To
enter new or additional time history analysis load cases
Click
.
To modify
previously entered time history analysis load cases
Select
a load case from the time history analysis load case list at the
bottom of the dialog box, then click and
modify the data entries.
To delete
previously entered time history analysis load cases
Select
a load case from the time history analysis load case list at the
bottom of the dialog box and click .
: Enter pertinent information for
eigenvalue analysis.
General
Name
Enter
the name of the time history analysis load case. The name is used
in "Combinations".
Description
State
a brief description related to the time history load case.
Analysis Type
Linear: Linear Time History
Analysis
Nonlinear: Nonlinear Time History
Analysis
Analysis Method
Modal: Modal Superposition Method
Direct Integration: Direct Integration
Method
Static: Static Analysis. Pushover
Analysis is possible by combining with Nonlinear from Analysis
Type.
Note
Combination
of Nonlinear Analysis and Static Analysis is equivalent to performing
Pushover Analysis.
Time History Type
Transient: Time history analysis
is carried out on the basis of loading a time load function only
once. This is a common type for time history analysis of earthquake
loads.
Periodic: Time history analysis
on the basis of repeatedly loading a time load function, which
has a period identical to End Time. This type is applicable for
machine vibration loads.
Geometric Nonlinearity
Type
Select Large Displacement to consider
the geometric nonlinear effect due to large displacement in Time
History Analysis. This option is valid only when Analysis Type
is "Nonlinear" and Analysis Method is "Direct Integration"
or "Static".
End of Time
The
finish time until which the time history analysis is required
[Second]
Note
If
the Time History Type is Transient, the analysis will be performed
until the specified End Time. If the Time History Type is Periodic,
the analysis will be repeated on the basis of the period identical
to the End Time.
Time Increment
The
time increment of a time history analysis significantly affects
the accuracy of the analysis results. A common rule of thumb for
determining the time increment is to use at least 1/10 of the
smaller of the period of the time forcing function or the natural
frequency of the structure. [Second]
Incremental Step (Activates
only for the Nonlinear Static Analysis)
Enter
the incremental steps until which the load will be incrementally
applied to the structure. For example, if the number of incremental
steps and the total load are 100 and 100 ton respectively in nonlinear
static analysis, the load increases by 1 ton, and analysis is
carried out for each step.
Step Number Increment for Output
Analysis
time step required for producing results of the time history analysis.
Results
produced at the interval of (Number
of Output Steps x Time Increment).
Order
in Sequential Loading
Data
related to a sequence of consecutively loaded multiple time history
analysis conditions are entered here.
Subsequent to
Select
a time history analysis condition previously defined, which precedes
the time history analysis condition currently being defined. The
Analysis Type and Analysis Method for the current time history
analysis condition must be consistent with those for the preceding
load condition. From the preceding analysis condition, displacement,
velocity, acceleration, member forces, variables for the state
of hinges and variables for the state of nonlinear link elements
are obtained and used as the initial condition for analysis. However,
in the case of loadings, the loading at the final state of the
preceding analysis condition is assumed to constantly remain in
the current analysis condition only when "Keep Final Step
Constantly" is checked on.
Load Case: Select a preceding
load case. In addition to the time history load (TH), the static
load (ST) and the construction stage load (CS) can be also considered.
It is not necessary to change a static load such as self weight
to a time history load. A static load case can be directly selected.
Initial Element Forces (Table):
It considers the equilibrium element forces due do the preceding
load case. If a preceding load is applied from Load Case, it is
limited to a load in the same structural system.
However,
using Initial Element Forces (Table), it is possible to apply
a preceding load to a structure whose boundary conditions change
such as in earthquake analysis. The preceding load case can be
in the form of equilibrium forces.
Note
This function considers Initial Element
Forces entered in Loads>Initial Forces>Small Displacement>Initial Element Force
Table as the preceding load case.
The
preceding load case of static load, construction stage load, and
equilibrium element forces do not support the fiber element. It
is recommended that the member forces due to the preceding load
case be kept in the elastic range. It may result in an inappropriate
outcome beyond the elastic range.
Cumulative D/V/A Result: The
displacement, velocity and acceleration results of a preceding
load case are produced cumulatively. This does not affect the
analysis itself. It is only applicable for a time history analysis
load (TH).
Keep Final Step Loads Constant
: The final step loads of the preceding load case are maintained.
It is only applicable for a time history analysis load (TH).
Damping
Direct Specification of Modal Damping:
Specify damping ratio for each mode directly.
