i.e., Sect 1, Sect 2, Sect 3 and Sect 4). To create the cross beams, use User type section.

[Unit: mm]

Section layout

• Section Table

Main menu > [Properties] Tab > [Section Properties] Group >  Section Properties

1. Click the  button

2. Check ‘1’ in the Section ID input field.

3. Enter ‘Sect1’ in the Name input field.

4. Select ‘Steel-I (Type1)’ in the Section Type selection box.

5. Input Slab’s Bc: ‘6.07’, tc: ‘0.25’, Hh: ‘0.028’

6. Input Girder’s Hw: ‘3.2’, B1: ‘0.8’, tf1: ‘0.032’

                          tw : ‘0.02’, B2 : ‘0.9’, tf2 : ‘0.034’

7.Click the  button

8. Check ‘ASTM (RC)’ in the DB selection box of Concrete Material.

9. Select ‘C6000’ in the Name selection box.

10. Select ‘ASTM (S)’ in the DB selection box of Steel Material.

11. Select ‘A53’ in the Name selection box.

12. Click the  button

13. Enter ‘0’ in the Ds / Dc field.

14. Select offset as 'Center-Center'.

15. Click the  button

16. Create 'Sect2' and 'Sect3' in the same way as above.

Section definition

Main menu > [Properties] Tab > [Section Properties] Group >  Section Properties

1. Select the DB / User tab

2. Check ‘4’ in the Section ID input field.

3. Enter ‘CBeam’ in the Name input field.

4. Select ‘I-Section’ in the Section Type selection box.

5. Select 'User'

6. Input H: ‘0.84’, B1: ‘0.4’, tw: ‘0.02’, tf1: ‘0.02’

7. Click the  button

8. Click the  button

Section Definition

2-4 Define Time-Dependent Material Properties

Time dependent material properties will be defined so as to consider variations in concrete strength led by variations in the modulus of elasticity of concrete, creep and drying shrinkage developing with time. Time dependent material properties are determined from the CEB-FIP Code. A slab thickness of 25 cm will be used for computing Notational size of member.                                

Main menu > [Properties] tab > [Material Properties] group > Time Dependent >  Creep / Shrinkage

1. Click the  button

2. Enter ‘Mat-1’ in the Name input field.

3. Select ‘CEB-FIP (1990)’in the Code selection box.

4. Enter ‘20000’ the Characteristic Compressive Strength of Concrete at the age of 28 days in the field.

5. Enter ’70’ in the Relative Humidity of ambient environment (40~99) field.

6. Enter notational size of member ‘0.245’

7. In Type of cement, select ‘Normal or rapid hardening cement (N, R)’ 

8. Enter ‘3’ in the Age of concrete at the beginning of shrinkage field.

9. Click the  button

10. Click the  button

Time-dependent member material definition

Placed concrete is hardened and gains strength with age. To consider this, a function of compressive strength of concrete is given here by the CEB-FIP Code. The data entered in the Time Dependent Material (Creep / Shrinkage) dialog box is adopted in the Time Dependent Material (Comp. Strength) dialog box.    

Main menu > [Properties] tab > [Material Properties] group > Time Dependent >  Comp. Strength

1. Enter ‘Mat-1’ in the Name input field.

2. Select ‘Code’ in Type

3. Select ‘CEB-FIP (1990)’ in the Code selection box of Development of Strength.

4. In the Mean Compressive Strength of Concrete at the age of 28 Days (fck+deltaf) field, Enter ‘28000’

5. Select ‘N,R: 0.25’ in the Cement Type (s) selection box.

6. Click the  button

7. Click the button &  button

Time-dependent member material definition

In MIDAS CIVIL NX, time dependent material is defined separately from the conventional material, and time dependent material properties can be assigned to a conventional material selected.

In this tutorial, time dependent material properties will be assigned to the concrete slab (Grade C6000).  

Main menu > [Properties] tab > [Material Properties] group >  Material Link

1. In the Creep/Shrinkage checkbox of Time Dependent Material Type Select ‘Mat-1’

2. In the Comp. Strength checkbox of Time Dependent Material Type Select, ‘Mat-1’ select

3. Select ‘3:Grade C6000’ in the Materials selection box of Select Material for Assign.

4. Click the  button

5. Click the  button

Connect regular materials and time-dependent materials

3. Bridge Modeling

After defining the groups required for composing construction stages, construct a bridge model for each construction stage. This tutorial explains a technique for assigning construction stages when using Composite Section.

3-1 Group Definition

Refer to the following table to define each group necessary to configure each construction stage. 

