[CIVIL NX] Construction Stage Analysis using FCM Bridge Wizard – MIDAS Support

Download the following file

0. Contents

1. Overview	1-1 Bridge dimensions and section views 1-2 Construction stages for FCM and stage analysis 1-3 Procedure for performing construction stage analysis for FCM bridge 1-4 Material properties and allowable stresses 1-5 Loads
2. Setting modeling environment
3. Section and material property definition
4. FCM bridge wizard modeling	4-1 Model data input 4-2 PSC box section properties input 4-3 Tendon placement input
5. Corrections to input data and additional data input	5-1 Checking construction stages 5-2 Modifications to construction stages 5-3 Definition and link of time-dependent material properties 5-4 Removal of tapered section groups
6. Perform structural analysis
7. Review of analysis results	7-1 Checking stresses and member forces by graphs 7-2 Checking stresses using tables 7-3 Checking prestress losses 7-4 Checking tendon coordinates 7-5 Checking tendon elongation 7-6 Checking tendon arrangement 7-7 Checking pretension losses in tendons 7-8 Deformation at a specific construction stage 7-9 Resulting member forces at a specific construction stage 7-10 Camber check 7-11 Camber control management 7-12 Checking element properties by construction stages 7-13 Section properties at the last construction stage 7-14 Checking member forces resulting from load combinations

1. Overview

Some representative post-tensioned box girder bridges are constructed by ILM (Incremental Launching Method), FCM (Free Cantilever Method or Balanced Cantilever Method), MSS (Movable Scaffolding System), etc. FCM is generally used in a terrain where obstacles such as rivers, creeks and roads lie under the bridge, which present difficulties in installing conventional shoring. FCM is generally used for long span bridges, which are typically accompanied with high piers. Since it involves constructing balanced cantilevers from a pier, it is often referred to as a balanced cantilever bridge.

Similar to any other segmental construction methods, FCM presents structural system changes in each construction stage, and each structural system needs to be analyzed throughout the construction process. The analyses also must reflect time dependent material properties, tendon relaxation, tension losses in tendons, etc., whose effects are then accumulated through the various stages of construction.

In this tutorial, CIVIL NX FCM Wizard is used to model construction sequence; analysis is performed; and, results for stresses, prestress losses and deflections are reviewed in construction stages.

This is an example of cast-in-place bridges.

Analytical Model (Completed)

1-1 Bridge dimensions and section views

The specifications of the target bridge are as follows.

Sectional Elevation View

Section Views (Variable section)

Tendon Layout

1-2 Construction stages for FCM and stage analysis

The following outlines a general procedure for FCM construction

Note: This example is a 3-span FCM bridge constructed with 4 Form Travelers (FT). As such FT will not be relocated.

1-3 Procedure for performing construction stage analysis for FCM Bridge

The concept of construction stage analysis in CIVIL NX entails activation and deactivation of predefined Structure Groups, Boundary Groups and Load Groups at each stage of construction.

Step 1.	Define Material and Section Properties
Step 2.	Structural modeling
Step 3.	Define Structure Groups
Step 4.	Define Boundary Groups
Step 5.	Define Load Groups
Step 6.	Enter loads
Step 7.	Place Tendon
Step 8.	Apply Prestress Loads
Step 9.	Define & Link Time-Dependent Material Properties
Step 10.	Perform Structural Analysis
Step 11.	Check Results

FCM Wizard automatically performs steps 2 to 8 of the above procedures.

1-4 Material properties and allowable stresses

Top concrete	Design strength	f_ck= 400 kgf/cm²
	Initial compressive strength	f_ck= 270 kgf/cm²
	Elastic modulus	E_c=3,000((Wc)^1.5) √f_ck+ 70,000 = 3.07×10⁵kgf/cm²
	Allowable stress	Immediately after stressing	After final losses
	Compression	f'_ca= 0.55f_ci = 148.5 kgf/cm²	f_ca= 0.4f_ck = 160.0 kgf/cm²
	Tension	f'_ta= 0.8(f_ci)^0.5= 13.1 kgf/cm²	f_ta= 1.6(f_ck)^0.5= 32.0 kgf/cm²

Lower concrete	Design standard strength	f_ck= 270 kgf/cm²
Lower concrete	Elastic modulus	E_c = 2.35 x 10⁵ kgf/cm²
P.C Tendon wire (KSD 7002 SWPC 7B-Φ15.2mm (0.6˝strand)	Yield strength	f_py= 160 kgf/mm²
	Tensile strength	f_pu= 190 kgf/mm²
	Cross-sectional area	A_p= 138.7 cm²
	Elastic modulus	E_p= 2.0 x 10⁶ kgf/cm²
	Inducted post-tension	f_pj = 0.72f_pu = 137 kgf/mm²
	Anchorage slip	Δs = 6mm
	Friction loss coefficient	μ = 0.30 / rad, k = 0.006 / m
	Allowable stress	Maximum stress at prestressing	Immediately after anchoring ( f_po )	Service loads after losses
	Allowable stress	0.9f_py= 144 kgf/mm²	0.7f_pu= 133 kgf/mm²	0.8f_py= 128 kgf/mm²

1-5 Loads

Dead load	Self-weight	Use "Self Weight" command
Dead load	Superimposed dead load	w = 3.432 tonf/m
Prestress	Tension materials	ϕ 15.2 mm x 19 (ϕ 0.6'' - 19)
	Cross-sectional area	Ap = 1.387 x 19 = 26.353 cm²
	Duct Size	100/103 mm
	Prestress load (72% of tensile strength)	f_pi= 0.72f_pu= 13680 kgf/cm² P_j= A_pf_pj= 360.5 tonf
	Loss immediately after jacking/anchoring (Calculated by the program)	Friction loss: Top tendon: μ = 0.20, k = 0.001 Bottom tendon: μ = 0.30, k = 0.006
	Loss due to anchorage slip	ΔI_c = 6mm
	Loss due to elastic shortening	ΔP_E = Δf_p · A_sp
	Final loss (Calculated by the program)	Relaxation Loss due to creep and shrinkage

Creep and shrinkage	Cement	Normal (type 1) cement
	Concrete age when becoming subjected to the sustained loads	t0 = 5 days
	Concrete age when becoming exposed to ambient condition	ts = 3 days
	Relative humidity	RH = 70%
	Ambient temperature or curing temperature	T = 20℃
	Code	CEB-FIP
	Creep coefficient	Calculated by the program
	Shrinkage strain of concrete	Calculated by the program
Form traveler load	Loads are as follows	P = 80.0 tonf e = 2.50 m M = P x e = 200.0 tonf

2. Setting modelling environment

First, open a new file ( New Project) to model the structural member and save ( Save) it as 'FCM Wizard'.

