The nonlinear response simulation of RC structures is the power point of COM3 calculations. The nonlinear parts have to be divided and meshed finely to present the complex nonlinear performance of RC materials. However if too fine elements are divided, the consuming time will increase sharply while the result precision is kept unchanged. This is not hoped.

The general dividing number in the possible plastic hinge parts based on our test is suggested to use two fiber elements and their length is the half of cross section effective height. The following figure shows the dividing number and their corresponding displacement results.

Two fiber elements using for plastic hinge parts are just for general recommendation. For a specific column or beam, the fiber element number can adjusted according to the section shape, reinforcement ratio and load strength.

The parts of RC components that do not enter plastic field suffer some simple strain-stress variety. The fiber element can be taken longer and the analysis time can be saved too. But over rough division of beam or column will result in an error in non-axial elastic bending deformation. Therefore here the plastic hinge length is suggested to use. Like plastic hinge parts, this length is affected by the section shape, reinforcement ratio and load strength. For a real model, a appropriate adjustment is needed.

For a pier bridge, the hinge part will appear at the base part of pier column
For Rahman structure bridges, the hinge parts will appear at the upper and lower parts of column.
For beams, the hinge parts will appear at the two side.

By the Road and Bridge CODE of Japan Road Association, the plastic length isonly for
in which,

	D	: Scale of section( diameter for circle section, the scale length in the acting direction for the rectangular section)
	h	: Height from foot base side of bridge to the inertia acting position on upper structure.

The plastic length in the Railway Structural Design Standard is expressed as

Due to the difference between the real structure and analysis model, the hinge location and length are some different from above definition. It is suggested that the static preliminary analysis be conducted before a formal analysis.

In general, the plastic response will not appear in the cross part between beams and columns as figure below. Therefore it should use non failure section check in the Section Material Editor window for these parts. The non failure section fiber element will behavior with an elastic constitutive law and the plastic non-linearity will not happen. The section can take as simple as possible.

For avoiding the redefinition of weight in the corner parts, it should define a part of fiber elements in the cross field to have a zero weight. The zero weight can be defined by inputting zero unit weight in Cell Material tab of Section Material Editor windows under the following window.

For Static Analysis, there are Displacement-controlled analysis and Load-controlled analysis. For the model with fewer statically unbalanced dimensions, the stability of Load-controlled analysis would be worse. In that case, the alterations are effective to reset the increased unit-load less or change to the Displacement-controlled analysis.

At the case that the observed earthquake waves are applied as the input wave loads, it is recommended that the main part of them (several seconds) are taken out for the analysis. When the input wave loads are composed of the combination of SIN waves, it may be better to make a few large waves continuously than multiple small waves continuously.

It is also effective to define the input wave period closer to the natural period of the structures. To make the execution time shorter, it is more effective to reduce the total analysis steps than reset the input waves to only one direction from three directions simultaneously. In order to calculate up to the last step with keeping the good accuracy of the convergent analysis, it is efficiently to set the time interval of the input wave by 0.02 second at first and reset it smaller by 0.01 second and 0.005 second in order at the case when the solution might be diverged.

In the load type definition, three kinds of load, Dead Weight, Static and Dynamic, are included.
To the load type combination, each three kinds of load can be calculated independently. And also the combination of loads is possible, Dead Weight + Static, Dead Weight + Dynamic, Dead Weight + Static + Dynamic and Static + Dynamic. The result of the former loading analysis is transmitted to the next loading analysis. In this case, analysis order is set by Dead Weight, Static and finally Dynamic. So, it is not allowed to load Static after Dynamic

Dead Weight Analysis is performed with loading the gravity weight to Vertical direction (Y-direction).

For Static Analysis, many loading patterns are registered in the program. By composing these loading patterns, you can define your own loading pattern. Displacement control and Load control are available.

[Note for Displacement control analysis]
For the analysis by Displacement controlled loading, it is necessary to restrict the boundary condition in the loading direction at the loading node. For example, the vertical direction of the loading node would be restricted when Beam element is loaded in vertical direction by displacement control. In this case, the result of the displacement only by the self-weight of the structure cannot be obtained because of the restriction in vertical direction. In the same way, the horizontal direction of the loading node would be restricted when Column element is loaded in horizontal direction by displacement control. At this time, the correct results cannot be obtained even if Dynamic analysis is executed after Static analysis because of the restriction in horizontal

Dynamic analysis is executed with defined acceleration waves.
The acceleration waves are loaded at the restricted node in all six degrees. Then, the loaded nodes should be restricted in all six degrees even at the case of the loading in only X-direction.
The correct results cannot be obtained even if Dynamic analysis is executed after Static analysis by Displacement controlled loading. When the dynamic analysis has to be executed after Static loading, Static loading by Load control should be carried out.

