Construction Stage Analysis Control
A civil structure such as a suspension bridge, cable stayed bridge or PSC (prestressed or post-tensioned concrete) bridge requires separate and yet inter-related analyses for the completed structure and interim structures during the construction. Each temporary structure at a particular stage of construction affects the subsequent stages. Also, it is not uncommon to install and dismantle temporary supports and cables during construction. The structure constantly changes or evolves as the construction progresses with varying material properties such as modulus of elasticity and compressive strength due to different maturities among contiguous members. The structural behaviors such as deflections and stress re-distribution continue to change during and after the construction due to varying time dependent properties such as concrete creep, shrinkage, modulus of elasticity (aging) and tendon relaxation. Since the structural configuration continuously changes with different loading and support conditions, and each construction stage affects the subsequent stages, the design of certain structural components may be governed during the construction. Accordingly, the time dependent construction stage analysis is required to examine each stage of the construction, and without such analysis the analysis for the final stage alone will not be reliable.
1. Creep effects of concrete members having different maturities
2. Shrinkage effects of concrete members having different maturities
3. Time dependent compressive strength gain for concrete members
4. Prestressing tendon relaxation
1. Creation (activation) and deletion (deactivation) of members with certain maturities.
2. Loading (activation) and unloading (deactivation) of loads relative to time
3. Change of boundary conditions relative to time
1. Model the structure.
2. Define the time dependent material properties such as creep and shrinkage. The time dependent material properties may be user defined or defined by the standards such as ACI and CEB-FIP. (Time Dependent Material(Creep/Shrinkage), Time Dependent Material(Comp. Strength))
3. Link the defined time dependent material properties to the general material properties through which the change of the concrete member material properties with time are automatically calculated and reflected. (Time Dependent Material Link)
4. Create the construction stages and time steps considering the true sequence of construction. (Define Construction Stage)
5. Define the construction stages using the predefined Element groups, Boundary groups and Load groups. (Define Construction Stage)
7. Combine the results of the construction stage analysis and that of the completed structure analysis as necessary.
The procedure for construction stage analysis is shown below.
From the Main Menu select Analysis > Analysis Control > Construction Stage.
Assign a stage to be considered as the Final Stage of the construction stage analysis.
Restart Construction Stage Analysis
Restart the construction stage analysis from the stage specified by the user. Restarting the analysis from the modified stage will save time.
: Select the stages to be used for Restart.
Include P-Delta Effect Only
Include Equilibrium Element Nodal Forces
Include Time Dependent Effect
Time Dependent Effect
If "Include Time Dependent Effect" is checked on in the Analysis Option,Click the to get the dialog box to input the time dependent information.Define the material properties related to creep and shrinkage in Time Dependent Material(Creep/Shrinkage)
Creep & Shrinkage
Convergence for Creep Iteration
Number of Iterations: Maximum number of repetitions
Tolerance: for convergence
Only User's Creep Coefficient
Internal Time Steps for Creep
Auto Time Step Generation for Large Time Gap
Tendon Tension Loss Effect (Creep & Shrinkage)
Consider Re-Bar Confinement Effect
Variation of Comp. Strength
Tendon Tension Loss Effect (Elastic Shortening)
Prestressing tension loss in tendons due to elastic deformations is caused by other loadings such as live loads, creep, shrinkage, prestressing other tendons, etc after the prestressing force is applied. Note that it is not the same as the elastic shortening loss, which is one of the instantaneous losses.
Click on the after checking the "Nonlinear Analysis control" and enter the following information in the dialog box below:
Number of Load Steps: Input the number of load steps for the non linear analysis.
Maximum Number of Iterations/Load Step: Maximum number of iterations of analysis per Load Step.
Convergence Criteria: Specify the basis on which to assess the convergence. Enter the norm values for Energy (Member force x displacement), displacement and member forces.
Click on after checking on "Include P-Delta Effect Only" under the Analysis Option and enter the following data in the dialog box
Number of Iterations: Maximum number of iterations of analysis
Convergence Tolerance: Tolerance for convergence
Load Cases to be distinguished from Dead Load for CS Output
Dead Load is generally the most significant component of all the loads applied to construction stage analysis. The results of all the load cases except for Creep, Shrinkage and Relaxation of Tendons are lumped into CS: Dead Load. Here we can select certain load cases to be distinguished from the Dead Load and produce the results under CS: Erection Load.
Add : Add an erection load case to be distinguished from Dead Load for C.S. Output.
Modify : Modify an existing erection load case selected from the list.
Delete: Delete the selected erection load cases from the list.
Load Case Name: Select the Load cases to be distinguished from Dead Load
Load Type for CS: Specify a load type classified into CS:Erection, which is differently categorized from CS:Dead. This is helpful in distinguishing the pre-composite dead load from the post-composite long term loads for the Steel Composite design as per AASHTO code. This is effective when the Auto Generation function is used for generating the load combinations.