Main menu > File > New Project

Main menu > File > Save

1. Enter ‘FCM Wizard’ in the file name Click the button

Save file

Set the units to ‘tonf’ & ‘m’. The units can be changed at any time depending on the type of modeling input and results.

Main menu > [Project] Tab > Unit System

Note

The Unit System can be changed using the unit selection button () in the Status Bar at the bottom of the screen.

1. Enter ‘m’ in the Length checkbox, and 'tonf’ in the Force (Mass) checkbox

2. Click the button

Setting Unit System

3. Section and material property definition

Defines the materials of the superstructure, substructure, and tendon.

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

1. Click the button

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

3. Check ‘KS-Civil (RC)’ in the Standard selection box and select ‘C400’ in the DB selection box.

Note

If you use the CGS unit system, use KS-Civil (RC), and if you use the SI unit system, use KS01-Civil (RC). choose

4. Click the button

Note

When defining several types of materials at once, it is convenient to use the Apply button.

5. Check ‘KS-Civil (RC)’ in the Standard selection box select ‘C270’ in the DB selection box.

6. Click the button

7. Enter ‘Tendon’ in the Name input field.

8. Select ‘User Defined’ in the Type of Design checkbox and select 'None' in the Standard selection box.

9. Enter ‘2.0e+7’ in the Modulus of Elasticity input field.

10. Enter '0.3' in the Poisson's Ratio input field.

11. Enter '1.0e-5' in the Thermal Coefficient.

12. Enter ’7.85’ in the Weight Density field.

13. Click the button

14. Click the button

Material Properties Dialog

Define the cross-sectional properties of the pier as User Type.

Note

Section properties of PSC box sections can be specified in the FCM Wizard.

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

1. Click the button

2. In the DB/User tab, check ‘1’ in the Section ID input field.

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

4. Select ‘Solid Rectangle’ in the Section Shape selection box.

5. After selecting the ‘User’ type in the image below, enter ‘1.8’ in the H input field and '8.1' in the B input field.

6. Click the button, Click the button

Section Properties Dialog

4. FCM bridge wizard modeling

FCM Bridge Wizard in CIVIL NX consists of three tabs - Model, Section and Tendon.

4-1 Model data input

Specify material properties, geometry, construction segments, pier table dimensions, pier type and size etc. in the Model Tab of FCM Bridge Wizard. Enter 12 days for constructing one segment (12 days).

Note

In this example, 7 day duration is assumed for installation of formwork, rebars, sheath, etc. followed by 5 days for casting and curing of concrete.

Main menu > [Structure] Tab > [PSC Bridge] Group > PSC Box Bridge> FCM Bridge

1. Check ‘Type1’ in the Bridge Model Data Type selection item.

2. In the Model tab, check ‘1 : C400’ in the Material (Girder) selection, Material (Pier) Select ‘2 : C270’ in the selection field.

3. Enter ‘2’ in the Number of Piers field.

4. Check ‘1 : Pier’ in the Pier Section selection and enter Stage Duration ’12’.

5. Check ‘Cast-in’ in the Method selection box.

6. Enter P.T. ’14’, and ‘6’ in input field of B of the Pier Table.

7. Enter ‘2’ in the K1 input field and ‘2’ in the K2 input field of the Key Segment.

8. Enter ’40’ in the H field and ‘4.2’ in the C field of the Pier.

9. Enter ‘2, 4@4.25’ in the FSM(L) input field and enter ‘2, 4@4.25' FSM(R) input field.

Note

Elements within the FSM zones are segmented to account for tendon anchors.

10. Enter ‘12@4.75’ in the Zone1 input field and Enter ‘12@4.75’ in the Zone2 input field.

Model Tab in FCM Bridge Wizard

Note

Click the button to save the Wizard data as a *.wzd file.

Note

Recall an existing *.wzd file by clicking button.

Note

A Curved FCM bridge can be modeled by checking on “Radius” and entering the radius value.

Note

A non-symmetrical FCM bridge or a FCM bridge constructed non-symmetrically, can be modeled by checking on “Advanced” and clicking the button.

Layout of construction segments

Construction Schedule (assumed)

In a typical FCM construction, not all the piers (substructures) are constructed simultaneously. As a result, the two cantilevers, which will be joined by a key segment, are not constructed at the same time, and the cantilevers have different ages at the time of erecting the Key Segment. Hence, the two cantilevers would undergo different creep, shrinkage and tendon losses, resulting in different stresses and deflections at the time of erecting the Key Segment. Such differences need to be reflected in preparing the construction stages for analysis.

CIVIL NX has a feature “Time Loads for Construction Stage", which is used to impose elapsed times to specific elements. The difference in ages (concrete maturity) of the two cantilevers in this example is because of the time difference in erecting the first segments of the two adjacent pier tables. The two identical piers are erected by the same schedule, but pier P2 is constructed at a later time relative to pier P1. Such a time difference can be handled by "Time Loads for Construction Stage".

Note

Time Loads for Construction Stage are defined in Load > Construction Stage Loads > Load >Time Loads for Construction Stage.

Figure illustrates the assumed construction schedule in which each horizontal line represents a 15-day duration. The construction of the first segment of pier P2 lags 60 days behind that of pier P1.

Click the button to enter the time difference between the construction times of the two pier tables.

1. Click the button

2. In P.T. click ‘P.T. 2’

3. Enter ’60’ in the Day input field.

4. Click the button then click the button.

Input for time difference between 2 Pier Tables

Concrete properties change with time. Such time-dependent properties change relatively rapidly in early ages. Construction dead loads are generally applied in early ages. The initial member ages represent the time when formwork and temporary supports are removed after curing, and the members are subjected to permanent loads. Using the initial member ages, the program automatically calculates the modulus of elasticity, creep coefficient and shrinkage coefficient. The initial member ages are specified by deducting the time spent for erecting formwork and rebar placement from the stage duration, and are as follows:

FSM zone	60 days
Key Seg	10 days
Pier Table	15 days
Segment	5 days
Pier	100 days

Click the button to enter the initial age for each main member.

1. Click the button

2. Enter ’60’ in the FSM input field, ‘5’ in the Segment input field, ’10’ in the Key Seg input field, Enter ‘100’ in the Pier input field and ’15’ in the Pier Table input field.