Damping Ratio for All Modes:
It applies to all modes except for the modes for which the user
has directly specified modal damping ratios. It applies to all
the modes other than the damping ratios assigned to specific modes
in the Modal Damping Overrides table below. In a modal analysis,
if the entered damping ratio is different from the damping ratio
the user specified in Response Spectrum Functions, the previous
spectrum data will be adjusted and used in analysis based on this
damping ratio entered here.
Modal Damping Overrides: User
directly defines damping ratios by modes.
Mode : Mode Number
Damping Ratio
Damping Type: Check whether
or not the damping matrix type is proportional to mass and/or
stiffness.
Direct Specification: Enter
the damping coefficients for the Damping Types checked on.
Calculate from Modal Damping:
The proportional coefficients are calculated from the user defined
modal damping ratios and automatically entered.
Coefficients Calculation from Modal
Damping: Depending on the checked Type of Proportional
Damping, one modal damping coefficient can be defined if it is
proportional to either mass or stiffness, and two modal damping
coefficients can be defined if it is proportional to both.
Frequency: Specify modal frequencies
for which the damping ratios will be defined, which will be used
to calculate the proportional coefficients.
Period: Specify modal periods
for which the damping ratios will be defined, which will be used
to calculate the proportional coefficients.
Damping Ratio: Specify the damping
ratios corresponding to the specified Frequencies or Periods.
: Damping Ratio calculator
dialog box is activated, which calculates and shows the modal
damping ratio having a specific frequency or period from the entered
proportional coefficients. Damping ratios are defined for a maximum
of two modes when damping proportional to mass and stiffness is
used. This function allows us to simply calculate the magnitudes
of damping ratios for the remaining modes.
Note
This function is not used to additionally specify the damping ratio
of a specific mode.
Damping ratios for each mode
are automatically calculated using the damping ratios specified
for element groups and boundary groups in Group
Damping, which are used to formulate the damping matrix. Therefore,
in the case of Strain Energy Proportional, it is necessary to
directly input damping ratios by element groups and boundary groups
in Group Damping. Strain Energy Proportional can be used in Modal
Analysis Method and Direct Integration Method.
Rayleigh
damping for each element is calculated using damping ratios specified
for element groups and boundary groups in Group Damping. Element
Mass & Stiffness Proportional Damping can be applied to specific
elements and boundaries, which can be applied to cases where different
materials with different damping exist or damping and base isolator
devices exist in a structure. Where groups are defined for elements
and assigned damping ratios for each group, and analysis is carried
out by modal superposition, modal damping ratios founded on Group
Damping can be checked from the Modal
Damping Ratio based on Group Damping after the analysis.
Note
Significant unbalanced equilibrium forces may result in Direct
Modal and Strain Energy Proportional due to the damping characteristics.
As such, it is recommended to go through convergence calculation
if Direct Modal and Strain Energy Proportional are selected.
Static Loading Control [Active only for Nonlinear Static Analysis]
The
program provides two control methods. Load Control Method increases
loads by steps until the final load is reached and analyzes each
step. Displacement Control Method increases displacements by steps
until the target displacement is reached and analyzes each step.
Load Control
Scale Factor:
Scale factor for loads used in Nonlinear Static Analysis
Displacement Control
Global Control:
It terminates the analysis when the maximum displacement of the
structure reaches the maximum translational displacement specified
by the user.
Maximum Translational Displacement: Specify a Maximum Translational
Displacement.
Master Node Control: It terminates the analysis when
the user-specified displacement of the Master Node reaches the
maximum displacement.
Master Node:
Specify the Master Node.
Master Direction:
Specify the direction of the maximum displacement control for
the Master Node.
Maximum Displacement: Enter the maximum displacement
for the Master Node.
Note
Caution should be exercised if nonlinear analysis is consecutively
performed because the control method of the nonlinear analysis
and the sequence of use affect the analysis results.
1. Load Control --> Displacement
Control
2. Load Control --> Displacement Control --> Displacement
Control
3. Displacement Control --> Load Control
4. Load Control --> Load Control
Correct results can be obtained
from Case 1 and 2, but Case 3 and 4 may result in inappropriate
outcomes.
Time Integration Parameters
Newmark Method: Newmark Method
is used to numerically integrate kinetic equations in the direct
integration method. The related parameters, Gamma and Beta are
entered. Three methods exist for input. Among them, Constant Acceleration
is recommended, which always results in stable analysis.