The input dynamic waves can be generated by tool menu of program or use a real time-history record. The waves generated by tool menu can be used to test structure dynamic properties.
The real time-history record is used to check the safety of structure. For a specific record, many information is included such as earthquake strength, seismic fault, seismic wave propagating routine and the local field properties. When the record is selected, the location and surround geological characteristics of project have been taken into account. Its frequency content and peak value will influence the response of structures. The simulated record form a characteristic response spectrum can also be used for anti-seismic investigation too.

The input direction of record must be justified for a most dangerous input. For a bridge, the bridge axial direction and its normal direction is considered for the Due to the stochastic characteristics of earthquake records, more than one record with the same magnitude and prominent frequency are suggest to be used to calculate. The average results can be taken into the project check.

The three items on safety should be investigated for the structures under/after the earthquake action.

1) Bending Capacity Check and Shear Capacity Check
The failure mode is firstly judged and then the acting bending moment or acting shear force is compared with sectional bending moment capacity or shear force capacity. For example, a judgment procedure is given as below.

1. Failure Mode Judgment
   (V·a)/Mu > 1.0 Bending Failure Mode
   (V·a)/Mu < 1.0 Shear Failure Mode
   (V: shear force capacity, a: shear span length, Mu: bending moment capacity)
2. Bending Failure Mode
   M/Mu<1.0
   (M: acting bending moment)
3. Shear Failure Mode
   S/V<1.0
   (S: acting shear force)

*For COM3(Fiber), the item of Failure Mode Judgment is not conducted. But the check b) is carried out regardless of the its possible failure mode and its results with step is shown in the Fiber Results (gauss point) window. The Shear Failure is not checked, but the S and V values is steppedly listed in the table according to the computation.

2) Damage judgment
The definition of damage criteria of structures depends on artificial settings for the calculating value. Not only the project cost and importance but also the respair/retrofitting cost affected the criteria level. The strain of steel and concrete is used in the COM3(Fiber) to define the model damage criteria.

3) Residual displacements
The Residual displacement must to be checked for a load action, especially for the earthquake action. The safe residual displacement is needed to keep under certain level. The Road and Bridge Code of Japan Road Association , for example, set a following criteria for the B type bridge( an important type).

in which,
: Residual Displacement
: Permitted residual displacement, the 1/100 height from the down side of pier to the acting position of inertia forces.

The anti-seismic investigation must be conducted for the more than one wave. The spectrum of input waves must have the frequency characteristics of local fields. The Road and Bridge Code of Japan Road Association suggests 3 waves at least to input, The average result of calculation is used to final judgment.

It should be taken care that the calculated results (section forces, strain and stress) be not saved if the boxes in the fiber section definition are not checked. By default these boxes are not checked. But the parts like the base plastic hinge parts of columns have to be checked. Therefore the responses of the nodes such as accelerations, displacements and reactions are saved regardless of these checks.

These check boxes are set for reducing the result file size. If all the gauss point sections and cells are checked, the size of the result files will reach hundreds of MB. In addition, the time for reading them will last much long.

The analyzing time firstly depends on the size of the model and nonlinear performance of materials in the analysis will increase the time. It is suggested that other applications be stopped when the calculation is being conducted. The size of samples and their analyzing time can give you some implication on this respect as below.

TABLE The Relationship of Model File Size and Calculation Time
( Computer : Pentium III 800MHz, Memory 256 MB )

a	Calculation Time	Step Number	Node Number	File Size
Sample1	About 2 Min.	Static 315	11	7MB
Sample2	About 7Min.	Static 425	19	14MB
Sample3	About 20 Min.	Dynamic 250	85	40MB
Sample4	About 2.5 Min.	Dynamic 250	264	86MB

The values of Maximum iteration and Convergence order in the Analysis Model Setting are suggested to use the default values. The default values are

	Maximum iteration.....12
	Convergence order.....1%

If the default values cannot assure the successful calculation, one or both of two values can be modified to make the calculation re-execute until a successful calculation is finished. But this may result in a longer computing time.

The node number of iso-solid elements can be taken as 20 or 8 in general. But in our program the 8 node element is employed by considering computer property. But it should be noted that the middle nodes at the edge of solid cube are set for editing models. In fact these nodes are not used for calculation and therefore they cannot be defined for boundary conditions and the loads.

The Iso-solid elements are suggested to use in the model that the Fiber elements are difficult to model the component of structures like the top floor plates of Sample 4. However it should be paid attention for defining the intersecting parts between the Iso-solid element and fiber elements. An example is shown in the following figure. The spinning of iso-solid components around the bridge pier axis will become free. If these parts are modeled by the Fiber elements, the fiber section can be defined as 'Non failure'.


Notice:
The strength of Iso-solid elements should be set large enough to keep them response in the elastic range and not reach the fracture. The setting of the strength input box is for the future vision.