Note

The initial ages of the segments, whose self-weights of incompletely cured concrete are reflected in construction stages, and the initial ages of key segments, must be less than the duration for constructing one segment.

3. Click the button

Input for initial Member Ages of main members

4-2 PSC box section properties input

In a FCM bridge construction, the sections at the piers are deeper than those at the mid spans to resist high moments and shear forces for cantilevers. By specifying the sections at the supports and mid-spans, the program automatically generates variable section profiles of a second order function.

Note

Refer to the On-line manual, “Using CIVIL NX > Model > Properties > Tapered Section Group”

Enter the section dimensions referring to figure followed by selecting Drawing under View Option to verify the sections.The weight of the form traveler, which includes the formwork and its support devices, is entered with an eccentricity. This is internally converted into a vertical force and a moment, which are then applied at the end of the cantilever segment. If the “Include Wet Conc. Load” option is selected, the weight of the wet concrete is applied at the time of completing the formwork and rebar placement, which is the number of days equal to the stage duration less the member age. The member age in this case represents the curing period (in the immediately previous stage) of the member being activated in the current stage. After loading the form traveler, if the weight of the wet concrete is loaded with a time gap without changing the structural system, “Additional Steps” can be used rather than creating another construction stage.

Note

Additional Steps are explained in the On-line manual, “Using CIVIL NX > Load > Construction Stage Analysis Data > Define Construction Stage”

It is recommended to include wet concrete load while defining construction stages in the FCM Wizard, as it results in more conservative stress calculations. However, if the camber control is referenced at the time of setting the form traveler, the deflection due to wet concrete should be ignored, or additional construction stages should be defined.

Main menu > [Structure] Tab > [PSC Bridge] Group > PSC Box Bridge> FCM Bridge

1. In the Section tab, check ‘1 Cell’ in the Section Type selection item.

2. Enter ‘0.25’ in the H1 input field, ‘2.19’ in the H2 input field, and enter '0.26' in H3 input field.

3. Enter ‘0.35’ in the H4 field, ‘0.325’ in the H5 field, and enter '0.25' in H6 input field.

4. Enter ‘5.9’ in the H2-1 field and ‘0.85’ in the H3-1 field.

5. Enter ‘2.8’ in the B1 input field, ‘0.45’ in the B2 input field, and enter '3.1' in B3 input field.

6. Enter ‘1.75’ in the B4 field, ‘1.75’ in the B5 field, and enter '1.25' in B6 field.

7. Check on Include Wet Conc in Form Traveler Load (include form load).

8. Enter ‘80’ in the P input field and ‘2.5’ in the e input field.

9. Select ‘Drawing’ in the View Option selection.

PSC box section

Note

Selecting the 2 Cell option provides a section with a middle web.

Section dimensions Input

Note

The eccentricities (stiffness center location) of beam elements created in FCM Wizard are automatically referenced to the Center-Top. This is to reflect the variable PSC section. The stiffness is automatically calculated relative to the Center-Top.

4-3 Tendon placement input

The tendon placement and the number of tendons anchored in each stage are defined in the Tendon tab. Defining the tendon and anchorage locations in the section and the number of tendons anchored in each segment will automatically generate the tendon profile.

FCM Wizard permits only equally spaced tendons. For unequal spacings, an average spacing may be used, as it will not affect the overall construction stage analysis significantly.

Main menu >[Structure] Tab > [PSC Bridge] Group > PSC Box Bridge> FCM Bridge

1. In the Tendon tab, Check On in the Tendon and Prestress section.

Note

Tendon information can be entered using Tendon Profile even if Tendon Properties and Prestress have not been defined.

2. Check ‘1 Cell’ in the Section Type selection.

3. Enter ‘0.17’ in the H1 input field, ‘0.32’ in the H2 input field, and enter '0.29' in H3 input field.

4. Enter ‘0.14’ in the H4 input field, ‘0.1’ in the W1 input field, and enter '0.1' in W2 input field.

5. Enter ‘0.06’ in the W3 field and ‘0.175’ in the S field.

6. Enter ‘0.1’ in the DX1 input field, ‘0.3’ in the DY1 input field, and enter '0.1' in DX2 input field.

7. Enter ‘0.3’ in the DY2 input field, ‘0.3’ in the DX3 input field, and enter '0.19' in DY3 input field.

8. Click the button

9. Select 'Equal item'

10. Enter ‘7’ in the N1 input field, ‘3’ in the N2 input field, '6' in N3 input field and ‘3’ in the N4 field.

11. Enter ‘2’ in the N5 input field, ‘7’ in the N6 input field, '2' in N7 input field and ‘5’ in the N8 field.

Note

N7 and N8 represent the numbers of tendons in the FSM zones.

Note

Selecting “Unequal” in Tendon Number allows us to input different numbers of tendons in Top/Bottom by spans and piers.

12. Click the button

Center span tendon placement. End span tendon placement.

Tendon placement input

Enter the tendon properties and jacking stresses. The coefficients related to tendon losses are different for the top and bottom tendons, which are defined separately. 72% of the ultimate strength is specified for the jacking stress. Bottom tendons can be anchored away from the ends of the segments in which cases the anchor locations are specified in terms of segment length ratios.

Main menu > [Structure] Tab > [PSC Bridge] Group > PSC Box Bridge> FCM Bridge

1. In the Tendon tab, click Tendon Property. Click the button

2. Click the button

3. Enter ‘Top’ in the Tendon Name field.

4. Check ‘Internal (Post-Tension)’ in the Tendon Type selection box.

5. Select ‘3 : tendon’ in the Material selection box.

6. Enter ‘0.0026353’ in the Total Tendon Area field or click the button, select ‘15.2mm’ in the Strand Diameter selection box and then enter the Number of Strands as '19'.

7. Enter ‘0.103’ in the Duct Diameter input field.

8. Check On in the Relaxation Coefficient and select ‘CEB-FIP’ enter ‘5’.

Note

Relaxation Coefficient is based on Magura’s equation. For normal tendons, it is 10, and for low relaxation tendons, it is 45. Also, CEB-FIP and JTG-04 methods are available.