Constant Acceleration: It is
assumed that the acceleration of a structure remains unchanged
during the time interval of each Time Step. The corresponding
Gamma (=1/2) and Beta (=1/4) are automatically entered. Based
on this assumption, divergence of analysis results can be prevented
irrespective of the value of Time Increment in the analysis of
direct Integration.
Linear Acceleration: It is assumed
that the acceleration of a structure varies linearly during the
time interval of each Time Step. The corresponding Gamma (=1/2)
and Beta (=1/6) are automatically entered. Based on this assumption,
the analysis results may become unstable in the analysis of direct
Integration when the value of Time Increment is bigger than 0.551
times the shortest period of the structure.
User Input: User directly enters
the values of Gamma and Beta.
Nonlinear Analysis
Control Parameters
Enter
the parameters necessary for nonlinear analysis when Nonlinear
is selected in Analysis Type.
If Modal is selected
Perform Iteration: It performs
convergence calculation by the Newton Raphson method.
Iteration Controls: Specify
an Iteration Control method that determines the accuracy and convergence
of a solution for nonlinear analysis.
Iteration Parameters: Specify
Iteration Parameters that determine the accuracy and convergence
of a solution for nonlinear analysis.
Permit Convergence Failure:
It becomes inactivated for Nonlinear-Static Analysis.
Minimum Step Size: It is a Minimum
value for Sub-steps, which are segmented from each analysis Time
Step. If convergence calculation by the Newton Raphson method
is used, but does not satisfy the Convergence Criteria even after
reaching the maximum number of iterations, it automatically divides
the time step into smaller sub-steps. The Minimum Sub-step Size
limits the time interval between the sub-steps.
Maximum Iteration: The maximum
number of iterations per each Sub-step for analysis. If Modal
is selected in Analysis Method, Fast Nonlinear Analysis Algorithm
developed by E. L. Wilson is used for iterative analysis. If Direct
Integration is selected, the Newton Raphson iterative method is
used. The maximum number of iterations is recommended to be less
than 10. A large value may lead to a long analysis time.
Convergence Criteria: Define
the convergence criteria for nonlinear time history analysis.
midas
Civil provides Displacement Norm, Force Norm and Energy Norm,
which are used for the acceptance criteria for convergence in
the iterative analysis process. Multiple norms can be selected.
When the modal superposition method is used, Displacement Norm
and Force Norm can be applied. For the direct integration method,
all the 3 Norms can be used.
Use
Line Search Method:
This feature introduces line
search to the Newton-Raphson algorithm
to solve the nonlinear residual equation. Line search increases
the effectiveness of the Newton method when convergence is slow
due to roughness of the residual.
This
feature is helpful for problems with flexible structures, where
the stiffness increases with the load, or if the nonlinear analysis
solution converges while vibrating. It may only increase the analysis
time when used on an ineffective problem.
Number
of Iterations to Start Line Search:
Input
the maximum number of line search per repeated calculation.
Boundary Nonlinear Analysis:
Specify a convergence method that determines the accuracy and
convergence of a solution for boundary nonlinear analysis.
Runge Kutta Method: Expand the
increment time in a Taylor series to solve the differential equations.
Fehlberg Method (Stepsize
sub-division for Non-convergence Control)
Cash-Karp Method (Adaptive
Stepsize Control)
If
Direct Integration is selected
Perform Iteration: It performs convergence calculations
by the Newton Raphson method.
Damping Matrix Update: When
Direct Integration is used in nonlinear time history analysis,
check whether to continuously update the element damping matrix
based on the change in stiffness. If it is unchecked, the initial
stiffness of the elastic state is used for the element damping
matrix. If it is checked on, the element damping matrix is calculated
using the presently modified stiffness. This menu only activates
for Mass and Stiffness Proportional and Element Mass & Stiffness
Proportional.
Iteration Controls: Specify
an Iteration Control method that determines the accuracy and convergence
of a solution for nonlinear analysis.
Iteration Parameters: Specify
Iteration Parameters that determine the accuracy and convergence
of a solution for nonlinear analysis.
Permit Convergence Failure:
When Displacement/Force/Energy diverges between the Steps specified
by the user, midas Civil automatically divides the steps and reanalyzes
the model. If divergence still continues, the analysis proceeds
unconverged to the next step if Permit Convergence Failure is
checked on. Analysis results may contain some margin of
error, but the unconverged results still may be helpful to understand
the approximate behavior of the overall structure or to identify
the cause of such divergence. Results obtained using this option
can be unconverged, especially when the change of stiffness is
significant due to nonlinear behavior. The time step should be
reduced in such cases.