Group in Tree Menu

1. Right-click on Structure Group and click ‘New’, Enter ‘SGroup’

2. Right-click in the Boundary Group and click ‘New’, Enter ‘BGroup’

3. Enter ‘E_Width’ 1~3 in the same way.

4. Right-click on Load Group and click ‘New’, Enter ‘DL (BC) 1’

5. In the same way, enter ‘DL (BC)’ 2~4 , ‘DL (AC)’

Group Definition

3-2 Bridge Modeling

Refer to figure below to generate girders.

Construction sequence for deck and each part of the deck section

In this tutorial, cross beams are to be placed at a spacing of 5m and slab concrete is to be poured in accordance with the sequence as depicted in above figure. To consider the effective width of girders, girder elements will be generated to have the following lengths.    

Main menu > [Node / Element] Tab > [General] Group > Create >  Create Element

1.  Click Top View

2.  Click Auto Fitting

3. Enter ‘0, 0, 0’ in the Coordinates (x,y,z) field.

4. Enter ‘1’ in the Number of Times field.

5. Enter ‘0, 6.15, 0’ in the Distances (dx, dy, dz) field.

6. Click the  button

Main menu > [Node / Element] Tab > [Element Detail] Group > Edit Elements >  Extrude

1. Click  Select All

2. In the Extrude Type selection list, select ‘Node -> Line Element’

3. Select ‘Beam’ in the Element Type selection box.

4. Select ‘1 : A53’ in the Material selection box.

5. Select ‘1 : Sect 1’ in the Section selection box.

6. Select ‘Translate’ in the Generation Type selection box.

7. Select ‘Unequal Distance’ in the Translation selection box.

8. Select ‘x’ in the Axis checkbox

9. In the Distances field enter ‘7@5, 1, 4, 3@5, 1, 4, 5@5, 4, 1, 3@5, 4, 1, 7@5’

10. Click the  button

Girder modeling

To assign the girder elements of CS3 to Sect 2, and the girder elements of CS4 to Sect 3, use the Drag & Drop feature. 

In Works Tree

1.  Click Select by Window to select all girders in CS3 section (element : 17 to 40)

2. Works > Properties > Section > Mouse over ’2 : Sect2’ Designate with the left button and drag and drop to Model View (Drag & Drop function)

3.  Click Select by Window to select all girders in element CS4 section (element : 41 to 66)

4. Works > Properties > Section > Mouse over ’3 : Sect3’ Designate with the left button and drag and drop to Model View (Drag & Drop function)

Different section assigned to different parts of girder

 Enter the crossbeam.

Main menu > [Node / Element] Tab > [General] Group > Translate > Translate Element

1. Check ‘General beam / Tapered beam’ in the Element Type selection box.

2. Select ‘2 : A36’ in the Material selection box.

3. Select ‘4 : CBeam’ in the Section selection box.

4. Intersect’s ‘Node’ check on

5. Switch the Nodal Connectivity input box to the mouse editor function (click with the mouse to change the background to green) and then Specify 1 and 2 in each order

Main menu > [Node / Element] tab > [Elements] Group >  Translate Elements

1. Click  Select Recent Entities

2. Check ‘Copy’ in the Mode selection box.

3. Check ‘Equal Distance’ in the Translation selection box.

4. Enter ‘5, 0, 0’ in the dx, dy, dz input fields.

5. Enter ‘29’ in the Number of Times field.

6. Check on Intersect's 'Node' and 'Elem'

7. Click the  button

Input cross beam

4. Enter Boundary Conditions

4-1 Enter Support Condition

Since all boundary conditions of the structure are simultaneously activated at CS1, designate BGroup as a boundary group in which all boundary conditions of the bridge will be included.   

Main menu > [Boundary] Tab> [Supports] Group >  Define Supports

1. Select ‘BGroup’ in the Boundary Group Name input field.

2. Check ‘Add’ in the Options selection box.

3. Click  Select Single to select node 21

4. ‘D-ALL’ check on

5. Click the  button

6. Click  Select Single to select nodes 1, 47, 67

7. ‘Dy, Dz’ check on

8. Click the  button

9. Click  Select Single to select nodes 2, 48, 68

10. ‘Dz’ check on

11. Click the  button

12. Click  Select Single to select node 22

13. ‘Dx, Dz’ check on

Enter boundary conditions

4-2 Enter Effective Width

Enter the Scale Factors to be applied to the moment of inertia of girder sections to account for effective width. In MIDAS CIVIL NX, the specified Effective Width Scale Factor will be used for calculating member stresses.    