9. Enter ‘190000’ in the Ultimate Strength field and enter ‘160000’ in the Yield Strength field.

10. Enter ‘0.2’ in the Curvature Friction Factor input field.

11. Enter Wobble Friction Factor ‘0.001’

12. In Anchorage Slip (Draw in), enter ‘0.006’ in the Begin input field and Enter ‘0.006’ in the End input field.

13. After checking ‘Bonded’ among the Bond Type selection items click the button

14. Enter ‘Bot’ in the Tendon Name field.

15. Repeat steps '4~10'.

16. Enter '0.3' in the Curvature Friction Factor input field.

17. Enter Wobble Friction Factor '0.001'.

18. Repeat step '13~14'.

19. Click the button.

20. In the Tendon Property, enter ‘Top’ in the Top checkbox and 'Bot' in the Bottom checkbox.

21. Enter ‘0.72 × Su’ in the Top field and Bottom field of Jacking Stress.

22. Enter ‘1’ in the x input field of Anchorage Position and in Top Tendon Grouting select ‘Every’ in the selection field and ‘1’ in the input field.

Note

If Top tendon grouting is entered at Every 1 Stages, then the grouted section properties are calculated for the stage immediately after the grouted stage for stress calculations.

Tendon properties input

Longitudinal tendon layout

The tendon quantity increases with the increase in the cantilever length. In some segments 2 tendons are anchored. Specify the number of tendons anchored in each segment by referring to figure.

Main menu > [Structure] Tab > [PSC Bridge] Group > PSC Box Bridge> FCM Bridge

1. Tendon Anchorage Number, click the button

2. Select 'Equal'

3. Select ‘P.T, Seg6, Seg7, Seg8, Seg9, Seg10’ of Segment

Note

Multiple segments can be selected while pressing the [Ctrl] key.

4. Enter ‘2’ in the Anchor. Num field

5. Click the button then button

6. Tendon Anchorage Number, click the button

7. Select 'Equal'

8. Select ‘Seg1, Seg2, Seg3, Seg4, Seg12’ of Segment

9. Enter ‘0’ in the Anchor. Num field

10. Click the button the button

11. Tendon Anchorage Number, click the button

12. Select 'Equal'

13. Select ‘Seg1, Seg2, Seg3, Seg4, Seg12’ of Segment

14. After entering ‘0’ in the Anchor. Num input field, click the button

15. Select ‘Seg5, Seg11’ of Segment

16. Enter ‘2’ in the Anchor. Num field

17. Click the button then button

Input for the number of tendons anchored in each segment.

After finishing the input, click to end FCM Bridge Wizard and verify the modeling. Check the modeling of the bridge and tendon layouts. Use "Zoom Window" and "Zoom Fit" to closely view local parts.

1. Point Grid, Point Grid Snap, Line Grid Snap Button Check Off

2. Node Snap, Element Snap Button Check On

3. After clicking Display, go to the Tendon Profile Point item in the Misc tab. Check On

4. Check On in the Support, Elastic Link section of the Boundary tab.

5. Zoom Fit, Hidden Button Check On

Bridge model generated by FCM Bridge Wizard

Note

FCM Wizard automatically assigns roller conditions at each end of the bridge and fixed conditions for the pier supports. The Wizard also assigns infinitely stiff elastic links between the piers and the box girder sections.

5. Corrections to input data and additional data input

5-1 Checking construction stages

When Construction Stage is defined, CIVIL NX has two operational modes (Base Stage mode and Construction Stage mode)

In the Base Stage mode, all input related to the structural model data, loading and boundary conditions is permitted. No analysis is performed for the Base Stage. Structural analysis is performed for Construction Stage. In the Construction Stage mode, no structural data is permitted to be changed or deleted other than the Boundary and Load Groups included in each stage.

Construction Stage is defined by activating and deactivating Structure (element) Groups, Boundary Groups and Load Groups, not individual elements and boundary and load conditions. In the Construction Stage Mode, boundary and load conditions included in each activated Boundary Group and Load Group can be modified and deleted.

Note

In Construction Stage mode, nodes and elements cannot be changed or deleted. This can be done only in the Base Stage.

Construction sequence

The construction sequence shown in figure is summarized by relating it to activation and inactivation of Structure, Load and Boundary Groups in each construction stage.

Construction Stage 1	- Activate Structure Groups for piers & pier tables - Activation of Boundary Group (Support) - First day: Activation of pre-stress, form traveler (FT) and self-weight - 7th day: Activation of self-weight of wet concrete (segment 1)
Construction Stage 2	- Activation of Segment 1 - First day: inactivate FT and wet concrete of Construction Stage 1, and activate FT load and prestress - 7th day: Activation of self-weight of wet concrete (segment 2)
Construction stages 3 to 12	Repeat construction stage 2
Construction Stage 13	- Activation of Segment 12 - First day: inactivate FT and wet concrete of Construction Stage 12, and activate Key Seg. FT loads & prestress - 20th day: Activation of self-weight of wet concrete (Key Seg. 1 & Key Seg. 3)
Construction Stage 14	- Activation of Key Seg. 1, 3 and FSM 1, 2 - Activation of Boundary Group (FSM_Left, FSM_Right) - First day: inactivate FT loads and self-wt of wet concrete of Key Seg. 1 and Key Seg. 3, and activate prestress - Last day: activate elements at the Pier 1 side and time load for FSM1
Construction Stage 15	- Activation of self-weight of unhardened concrete of Key Seg. 2
Construction Stage 16	- Activation of Key Seg. 2 - First day: inactivate FT loads and self-wt of wet concrete, and activate prestress - First day: activate 2nd (superimposed) dead loads

Check the construction stages auto-generated by FCM Bridge Wizard. The Stage toolbar and Works Tree can be used to verify the construction stage information. From the Stage toolbar, each construction stage can be checked for activated and deactivated Structure Group, Boundary Group and Load Group in conjunction with Works Tree. The Stage toolbar also enables us to check the change of structures through the various construction stages in the Model View.

1. After clicking Display, Check On 'Load Value' among the Load Case items in the Load tab.

2. After Check On in the Nodal Load item click button

3. Go to Works tab in Tree Menu

4. Select ‘CS4’ in the Stage selection box.

Note

After placing the cursor on the Stage Toolbar, arrows on the keyboard can be used to navigate between the stages. The wheel mouse can be used as well.

Structural system for the construction stage 4

5-2 Modifications to construction stages

In FCM Wizard, we have specified 12 days for constructing each segment. However, 30 days are required for constructing a Key Segment as per Figure. Accordingly, after activating segment 12, preparation for the construction of Key Segment is 30-10=20 days (where 10 is the initial age of Key Segment). We then correct the construction stage duration for segment 12 to 30 days and assign an “Additional Step” of 20 days for applying the wet concrete weight of the Key Segments (KeyWC1 and KeyWC3).