Assignment Load Cases: Select the load cases from the load case list to be classified as erection loads.
Cable-Pretension Force Control
Define the method of applying the pretension forces in cable elements.
Internal force: Apply the pretension forces as internal forces (which change after redistribution within the structure in the current construction stage).
External force: Apply the pretension forces as external forces forces (which remain unchanged in the current construction stage).
Pretension load of Internal Type is applied as deformation in the member equivalent to the pretension load, and the overall structure is analyzed. The resulting member force depends on the stiffness of the end nodes to which the member is attached. Upon applying the deformation to the truss member, large nodal displacements of the end nodes would imply a small member force, and vice versa. If the end nodes are fixed, the resulting member force will be equal to the specified pretension load. When other loads are acting on the member in the same load case, the principle of superposition applies.
Pretension load of External Type is applied to a member when we wish to impose the member to be subjected to the specified pretension load, while the overall structure is analyzed. This leads to the applied pretension load becoming equal to the resulting member force. When a pretension load is inducted into a cable in a particular construction stage, we are controlling the tension in the cable as opposed to controlling its deformation to a uniform magnitude. The External Type load has been implemented so that a specific tension force can be maintained in a particular cable in a particular construction stage. If other loads are applied to the member in the same load case, the resulting member force will remain constant as the pretension load.
The External Type load can be used only in the current construction stage. The options, Add and Replace, are provided to handle when pretension load is input more than once. If Add is checked on, any subsequent pretension load applied to a member will be added to the pre-existing force in the member. If Replace is selected, a pretension load applied to a member is maintained considering the pre-existing member force. The program automatically computes the additional tension force to make the tension force in the member equal to the specified pretension value.
Since a pretension is a loading, it is independent of the stiffness of the structure. Even in the case of the cable element, whose stiffness changes with tension forces, pretension is treated as a regular load.
Add: Add external pretension forces to the pre-existing tension forces of cable elements.
Replace: Replace the pre-existing tension forces of cable elements with applied external pretension forces.
Initial Force Control
Convert final stage member forces to Initial forces for PostCS
The member (axial) forces of the last step of the last construction stage in a construction stage analysis are converted into Initial Force for Geometric Stiffness to reflect the forces into the geometric stiffness of the structure at the post construction (Post CS) stage. Converted member forces of the last construction stage are shown in the main menu, Load > Initial Forces > Small Displacement > Initial Element Forces(CS) table and reflected in the analysis at Post CS. This functionality will become quite useful when a forward analysis is carried out for a suspension or cable stayed bridge and the cable tensions at the last step are used as Initial Force for Geometric Stiffness.
If both Initial Element Forces table and Initial Element Forces(CS) table are entered, Initial Element Forces table directly entered by the user will be applied first in priority. However, if Apply Initial Member Force to C.S. is checked on, (Initial Element Forces(CS)) at the last step of the last construction stage will be applied to the Post CS stage.
Truss: Applicable for Truss and Cable elements (When Include Nonlinear Analysis option is activated)
Beam: Applicable for Beam elements
Change Cable Element to Equivalent Truss Element for PostCS
Load cases considered at post construction stage (Post CS or Completed stage) in cable stayed bridge or suspension bridge analysis include linear static load cases (ST), moving load cases (MV), settlement load cases (SM) and response spectrum load cases (RS). In moving load analysis, cable elements are automatically considered as truss elements. On the other hand, linear static analysis reflects true stiffness of cable elements. As such, it is not correct to linearly combine the analysis results obtained by different stiffnesses for the same elements. This function applies the same cable element stiffness to all the load cases acting in Post CS.
Check on: Equivalent cable element stiffness is calculated using the tensions in the cable elements at the last construction stage. The equivalent stiffness is then used to analyze all the load cases in Post CS. Change in stiffness due to changes in tensions in the cable elements is not recalculated for linear load combination. By checking this function, the same stiffness can be applied to various load cases at Post CS.
Check off: Different stiffnesses are applied to each load case as below.
Apply Initial Member Force to C.S. :
Apply initial forces entered in the Initial Element Forces table to member forces for construction stages. The initial forces are applied to a specific construction stage at which the corresponding elements are first activated. This function is useful when we perform construction stage analysis from a specific construction stage by considering the member forces of the preceding construction stage as initial forces. Initial forces entered during construction stages will not be reflected in the geometric stiffness.
Initial Tangent Displacement for Erected Structures
This function calculates real displacements of the elements, which will be created in the next stage, considering the rotational angles of nodes resulting from each current construction stage. This functionality is used for fabrication cambers for structural steel and precast concrete members.
All: Calculate real displacements for all members.
Group: Calculate real displacements for specific groups.