If you want to calculate stresses in a section to account for effective flange width, use the Effective Width Scale Factor command with the ratio of Iyy of the effective section to Iyy of the gross section, entered in the Scale Factor for Iy field.                      

Main menu > [View] Tab > [Display] Group > Display >  Display

1. In the Boundary tab, Check On in the Support item.

Main menu > [Properties] Tab > [Section Properties] Group >   Effective Width

1. Select ‘E_Width1’ in the Boundary Group Name input field.

2.  Enter 1to16 in the Select Elements by Identifying field.

3. Enter ‘0.985’ in the Iy Scale Factor for Sbz input field.

4. Click the  button

5. Select ‘E_Width2’ in the Boundary Group Name input field.

6.  Entre 17to26 in the Select Elements by Identifying field. input

7. Enter ‘0.965’ in the Iy Scale Factor for Sbz field.

8. Click the  button

9. Select ‘E_Width2’ in the Boundary Group Name input field.

10.  Enter 27to40 in the Select Elements by Identifying field

11. Enter ‘0.992’ in the Iy Scale Factor for Sbz input field.

12. Click the  button

13. Select ‘E_Width3’ in the Boundary Group Name input field.

14.  Enter 41to50 in the Select Elements by Identifying field

15. Enter ‘0.965’ in the Iy Scale Factor for Sbz field.

16. Click the  button

17. Select ‘E_Width3’ in the Boundary Group Name input field.

18.  Enter 51to66 in the Select Elements by Identifying field

19. Enter ‘0.985’ in the Iy Scale Factor for Sbz field.

20. Click the  button

Enter the second-moment of inertia ratio according to the effective width

5. Loading Data

For this tutorial apply the pre- and post-composite loads by Element Beam Loads. Refer to the table below to apply the loads to each construction stage.             

To define the loads to be applied to each construction stage, select Construction Stage Load for the Load Type.     

 First, set the load cases.

Main menu > [Load] Tab > [Load type] Group > Static Loads > [Create Load Cases] Group > Static Load Cases

1. Enter ‘DL (BC)1’ in the Name input field of the Static Load Cases dialog box.

2. Select ‘Construction Stage Load’ in the Type selection box.

3. Click the  button

4. Refer to the picture below and repeat steps 2 to 5 to enter the remaining load cases

5. Click the  button

Enter load cases

5-1 Input Dead Load Before Composite Action

 Input the uniformly distributed load on the beam element using the Element Beam Loads function.

Main menu > [Load] Tab > [Load type] Group > Static Loads > [Static Loads] Group >  Self Weight

1. Check ‘DL (BC) 1’ in the Load Case Name selection box.

2. Enter ’-1’ in Z in the Self Weight Factor input field.

3. In the Operation selection box, click the  button

Main menu > [Load] Tab > [Load type] Group > Static Loads > [Static Loads] Group > Beam Loads > Element

1. Select ‘DL (BC)2’  in Load Case Name

2. Select ‘DL (BC)2’in Load Group Name.

3. Check ‘Uniform Loads’ in the Load Type selection box.

4. Select ‘Global Z’ in the Direction selection box.

5. After checking ‘x1: 0’, ‘x2: 1’ in Value, enter w. Enter ‘-38.96’

6.  Click Select Elements by Identifying

7. Select ‘Section’ in the Select Type box.

8. After selecting ‘1: Sect1’, Click the  button and Click the  button

9. Click the  button

10.  In the Select Elements by Identifying field Enter ‘2to16by2’

11. Select ‘Uniform Moments / Torsions’ in the Load Type selection box.

12. Select ‘Global X’ in the Direction selection box.

13. In Value, enter ‘1.49’ in the M field.

14. Click the  button

15.  In the Select Elements by Identifying field Enter ‘1to15by2’

16. In Value, enter ‘-1.49’ in the w field.

17. Click the  button

Input the total composite load of CS3 section (DL (BC)3) and CS4 section (DL (BC)4) in the same way as above.

Floor load in CS2 section

Floor load in CS3 and CS4 sections

5-2 Input Dead Load after Composite Action

 Input the uniformly distributed load on the beam element using the Element Beam Loads function.