Select ‘Base’ in the Stage selection box, Hidden Button Check Off

Note

Change to Base Stage. Construction stage information can be changed in Base Stage only.

Main menu > [Load] Tab > [Construction Stage] Load Type> Define C.S

1. After selecting ‘CS13’ in Name, click the button

2. Enter ’30’ in the Duration field of Stage.

3. After selecting Step 1 of Additional Steps, click the button. After entering ’20’ in the Day input box, click the button

4. In the Load tab, select KeyWC1 and KeyWC3 in Activation and select '20' in the Active Day selection box

Note

Auto-generated Element, Boundary and Load Groups by Bridge Wizard is explained in “Define Structure (Boundary, Load) Group” in on-line manual.

5. Click the button

6. Click the button and then click the button.

Corrections to Construction Stage 13 information

Similarly for Stage 13, Stage 15 is corrected. The construction schedule on Figure indicates that the duration for constructing Key Segment 2 is 30 days. The stage duration for the Stage 15 is thus changed to 30 days.

Main menu > [Load] Tab > [Construction Stage] Load Type> Define C.S

1. After selecting ‘CS15’ in Name, click the button

2. Enter ’30’ in the Duration field of Stage.

3. Enter ’20’ in the Day input field of Additional Steps. Click the button

4. In the Load tab, select KeyWC2-1 and KeyWC2-2 in Activation and then select '20' in the Active Day selection box.

5. Click the button.

6. Click the button and then click the button.

Corrections to Construction Stage 15 information

Once all the Key Segments are constructed, the 2nd dead load (superimposed dead load - pavement, barriers, railings, etc.) is applied. It is assumed that the camber control management due to creep is carried out until 10,000 days after applying the 2nd dead load. We will apply the 2nd dead load in CS16 and assign 10,000 days for its duration. For this, a load case is defined, and a Load Group is created.

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

1. Enter ‘2nd’ in the Name input field.

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

3. Click the button and then click the button.

Main menu > [Structure] Tab > [Group] Group > Define Load Group

1. Enter ‘2nd’ in the Name input field.

2. Click the button and then click the button

Definition of Load Case and creation of Load Group

We apply the 2nd dead load, 3.432 tonf/m, in the –Z direction

Main menu > [Load] Tab > [Static Loads] Load Type > Element Beam Loads

1. Click Display and go to Load tab

2. Check Off Nodal Load

3. Go to the Misc tab and Check Off the Tendon Profile section.

4. Go to the Boundary tab and Check Off the Support and Elastic Link items.

5. Click the button

6. Click Front View

7. Click Select Window and select ‘Area ①’ in the picture below.

8. Select ‘2nd’ in the Load Case Name selection box.

9. Select ‘2nd’ in the Load Group Name selection box.

10. Check ‘Add’ in the Options selection and select the Load Type as ‘Uniform Load’.

11. Select ‘Global Z’ in the Direction selection box and then select 'No' in the Projection box.

12. Check ‘Relative’ in the Value selection.

13. Enter ‘0’ in the x1 field, ‘1’ in the x2 field, and enter W in the field. Enter ‘-3.432’

14. Click the button

Applying the 2^nd dead load

In Stage 16, Load Group “2nd" is activated, and its duration is changed to 10,000 days.

Main menu > [Load] Tab > [Construction Stage] Load Type> Define C.S

1. Select ‘CS16’ in Name

2. Enter ‘10000’ in the Duration field of Stage.

3. Move to the Load tab and select ‘2nd’ from the Group List

4. Check ‘First’ in the Active Day selection box of Activation. Click the button

5. After clicking the button, click the button

Corrections to Construction Stage 16 information

We will now check the construction stage data input. Activation (symbol “O”) and deactivation (symbol “X”) of Structure, Boundary and Load Groups are summarized.

Main menu > Load > [Construction Stage] Load Type> Group Activation of CS

Structure Group Activation Summary

5-3 Definition and link of time-dependent material properties

Having completed the modeling of the structure, we now define the time dependent material properties (compressive strength gain curve, creep and shrinkage coefficients) and link them to each section.

Note

Since the creep and shrinkage coefficients are a function of physical shapes (Notational Size of Member), we will define the time dependent material properties after determining the variable section dimensions.

Based on the CEB-FIP standards, different section dimensions result in different creep and shrinkage coefficients. That is, each section must be linked to the corresponding time dependent material properties. CIVIL NX automatically calculates time dependent material properties based on the concrete maturity (age) and apply them to the corresponding materials. Using "Change Element Dependent Material Property", the time dependent material properties are calculated as per CEB-FIP and automatically assigned to each corresponding element.

Note

In order to automatically link (regular) material properties and time dependent material properties, section properties must be defined by DB/User Type or PSC Type.

The procedure for applying creep and shrinkage coefficients to the tapered elements by the "Change Element Dependent Material Property" function is as follows:

1. Define creep and shrinkage material properties as per CEB-FIP

2. Link time dependent material properties to (regular) material properties

3. Using the "Change Element Dependent Material Property" function, assign "Notational Size of Member" (dimensions of elements) to the elements

When the above procedure is followed, the coefficients defined in the step 1 are not applied, and rather the creep and coefficients are calculated based on the member sizes defined in the step 3 and applied to the elements having the "Change Element Dependent Material Property" values.

Enter the time-dependent material properties by referring to the following values.

28 day strength	f_ck = 400 kgf/cm²(PSC box girder), 270 kgf/cm²(pier)
Relative humidity	RH = 70%
Notational Size	specify an arbitrary value (the above step 3 overrides this)
Type of concrete	Normal concrete (N.R)
Time at which formwork is removed	3 days

Main menu > [Properties] Tab > [Material Properties] Group > Time-Dependent> Creep / Shrinkage

1. Click the button

2. Enter ‘C400’ in the Name input box and then enter the Code selection box. Select ‘CEB-FIP (1990)’

3. Enter '4000' in the Characteristic Compressive strength of concrete at the age of 28 days.

Note

28 days strength is converted into the current unit system.

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

5. Enter ‘1’ in the Notational size of member field.

6. In the Type of cement selection item, select ‘Normal or rapid hardening cement (N, R)’

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

8. Click the button

9. Enter ‘C270’ in the Name input box and then enter the Code selection box. Select ‘CEB-FIP (1990)’

10. Enter '2700' in the Characteristic Compressive strength of concrete at the age of 28 days.

Note

28 days strength is converted into the current unit system.