Lack-of-Fit Force Control
In forward construction stage analysis of a cable stay bridge, the Lack-of-Fit Force plus the pretension obtained from the initial state analysis is applied as pretension in construction stages. This results in the tension forces of the initial state analysis at the final stage without having to analyze backward analysis.
A typical cable stay bridge consists of 3 spans. Such cable stay bridge includes Key Segment closure. Just prior to placing the Key Seg closure, the elements at each end of the Key Seg closure exhibit deflections. Placing the Key Seg in the deflected structure will result in discontinuous deflection and deflected angles, which in turn results in incorrect analysis after the connection, compared to the results of the initial state analysis. For correct analysis. forced displacements at each end of the Key Seg are calculated and then converted into equivalent member forces, which are then applied to the Key Seg at the time of placing the Key Seg. This then leads to the same results at the last stage after connection as that of the initial state analysis. The forced displacements (equivalent forces) applied to the Key Seg are also referred to as Lack-of-Fit Force. This process enables us to perform forward analysis without resorting to finding pretension forces in cables through backward analysis
In order to calculate Lack-of-Fit Force, we need to define a Structure Group for the truss and beam elements for which Lack-of-Fit force will be calculated. We then check on the Lack-of-Fit Force Control and select the Structure Group defined earlier from the combo box.
The results such as member forces or nodal displacements used in calculating Lack-of-Fit force can be checked from Result>Result Tables>Construction Stage>Lack of Fit Force>Beam or Truss.
When we apply Lack-of-Fit Force to all the cable and Key Seg elements in general cable stayed bridge analysis, we can omit the process of calculating the cable tension forces during construction, and forward analysis alone enables us to design a cable stayed bridge.
2. Lack of Fit Force option must be used with Internal Force type under Cable Pretension Force Control function. Cable-Pretension Force Control function is used to control Cable-Pretension for construction stage analysis of a cable stayed bridge. In general, due to force redistribution the resultant cable forces differ from the Pretension Loads entered. External Force type is selected when the user directly enters cable pretension. In that case the program does not change the cable force values and use the user defined values. Hence in order to use pretension obtained from the completed state, select Internal Force type and Lack-of-Fit Force Control to automatically calculate pretension for each stage.
Consider Stress Decrease at Lead Zone by Post-tension
Select a method of computing stresses over a transfer length in a post-tension model. This feature is applicable only when a Transfer Length is entered in the Tendon Profile dialog.
Linear Interpolation: Linearly interpolate stresses from end anchorage zone to stress-free zone
Constant: Stress* : Stresses over a stress-free zone are computed by multiplying stresses, without considering a Transfer Length, by a constant ratio. For example, enter 0.5 to use 50% of stress for the stress over a stress-free zone.
If "Composite Section for Construction Stage" is used, this function cannot be applied.
Beam Section Property Changes
Select whether to consider the presence of tendons for calculating section properties.
Constant: Do not consider the effect of tendon for calculating section properties.
Change with Tendon: Calculate section properties considering the effect of tendons. In case of post-tension, use a net section with duct areas excluded before grouting, and use a transformed section with duct areas included after grouting.
Calculate Concurrent Forces of Frame: corresponding force components of elements during construction stages. When a max or min value of a particular force component (say strong axis moment) is found, the corresponding other force components (say shear and axial forces) are also calculated.
Calculate Output of Each Part of Composite Section: Check on to calculate stresses and forces pertaining to each of the concrete deck part and the girder part. Otherwise, output will be produced for the total composite section.
Self-Constrained Forces & Stresses: Check on to calculate self-restraint forces and stresses due to creep, shrinkage and temperature gradient pertaining to each of the concrete deck part and the girder part. In steel-concrete composite beams, due to compatibility conditions, creep and shrinkage of concrete part of the cross-section (concrete slab) results in a redistribution of stresses. When deformation of shortening happens in the concrete part, the steel part of the cross-section prevents free deformation of concrete. As a result of restrained deformation, tensile stresses appear in concrete slab, Due to equilibrium, compressive stresses in the steel part of cross-section appear as well. Also, these self-restraint stresses of composite sections can occur due to nonlinear temperature gradient in the cross-section. These self-restraint stresses of composite sections can be checked in the Results > Result Tables > Composite Section for C.S. > Self-Constraint Force & Stress.
Remove the conditions for a construction stage analysis. The construction stage analysis is not performed in this case.
Tendon Primary represents member forces caused by Tendon Prestress forces. Tendon Secondary represents member forces resulting from Tendon Prestress forces acting in an indeterminate structure. To check analysis results, Primary and Secondary can be regarded as internal forces and external forces respectively. For design, however, the program internally recalculates member forces due to Primary considering the translation of neutral axis so as to use them as internal forces, and member forces due to Secondary are used as external forces.
Save Output of Current Stage
From V671, results for the current stage can be saved and printed. In the previous version, output was available only for accumulated forces and stresses.