Minimum Step Size: It is the
Minimum value for Sub-steps that are segmented from each analysis
Time Step. If the convergence calculation by Newton Raphson method
is used, but does not satisfy the Convergence Criteria even after
reaching the maximum number of iterations, it automatically divides
the time step into smaller sub-steps. The Minimum Sub-step Size
limits the time interval between the sub-steps.
Maximum Iteration: It is the
maximum number of iterations per each Sub-step for analysis. If
Modal is selected in the Analysis Method, Fast Nonlinear Analysis
Algorithm developed by E. L. Wilson is used for iterative analysis.
If Direct Integration is selected, the Newton Raphson iterative
method is used. The maximum number of iterations is recommended
to be less than 10. If the number of iterations is large, considerable
time may be required for analysis.
Convergence Criteria: Define
the convergence criteria for nonlinear time history analysis.
midas
Civil provides Displacement Norm, Force Norm and Energy Norm,
which are used for the acceptance criteria for convergence in
the iterative analysis process. Multiple norms can be selected.
When the modal superposition method is used, Displacement Norm
and Force Norm can be applied. For the direct integration method,
all the 3 Norms can be used.
Boundary Nonlinear Analysis:
Specify a convergence method that determines the accuracy and
convergence of a solution for boundary nonlinear analysis.
Runge Kutta Method: Expand the
increment time in a Taylor series to solve differential equations.
Fehlberg
Method (Stepsize sub-division for Non-convergence Control)
Cash-Karp Method (Adaptive
Stepsize Control)
If Static
is selected
Perform
Iteration: It performs convergence
calculations by the Newton Raphson method.
Iteration
Controls: Specify an Iteration
Control method that determines the accuracy and convergence of
a solution for nonlinear analysis.
Iteration
Parameters: Specify Iteration Parameters that determine
the accuracy and convergence of a solution for nonlinear analysis.
Permit
Convergence Failure: When Displacement/Force/Energy diverges
between the Steps specified by the user, midas Civil automatically
divides the steps and reanalyzes the model. If divergence
still persists, the analysis proceeds unconverged to the next
step if Permit Convergence Failure is checked on. Analysis
results may contain some margin of error, but the unconverged
results still may be helpful to understand the approximate behavior
of the overall structure or to identify the cause of such divergence.
Results obtained using this option can be unconverged, especially
when the change of stiffness is significant due to nonlinear behaviors.
The time step should be reduced in such cases.
Max.
Number of Substeps:
Maximum
Iteration: It is the maximum number of iterations per each
Sub-step for analysis. If Modal is selected in Analysis Method,
Fast Nonlinear Analysis Algorithm developed by E. L. Wilson is
used for iterative analysis. If Direct Integration is selected,
the Newton Raphson iterative method is used. The maximum number
of iterations is recommended to be less than 10. If the number
of iterations is large, considerable time may be required for
analysis.
Convergence
Criteria: Define the convergence criteria for nonlinear
time history analysis.
midas Civil provides Displacement
Norm, Force Norm and Energy Norm, which are used for the acceptance
criteria for convergence in the iterative analysis process. Multiple
norms can be selected. When the modal superposition method is
used, Displacement Norm and Force Norm can be applied. For the
direct integration method, all the 3 Norms can be used.
Boundary
Nonlinear Analysis: Specify a convergence method that determines
the accuracy and convergence of a solution for boundary nonlinear
analysis.
Runge
Kutta Method: Expand the increment time in a Taylor series
to solve differential equations.
Fehlberg
Method (Stepsize sub-division for Non-convergence Control)
Cash-Karp
Method (Adaptive Stepsize Control)
Note 1
In order to carry out a time history analysis, the required data
related to Eigenvalue analysis or Ritz vector analysis must be
entered in Eigenvalue
Analysis Control. In the case of Eigenvalue analysis, the
number of eigenvalues, the range of natural frequencies to be
considered, the maximum number of repetitions for the eigenvalue
calculation, the subspace dimension, the convergence tolerance,
the Frequency Shift for a rigid body motion, etc. must be entered.
In the case of Ritz Vector analysis, specify the starting load
vectors and the number of Ritz Vectors to be generated for each
starting load vector.
Note 2
During
Nonlinear Static or Nonlinear Time History Analyses, the section
can completely fail upon reaching the ultimate state. This is
because all the tension rebars yield or the concrete in the compression
zone is rapidly transferred to the Softening state having a negative
modulus of elasticity. |