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

12. Enter ‘1’ in the Notational size of member input field.

13. In the Type of cement selection item, select ‘Normal or rapid hardening cement (N, R)’

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

15. Click the button and then click the button

Definition of creep and shrinkage material properties

The curve for gain in concrete strength is defined for each grade of concrete. Such strength changes affect the modulus of elasticity. CEB-FIP code is used. Also the values used for defining creep and shrinkage are entered for defining concrete strength.

Main menu > [Properties] Tab > [Material Properties] Group > Time-Dependent> Comp. Strength

1. Click the button

2. Enter ‘C400’ in the Name field and check ‘Code’ in the Type selection field.

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

4. Enter ‘4815.773’ in the Mean compressive strength of concrete at the age of 28 days field

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

6. Click the button

7. Click the button

8. Click the button

9. Enter ‘C270’ in the Name field and check ‘Code’ in the Type selection field.

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

11. Enter ‘3515.773’ in the Mean compressive strength of concrete at the age of 28 days field

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

13. Click the button

14. After clicking the button, click the button

Definition of strength gain curve

The time dependent material properties (which are used in construction stages) are linked to the (regular) material properties (which are used in post construction stages).

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

1. Select ‘C400’ in the Creep/Shrinkage selection box of Time Dependent Material Type.

2. Select ‘C400’ in the Comp. Strength selection box

3. After selecting ‘1 : C400’ in Materials of Select Material to Assign, click the button

4. Click the button

5. Select ‘C270’ in the Creep/Shrinkage selection box of Time Dependent Material Type.

6. Select ‘C270’ in the Comp. Strength selection box.

7. After selecting ‘2 : C270’ in Materials of Select Material to Assign, click the button

8. Click the button

Time dependent material properties link

When Notational Size of Member, h, is defined in "Change Element Dependent Material Property", the “h” value that was defined in Time Dependent Material (Creep/Shrinkage) is ignored. New creep and shrinkage functions are calculated based on the “h” values defined in "Change Element Dependent Material Property" and are assigned to individual elements.

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

1. Click on Select all

2. Check ‘Add / Replace’ in the Option selection.

3. Select ‘Notational Size of Member’ in the Element Dependent Material selection box and select ‘Auto Calculate’

Note

Selecting “Auto Calculate” automatically calculates the “h” values for all the selected elements, which are applied to the calculation of creep and shrinkage. Selecting “Input” allows us to specify user-defined “h” values for selected elements.

4. Select ‘CEB-FIP’ in the Code selection box.

5. Click the button

Input for Notional Size of Member, h

Note

When calculating geometric dimensions (h), select and use the applicable national standards. CIVIL NX provides CEB-FIP, Korea, Japanese, Chinese Standard.

5-4 Removal of tapered section groups

FCM Wizard creates tapered section group for non-prismatic elements. The "Tapered Section Group" function automatically calculates the section properties of the varying element sections based on the section information at both ends of a member. CIVIL NX calculates all the section properties of the elements assigned in "Tapered Section Group" prior to performing analysis and retains the section data for analysis. Hence, it is recommended to remove Tapered Section Group prior to performing analysis, to save time.

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

1. Select ‘TSGroup1 ~ 4’ in Name

Note

Select TSGroup1~4 in the list box at the bottom.

2. Click the button

3. Enter ‘1’ in the New Start Section Number input field

Note

Enter the starting number for newly created tapered section data as a result of removal of Tapered Section Groups.

4. Click the button

Removal of Tapered Section Group

6. Perform structural analysis

Having completed defining the structural model and construction stages, we now select the options to consider time dependent material properties and tension losses in tendons for construction stage analysis. We also define the convergence and iteration conditions for creep.

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

1. Check ‘Last Stage’ in the Final Stage selection.

2. In the Include Time Dependent Effect item of Analysis Option Check On

3. Check On in the Creep Shrinkage item of Time Dependent Effect

4. Enter ‘Creep & Shrinkage’' in the Type selection field

5. Enter ‘5’ in the Number of Iteration field of Convergence for Creep Iteration and enter ‘0.01’ in the Tolerance input field.

6. Check On in the Auto Time Step Generation for Large Time Gap item

Note

If “Auto Time Step Generation” for Large Time Gap is checked on, additional time steps will be generated for those stages having duration beyond the specified periods to reflect long term effects.

7. Check On Tendon Tension Loss Effect (Creep & Shrinkage)

8. Check On Variation of Comp. Strength

9. Check On Tendon Tension Loss Effect (Elastic Shortening)

10. Select ‘Change with Tendon’ in the Beam Section Property Changes selection field

Note

If“Change with Tendon” is checked on, the stiffness change in tendons is reflected in calculating construction stage stresses.

11. Check On in the Save Output of Current Stage(Beam/Truss) selection.

Note

If Save Output of Current Stage (Beam/Truss) is checked on, member forces at the current stage can be separately checked.

12. Click the button

Definition of control parameters for construction stage analysis

When construction stage analysis is carried out, construction stage load cases are automatically generated. The loadings that are applied in construction stages are predominantly due to self-weight. Hence, the program generates all the loads lumped into “CS: Dead”, except for creep, shrinkage and tendon loads. If there is a specific load case which needs to be separated from the “CS: Dead”, such a load case is selected and assigned to “Load Cases to be Distinguished from Dead Load for CS Output”, which is then classified as CS: Erection. For example, this function may be applied when we need to separately check the effects of form traveler loads from the total stage analysis results.

Up to this point all inputs, including structural modeling and construction stage configuration, have been completed. We will now perform analysis.

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

7. Review analysis results

Construction stage analysis results can be checked in two ways. Stresses and displacements accumulated up to a specific construction stage for all the members can be checked, or the change in stresses and displacements of a specific element can be checked with the progress of each construction stage. CIVIL NX generates graphs and tables to check both results.

7-1 Checking stresses and member forces by graphs

We will review the stresses at the section bottom at the stage 13 where the largest compressive stress occurs.

Main menu > [Results] Tab > [Bridge Specialization] Type > Bridge Girder Diagrams

1. Select ‘CS13’ in the Stage selection box.

2. Among the Step List items in Load Cases/Combinations, check on First Step and User Step.

3. Select ‘CS: Summation’ in the Load Cases/Combination selection box.

4. Select ‘Stress’ in the Diagram Type selection and then select X-Axis Type as ‘Node’

5. Select ‘BridgeGirder’ in the Bridge Girder Elem. Group check box.

Note

In FCM Wizards, Structure Groups for section stress checks are automatically generated. Bridge Girder is an element group to which the main girder is assigned.