Main menu > [Load] Tab > [Load type] Group > Static Loads > [Static Loads] Group > Beam Loads > Element

1. Check ‘DL (AC)’ in Load Case Name

2. Check ‘DL (AC)’ in Load Group Name

3. Check ‘Uniform Load’ in the Load Type selection box.

4. Select ‘Global Z’ in the Direction selection box.

5. After checking ‘x1: 0’, ‘x2: 1’ in Value, enter w. Enter ‘-18.69’

6.  Click Select Elements by Identifying

7. Select ‘Section’ in the Select Type box.

8. After selecting ‘1: Sect1, 2: Sect2, 3: Sect3’, click the  button, click the button

9. Click the  button

10.  In the Select Elements by Identifying field Enter ‘2to62by2’

11. Select ‘Uniform Moments / Torsions’ in the Load Type selection box.

12. Select ‘Global X’ in the Direction selection box.

13. In Value, enter ‘-19.69’ in the M field.

14. Click the  button

15.  In the Select Elements by Identifying field Enter ‘1to61by2’

16. In Value, enter ’19.69’ in the M field.

17. Click the  button

Enter additional dead load

6. Construction Stage Definition

6-1 Element Group Definition

 Enter elements and nodes into the element group to be used when defining the construction stage.

Go to Group in the Tree Menu

1. Click  Select All

2. In Structure Group, select ’SGroup’ with the left mouse button and then go to Model View. Drag and drop (Drag & Drop function)

Assign elements to Structure Group

6-2 Composition of Construction Stage

Refer to the following table to define each construction stage.

Main Menu > [Load] tab > [Load Type] Group > Construction Stage >  Define C.S

1. Click the  button

2. Enter ‘CS’ in the Stage Name input field.

3. Enter ‘1to4’ in the Suffix field.

4. Enter ‘30’ in the Duration field.

5. Enter ’25’ in the Day input field of Additional Steps, click the  button

6. Click the  button

Generate function at each construction stage

Click the Generate button to generate every construction stage at once, and then modify the data for the stage selected. Select CS1 and modify the data for the stage.

1. After clicking ‘CS1’, click the  button

2. Enter ‘0’ in the Day input field of Additional Steps, click the  button

3. Enter ‘5’ in the Duration field.

4. Select Group List ‘SGroup’ in the Element tab and enter Age in the field. Enter ‘0’

5. Click the  button

6. After selecting Group List ‘BGroup’ in the Boundary tab, Select ‘Deformed’

7. Click the  button

8. In the Load tab, select Group List ‘DL (BC)1, DL (BC)2’ and select Active Day as ‘First’.

9. Click the  button

10. Click the  button  

CS1 Construction Stage Modification

 Modify CS2, CS3.

1. After clicking ‘CS2’, click  button

2. After selecting Group List ‘E_Width1’ in the Boundary tab, Select ‘Deformed’

3. Click the  button

4. In the Load tab, select Group List ‘DL (BC)3’ and then on Active Day, Select ‘25’

5. Click the  button

6. Click the  button

7. After clicking ‘CS3’, click the  button

8. After selecting Group List ‘E_Width2’ in the Boundary tab, Select ‘Deformed’

9. Click the  button

10. After selecting Group List ‘DL (BC)4’ in the Load tab, Select ‘25’ on Active Day

11. Click the  button

12. Click the  button

CS2, CS3 construction stage modification

For CS4, to view the long-term behavior of the structure, enter 10,000 days as the number of construction days and modify the load group to activate the additional dead load.

1. After clicking ‘CS4’, click the  button

2. Enter ‘0’ in the Day input field of Additional Steps, click the  button

3. Enter ‘10000’ in the Duration field.

4. After selecting Group List ‘E_Width3’ in the Boundary tab, Select ‘Deformed’

5. Click the  button

6. After selecting Group List ‘DL (AC)’ in the Load tab, Select ‘First’ on Active Day

7. Click the  button

8. Click the  button

CS4 construction stage modification

Construction stage definition dialog box

6-3 Definition of Composite Section for Each Construction Stage

Specify the construction stage at which the girder or slab sections become activated. When the Section Type is set to “Composite”, the previously defined section properties can be used. Refer figure below to specify the Active Stage at which the girder or slab sections become activated. For this example, model assume that every girder is activated at CS1.       

Construction sequence for deck and each part of the deck section

Firstly assign the first part of the slab section (i.e., CS2).

By default, Composite Type is set to “Normal”. Note that Part 1 and Part 2 only are available for entering the construction stage. When “User” is selected from the Composite Type drop-down list, you can assign as many Parts as you desire, where you must use the outer dimensions or centroid pertaining to the post-composite section.  