Q1. There are construction stage load cases, namely, “creep primary”, “creep secondary”, “shrinkage primary” and “shrinkage secondary”. What are the meaning of “primary” and “secondary”, their differences and application?
A1. Tendon Primary represents member forces caused by Tendon Prestress forces. Tendon Secondary represents member forces resulting from Tendon Prestress forces acting in an indeterminate structure. To check analysis results, Primary and Secondary can be regarded as internal forces and external forces respectively. For design, however, the program internally recalculates member forces due to Primary considering the translation of neutral axis so as to use them as internal forces, and member forces due to Secondary are used as external forces.
Likewise in creep, we have both primary as well as secondary effects. Creep Primary Effects refers to deformation and forces required to cause creep strain. Whereas creep secondary refers to effects caused by creep in indeterminate structure.
Primary forces are the imaginary forces whereas, the secondary forces are the actual forces developing inside the member. So for design, only the consideration of secondary forces is adequate. But especially for shrinkage, there are few more considerations as discussed below. There are three effects of shrinkage in the steel composite girder as follows:
1. Auto-equilibrated stresses and an imposed rotation in a determinate structure.
2. Deflection due to the imposed deformation.
3. Member forces in a indeterminate structure.
Often, item 1 and 2 are denoted primary effects and item 3 secondary effects of shrinkage. In midas, the item 1 and 3 can be checked with CS: Shrinkage Secondary. The item 2 can be checked with CS: Shrinkage primary.
For the serviceability stress check, the item 1 and stresses caused by item 3 should be considered. For the ultimate limit state check, the item 3 should be considered. Since item 2 is not checked as per the code’s provisions, the auto generated load combinations in midas Civil do not include the Shrinkage primary.
Q3. Please give me your recommendation regarding the eigenvalue analysis of suspension bridge. How can I make eigenvalue analysis of suspension bridge taking into account both axial stiffness based on the Ernst equation (sagging effect) and geometrical stiffness in cable?
Eigenvalue analysis of a cable structure
For the calculation of accurate natural frequency of a cable structure, the following two things should be considered in the analysis.
- The effect of cable tension on the axial stiffness of cable by Ernst equation (horizontal direction in the verification example below)
- The effect of cable tension on the geometric stiffness of cable (vertical direction in the verification example below)
The natural frequency of single degree of freedom system is determined as the equation below.
The axial stiffness of truss element is determined as below.
k (truss) = EA/L
In order to calculate the axial stiffness of cable, first we calculate the equivalent modulus of elasticity using Ernst equation.
where E indicates the elastic modulus of the cable, L the horizontal projection length of the cable element, w the cable weight per unit length, A the cross-sectional area of the cable, and T the axial force of the cable element.
Then, the axial stiffness of cable can be determined as below. Refer to midas analysis manual.
The element stiffness matrix may be separated into an elastic part, kE, plus a geometric part, kG that accounts for the effects of finite deformation.
where the first matrix is the elastic stiffness matrix and the second matrix is the geometric element stiffness matrix. The approximation (T/L) = (T/Lo) is sufficiently accurate in most applications.
How Ernst equation and Geometric stiffness can be taken into account for the eigenvalue analysis?
1) Ernst equation
Use cable element type.
Create construction stage model.
Check on the 'Change Cable Element to Equivalent Truss Element for PostCS' option in the 'Construction Stage Analysis Control Data' dialog as below.
2) Geometric stiffness
Check on the 'Convert Final Stage Member Forces to Initial Forces for PostCS' option in the 'Construction Stage Analysis Control Data' dialog as below.
Perform eigenvalue analysis.
Title: Eigenvalue analysis of a cable
Description: Obtain natural frequencies of vibration of a cable in the horizontal and vertical direction.
Structural geometry and analysis model
Analysis type: 2D eigenvalue analysis (X-Z plane)
Unit system: m, kN
Dimension: Length = 5 m
Element: Cable element
Modulus of elasticity: E = 2.10 x 108 kN/m2
Poisson's ratio: ν = 0.3
Area: A = 0.001963 m2
Node 1: Restrain DX, DY & DZ
Node 2: Negligible stiffness in the Z-axis (or vertical direction) in order to avoid singular condition.
A concentrated load, 10 kN is applied to the node 2 in the (+)X direction.
This load will generate cable tension of 10 kN.
MX = 100 kN/(m/sec2)
MZ = 100 kN/(m/sec2)
Results: Eigenvalue analysis results
Mode shape (mode 1): Vertical vibration
Mode shape (mode 2): Horizontal vibration
Hand-calculation of frequency
Mode 1 (vertical vibration)
- Elastic stiffness = 0
- Geometric stiffness
Mode 2 (horizontal vibration)
Axial stiffness with equivalent modulus of elasticity
Equivalent modulus of elasticity (Ernst equation)
Comparison of results