6. After selecting ‘Combined’ in the Components selection field, Select ‘Maximum’

7. Check on Draw Allowable Stress Line of Allowable Stress Line section

8. Enter ‘1600’ in the Comp. input field and then enter '320' in the Tens. input field

9. Select ‘Current Stage-Step’ in the Generation Option selection.

10. Click the button

Bottom stress graph at the construction stage 13

If any specific area of the graph needs to be magnified, drag the mouse on that area, keeping the mouse button clicked. To revert back to the entire graph, right-click the mouse and select “Zoom-Out All”.

Magnifying the stress graph

Using the "Stage/Step History Graph", we will check the change of stresses with construction stages for the pier table (element 19, i-end) on a graph.

Note

Stage/Step History Graph can be viewed only when the Model View is active.

Main menu > [Results] Tab > [Analysis Results] Type > [C.S/ Nonlinear] Group > Stage / Step Graph

1. Select ‘Beam Force / Stress’ in the Define Function selection box.

2. Click the button

3. Enter ‘Top’ in the Name field of Beam Force/Stress.

4. Enter Element No. ’19’ in the input box and select ‘Stress’

5. Select ‘I-Node’ in the Point selection box and then select ‘Bend (+z)’ in the Components selection box.

6. After Check On in the Combine Axial item, click the button

7. Click the button

8. Enter ‘Bot’ in the Name field of Beam Force/Stress.

9. Enter Element No. ’19’ in the input box and select ‘Stress’

10. Select ‘I-Node’ in the Point selection box and then select ‘Bend (-z)’ in the Components selection box.

11. After Check On in the Combine Axial item, click the button

12. Check ‘Multi Func.’ in the Mode selection item.

13. Select ‘All Steps’ in the Step Option selection and then select ‘Stage / Step’ in X-Axis input field.

14. Check On the Top and Bot items of Check Function to Plot.

15. Select ‘Summation’ in the Load Cases/Combinations checkbox.

16. Enter ‘Stress History’ in the Graph Title field.

17. Click the button

Graph showing the change of stresses by construction stages

Invoke the Context Menu in the "Stage/Step History Graph" by right-clicking the mouse. Select "Save Graph As Text" in the Context Menu and save the change in stresses in text form.

1. Right-click and select ‘Save Graph As Text’

2. Enter ‘Stress History’ in the file name input field.

3. Click the button

Saving stresses by construction stages as a text format

Using "Stage/Step History Graph", we will now check the change in member forces by construction stages for the pier table (element 19, i-end) on a graph

Main menu > [Results] Tab > [Analysis Results] Type > [C.S/ Nonlinear] Group > Stage / Step Graph

1. Select ‘Beam Force / Stress’ in the Define Function selection box.

2. Click the button

3. Enter ‘Moment’ in the Name input field of Beam Force/Stress.

4. Enter Element No. ’19’ in the input box and select ‘Force’

5. Select ‘I-Node’ in the Point selection box and then select 'Moment-y' in the Components selection box.

6. Click the button

7. Select ‘Multi LCase’ in the Mode selection field.

8. Select ‘Last Steps’ in the Step Option selection and then select ‘Stage / Step’ in X-Axis

9. Check on Load Cases to Plot

Dead Load, Erection Load, Tendon Primary, Tendon Secondary, Creep Primary, Shrinkage Primary, Creep Secondary, Shrinkage Secondary, Summation

10. Select ‘Moment’ in the Defined Functions check box.

11. Enter ‘Moment’ in the Graph Title field.

12. Click the button

Graph showing the change in forces by construction stages

7-2 Checking stresses using tables

When construction stage analysis results are checked in tables, Records Activation Dialog is used to sort the results by elements, load cases, stages, element parts of interest, etc. We will check the change in stresses with construction stages at the end of a pier table.

Main menu > [Results] Tab > [Analysis Results] Type > [Tables] Group > Stresses > Stresses (PSC)

1. Enter ’19’ in the Element input field.

2. Check On Summation (CS) in the Load case/Combination item

3. Check On CS1:001(first) ~ CS16:002(last) of Stage/Step

Note

By selecting CS1 and CS16 while the Shift key is pressed, we can select all the construction stages from CS1 to CS16.

4. Check On Part i of Part Number

5. Check On Pos-3 of Section Position

6. Click the button

Table showing stresses by construction stages.

7-3 Checking prestress losses

We will check the change in tension with construction stages due to prestress losses in the "Tendon Time Dependent Loss Graph" dialog, only the tendons which exist in the current stage, can be checked. Hence, it is necessary to revert to the construction stage in which the tendon intended to be examined is included. For viewing the change of tension in a tendon with construction stages, click the button.

Main menu > [Results] Tab > [Bridge Specialization] Type > Tendon Loss Graph

1. Select ’Top01-01’ in the Tendon selection box.

2. Click the button

Prestress loss graph

7-4 Checking tendon coordinates

CIVIL NX provides the coordinates of tendons at the quarter points of the elements to which tendons are assigned.

Main menu > [Results] Tab > [Result Tables] Group > Tendon > Tendon Coordinates

Table of tendon coordinates

7-5 Checking tendon elongation

CIVIL NX provides the elongation of tendons.

Main menu > [Results] Tab > [Result Tables] Group > Tendon > Tendon Elongation

Tendon elongation table

7-6 Checking tendon arrangement

The effective stress and prestress forces in the tendons are tabulated as per tendon groups and construction stages.

The distance from the center of tendon group to the section centroid, directional cosine of tendon placement, vertical and horizontal components of tendon forces, etc. are tabulated.

Main menu > [Results] Tab > [Result Tables] Group > Tendon > Tendon Arrangement

Tendon arrangement table

7-7 Checking pretension losses in tendons

Tension losses due to friction, anchorage draw-in, elastic shortening, creep, shrinkage and relaxation are generated.

Main menu > [Results] Tab > [Result Tables] Group > Tendon > Tendon Loss

Tendon loss (stress and force) tables

7-8 Deformation at a specific construction stage

CIVIL NX provides a function, which enables us to check the deformation of the structure at a specific stage. We will check the deformation at construction stage 13.

Main menu > [Results] Tab > [Result Display] Group > Deformations > Deformed Shape

1. Click on Front View

2. Select ‘CS13’ in the Stage selection box.

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

4. Select ‘DXYZ’ in the Components selection.

5. Check on Legend, Current Step Displ. in Type of Display

6. Click the button

Deformation at a specific construction stage

7-9 Resulting member forces at a specific construction stage

Use the "Beam Diagram" option to check the member forces generated in diagram format.