Main Menu > [Load] tab > [Load Type] Group > Construction Stage >  Composite Section for C.S

1. Click the  button

2. Select ‘CS1’ in the Active Stage selection box.

3. Select ‘1 : Sect1’ in the Section selection box.

4. Select ‘Normal’ in the Composite Type selection box.

5. In the Part 1 input box, enter ‘Element’ in the Material Type and ‘Active Stage' in Composite Stage input box. Enter ‘0’ in the Age field.

6. In the Part 2 input field, enter ‘Material’ in the Material Type, ‘3:Grade C6000’ in the Material input field, ‘CS2' in the Composite Stage input field and enter ‘5’ in the Age input field.

7. Click the  button

Define a composite section for construction stage

 The following defines the second and third floor slab pour sections.

Main Menu > [Load] tab > [Load Type] Group > Construction Stage >  Composite Section for C.S

1. Click the  button

2. Select ‘CS1’ in the Active Stage selection box.

3. Select ‘2 : Sect2’ in the Section selection box.

4. Select ‘Normal’ in the Composite Type selection box.

5. In the Part 1 input box, enter ‘Element’ in the Material Type and  in the Composite Stage input box. Enter ‘0’ in the Age input field.

6. In the Part 2 input field, enter ‘Material’ in the Material Type, ‘3:Grade C6000’ in the Material input field, ‘CS3’ in the Composite Stage input field and enter ‘5’ in the Age input field

7. Click the  button

8. Select ‘3 : Sect3’ in the Section selection box.

9. Select ‘Normal’ in the Composite Type selection box.

10. In the Part 1 input box, enter ‘Element’ in the Material Type and ‘Active Stage’ in the Composite Stage input box. Enter ‘0’ in the Age input field.

11. In the Part 2 input field, enter ‘Material’ in the Material Type, ‘3:Grade C6000’ in the Material input field, ‘CS4’ in the Composite Stage field and enter '5' in the Age field

12. Click the  button

Define a composite section for construction stage

 Enter Construction Stage Analysis Data to perform construction stage analysis.

Main menu > [Analysis] tab > [Analysis Control] group >  Construction Stage

1. Select ‘Last Stage’ in Final Stage

2. Check ‘Include Time Dependent Effect’ in Analysis Option

3. Click the [Time Dependent Effect Control] button

4. Check on ‘Creep & Shrinkage’, Select Creep / Shrinkage

5. Enter Number of Iterations ‘5’ , and ‘0.01’ in Tolerance in the Convergence for Creep Iteration box.

6. Enter ‘1’ in the Internal Time Step for Creep field.

7. Check on ‘Auto Time Step Generation for Large Time Gap’

8. Check On ‘Variation of Comp. Strength’

Definition of construction stage analysis control

7. Perform Structural Analysis

The construction stage analysis input for the composite section has been completed, so structural analysis is performed.

Main menu > [Analysis] tab > [Perform] Group >  Perform Analysis

8. Review of Analysis Results

There are two methods of reviewing analysis results from construction stage analysis. One is to review accumulated member forces and displacements of all the members at each specific construction stage, and the other is to review the changes of stresses in each part of the composite section due to preceding construction stages in a table format.  

8-1 Check Member Forces

Review the member forces at the construction stage CS4, which represents the completion of long-term loss.

 Here Summation = Dead + Erection Load + Creep Secondary + Shrinkage Secondary

Main menu > [Results] Tab > [Load Type] Group > Analysis Result > [Result Display] Group > Forces >  Beam Diagrams

1. Select ‘CS4’ in Stage

2. Select ‘CS : Summation’ in the Load Cases / Combinations selection box.

3. Select ‘Last Step’ in the Step selection box.

4. Click ‘My’ in Components

5. Check ‘Contour’ in the Type of Display selection box.

6. Click the  button

Moment diagram in CS4

Next, check the moment change at each stage.

Moment diagram at each construction stage

8-2 Check Stresses

Review the stresses for each part of the composite section at the construction stage CS4, which represents the completion of long-term loss. 

Main menu > [Results] Tab > [Load Type] Group > Analysis Result > [Tables] Group > Result Tables > Composite Section for C.S >  Beam Stresses

1. Enter ‘19’ in the element input field.

2. Check on ‘Summation (CS)’ in the Load Cases / Combinations selection box.

3. In the Stage / Step selection box, ‘CS1 : 001(first) ~ CS4 : 002 (last)’ select

4. Select ‘Part j’ in the Part Number selection box.

5. Click the  button

Member force and stress table for each construction stage of the composite section

When live loads and general loads are applied after construction stages are completed, the program creates a new load combination to combine those loads and construction stage loads and determines stresses for PostCS design (i.e., Post Construction Stage design).