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

1. Select ‘CS13’ in the Stage selection box.

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

3. Check ‘My’ in the Components selection.

4. Check on Contour, Legend, Current Step Force item of Type of Display checkbox

5. Click the button

Member forces at construction stage 13

Use the "Beam Stresses (PSC)" function to check the stresses of the PSC cross-sectional beam elements in diagram format. Superior and inferior margins (1 to 4), central region (7, 8) and the shear review location (5, 6, 9, 10) set when defining the PSC cross section.

Check the lower edge stress for CS:Summation at construction stage CS13.

Main menu > [Results] Tab > [Analysis Results] Type > [Tables] Group > Beam > Stress (PSC)

1. Select ‘CS13 in the Stage selection box.

2. Check ‘CS : Summation’ in the Load Cases/Combinations selection and then Step Select ‘Last Step’ in the checkbox

3. Select ‘Sig-xx (Summation)’ in the Components selection field.

4. Check on Contour, Legend item of Type of Display checkbox

5. Click the button

Check lower edge stress at construction stage 13

Using the User Defined Diagram, you can check different displacement/member force/stress results for each element/group.

Displacement results for the left span, bending moment for the center span, and stress results for the right span are displayed simultaneously on one screen.

Main menu > [Results] Tab > [Results] Group > Diagram > Define Diagram

1. Select ‘CS13’ in the Stage selection box.

2. Enter ‘1to35’ in the Element input field.

3. Select ‘Beam Forces / Moments’ in the Type of Result check box.

4. Select ‘My’ in the Component selection field.

5. Enter ‘Left-My’ in the Group Name field.

6. Click the button

7. Enter ‘38to72’ in the Element input field.

8. Select ‘Beam Stresses’ in the Type of Result check box.

9. Select ‘Combined’ in the Component selection and select ‘Maximum’ select

10. Enter ‘Right-Normal’ in the Group Name field.

11. Click the button

Main menu > [Results] Tab > [Results] Group > Diagram > Plot Diagram

1. Check On the Left-My, Right-Normal items of the Diagram Group

2. Click the button

User Defined Diagram output

Note

Different types of results can be combined and generate output for the same construction stage.

7-10 Camber check

In order to produce a camber graph, we need to select element and node groups corresponding to girders, supports and key segments. FCM Bridge Wizard automatically defines all the groups required for camber results. Select Camber Control groups to check cambers.

Main menu > [Results] Tab > [Bridge Specialization] Type > FCM Camber > FCM Camber Control

1. Select ‘Bridge Girder’ in the Bridge Girder Element Group check box.

2. Select ‘SupportNode’ in the Support Node Group selection box.

3. Select ‘KeySegAll’ in the Key-Segment Elem. Group check box.

4. Click the button

Main menu > [Results] Tab > [Bridge Specialization] Type > FCM Camber > FCM Camber Graph View

5. Check On in the Summation item of Camber Load Case

6. Click the button

Camber graph

7-11 Camber control management

Check the camber table, which will be used to manage cambers during construction. Camber tables are produced for each FSM zone and pier. In this example, FSM1 & FSM2 (pages 1 & 4, respectively) and Pier 1 & Pier 2 (pages 2 & 3, respectively) are generated.

Main menu > [Results] Tab > [Bridge Specialization] Type > FCM Camber > FCM Camber Table

1. Check On the Summation item of Camber Load Case

2. Click the button

Camber control table

7-12 Checking element properties by construction stages

For each construction stage, element properties (start maturity age, end maturity age, Modulus of Elasticity at start & end, accumulated shrinkage strain and accumulated Creep Coefficient are tabulated.

Main menu > [Results] Tab > [Result Tables] Group > Construction Stage > Element Properties at Each Stage

1. Select ‘CS14’ in the Stage selection box.

2. Click the button

Element properties at construction stage 14

7-13 Section properties at the last construction stage

When construction stage analysis is performed, transformed section properties at the last stage are tabulated.

Note

*.out file, which is generated after analysis, contains the properties of transformed sections at each construction step.

The properties of transformed sections, which include tendons, vary with tendon properties, grouting timing and the change in modulus of elasticity of concrete.

Since the transformed section properties are generated at the last stage, it is easy to check the properties in “PostCS” (completed stage). These properties can be used to calculate stresses due to additional loads such as moving loads, temperature loads, etc.

Main menu > [Results] Tab > [Result Tables] Group > Construction Stage > Beam Section Prop. at Last Stage

1. Select ‘Post CS’ in the Stage selection box.

2. Enter ‘1to76’ in the Beam Element input box and Check On ‘I, J’ in Part field

3. Click the button

Element properties at last construction stage

7-14 Checking member forces resulting from load combination

Once the PSC box bridge has been constructed, wearing surface, live load, temperature change, support settlement, etc. need to be combined with the effects of construction dead load. Structural analysis for loads other than the Construction Stage Load is carried out in the PostCS Stage (final stage). Such PostCS loads can be combined with the results of the construction stage analysis. Since we have not specified any load other than the construction stage load in this example, we will define load factors for the construction stage loads and check member forces. First, we will define the load combinations.

Select ‘PostCS’ in the Stage selection box.

Main menu > [Results] Tab > [Combination] Group > Load Combination

1. Enter ‘Dead’ in the Name input field.

2. Select ‘Active’ in the Active check box.

3. Check ‘Add’ in the Type selection box.

4. Select ‘Dead Load (CS)’ in the Load Case selection box and enter '1.3' in the Factor input field.

5. Select ‘Erection Load (CS)’ in the Load Case selection box and enter '1.3' in the Factor input field.

6. Select ‘Tendon Secondary (CS)’ in the Load Case selection box and enter '1.0' in the Factor input field.

7. Select ‘Creep Secondary (CS)’ in the Load Case selection box and enter '1.3' in the Factor input field.

8. Select ‘Shrinkage Secondary (CS)’ in the Load Case selection box and enter '1.3' in the Factor input field.

9. Click the button

Definition of load combinations

Check bending moment diagram due to factored load combination.

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

1. Check ‘CB : Dead’ in the Load Cases / Combinations selection box.

2. Select ‘My’ in the Components selection field.

3. Check ‘5 Points’, ‘Line Fill’ in Display Options and enter them in the Scale input field. Confirm ‘1.0’

4. Check On the Contour and Legend items of Type of Display

5. Click the button

Bending moment diagram