Inelastic Plane Frame

Nonlinear analysis of a concrete portal frame.

This set of examples investigates the nonlinear analysis of a reinforced concrete frame. The nonlinear beam column element with a fiber discretization of the cross section is used in the model.

Model Building  

The function create_portal creates a model representing the portal frame in the figure above. The model consists of four nodes, two nonlinear beam-column elements modeling the columns and an elastic beam element to model the girder. For the column elements a section, identical to the section used in Example 2, is created using steel and concrete fibers.

1. Begin with nodes and boundary conditions

   # create ModelBuilder (with two-dimensions and 3 DOF/node)
   model = ops.Model(ndm=2, ndf=3)
   
   # Create nodes
   # ------------
   model.node(1, (0.0,      0.0))
   model.node(2, (width,    0.0))
   model.node(3, (0.0,   height))
   model.node(4, (width, height))
   
   # set the boundary conditions - command: fix nodeID uxRestrnt? uyRestrnt? rzRestrnt?
   model.fix(1, (1, 1, 1))
   model.fix(2, (1, 1, 1))

   set width    360
   set height   144
   
   model basic -ndm 2 -ndf 3
   # Create nodes
   #    tag        X       Y 
   node  1       0.0     0.0 
   node  2    $width     0.0 
   node  3       0.0 $height
   node  4    $width $height
   
   
   # Fix supports at base of columns
   #    tag   DX   DY   RZ
   fix   1     1    1    1
   fix   2     1    1    1

Materials  

#                                   tag  f'c    ec0    f'cu   ecu
# Core concrete (confined)
model.uniaxialMaterial("Concrete01", 1, -6.0, -0.004, -5.0, -0.014)
# Cover concrete (unconfined)
model.uniaxialMaterial("Concrete01", 2, -5.0, -0.002, -0.0, -0.006)


# Reinforcing steel 
fy =    60.0;      # Yield stress
E  = 30000.0;      # Young's modulus
#                                tag fy  E   b
model.uniaxialMaterial("Steel01", 3, fy, E, 0.01)

# Core concrete (confined)
#                           tag  f'c     ec0  f'cu        ecu
uniaxialMaterial Concrete01  1  -6.0  -0.004  -5.0     -0.014

# Cover concrete (unconfined)
uniaxialMaterial Concrete01  2  -5.0  -0.002   0.0     -0.006

# Reinforcing steel 
set fy 60.0;      # Yield stress
set E 30000.0;    # Young's modulus
#                        tag  fy E0    b
uniaxialMaterial Steel01  3  $fy $E 0.01

Sections  

Define a cross section for the columns, following the procedure from the moment-curvature example

# Define cross-section for nonlinear columns
# ------------------------------------------
# set some parameters
colWidth = 15.0
colDepth = 24.0
cover    =  1.5
As       =  0.6      # area of no. 7 bars

# some variables derived from the parameters
y1 = colDepth/2.0
z1 = colWidth/2.0

model.section("Fiber", 1)
# Add the concrete core fibers
model.patch("rect", 1, 10, 1, cover-y1, cover-z1, y1-cover, z1-cover, section=1)
# Add the concrete cover fibers (top, bottom, left, right)
model.patch("rect", 2, 10, 1, -y1, z1-cover, y1, z1, section=1)
model.patch("rect", 2, 10, 1, -y1, -z1, y1, cover-z1, section=1)
model.patch("rect", 2,  2, 1, -y1, cover-z1, cover-y1, z1-cover, section=1)
model.patch("rect", 2,  2, 1,  y1-cover, cover-z1, y1, z1-cover, section=1)
# Add the reinforcing fibers (left, middle, right, section=1)
model.layer("straight", 3, 3, As, y1-cover, z1-cover, y1-cover, cover-z1, section=1)
model.layer("straight", 3, 2, As,      0.0, z1-cover,      0.0, cover-z1, section=1)
model.layer("straight", 3, 3, As, cover-y1, z1-cover, cover-y1, cover-z1, section=1)

# Define cross-section for nonlinear columns
# ------------------------------------------

# set some parameters
set colWidth 15
set colDepth 24 

set cover  1.5
set As    0.60;     # area of no. 7 bars

# some variables derived from the parameters
set y1 [expr $colDepth/2.0]
set z1 [expr $colWidth/2.0]

section Fiber 1 {
    # Add the concrete core fibers
    patch rect 1 10 1 [expr $cover-$y1] [expr $cover-$z1] [expr $y1-$cover] [expr $z1-$cover]

    # Add the concrete cover fibers (top, bottom, left, right)
    patch rect 2 10 1  [expr -$y1] [expr $z1-$cover] $y1 $z1
    patch rect 2 10 1  [expr -$y1] [expr -$z1] $y1 [expr $cover-$z1]
    patch rect 2  2 1  [expr -$y1] [expr $cover-$z1] [expr $cover-$y1] [expr $z1-$cover]
    patch rect 2  2 1  [expr $y1-$cover] [expr $cover-$z1] $y1 [expr $z1-$cover]

    # Add the reinforcing fibers (left, middle, right)
    layer straight 3 3 $As [expr $y1-$cover] [expr $z1-$cover] [expr $y1-$cover] [expr $cover-$z1]
    layer straight 3 2 $As 0.0 [expr $z1-$cover] 0.0 [expr $cover-$z1]
    layer straight 3 3 $As [expr $cover-$y1] [expr $z1-$cover] [expr $cover-$y1] [expr $cover-$z1]
}

Gravity Analysis  

We now implement a function called gravity_analysis which takes the instance of Model returned by create_portal, and proceeds to impose gravity loads and perform a static analysis. Its use will look like:

# Create the model
model = create_portal()

# perform analysis under gravity loads
status = gravity_analysis(model)

create_portal;
gravity_analysis;

Inside the function, a single load pattern with a Linear time series is created and two vertical nodal loads are added acting at nodes 3 and 4:

...
model.pattern("Plain", 1, "Linear", load={
# nodeID  xForce yForce zMoment
     3:   [ 0.0,   -P,   0.0],
     4:   [ 0.0,   -P,   0.0]
})

# Create a Plain load pattern with a Linear TimeSeries
pattern Plain 1 "Linear" {
      # Create nodal loads at nodes 3 & 4
      #    nd    FX          FY  MZ 
      load  3   0.0  [expr -$P] 0.0
      load  4   0.0  [expr -$P] 0.0
}

The model contains material non-linearities, so a solution algorithm of type Newton is used.

model.algorithm("Newton")

algorithm Newton;

For this nonlinear problem, the gravity loads are applied incrementally until the full load is applied. To achieve this, a LoadControl integrator is used which advances the solution with an increment of 0.1 at each load step.

model.integrator("LoadControl", 0.1)

integrator LoadControl 0.1;

To achieve the full gravity load, 10 load steps are performed.

model.analyze(10)

analyze 10

At end of analysis, the state at nodes 3 and 4 is printed. The state of element 1 is also reported.

Pushover analysis  

After performing the gravity load analysis on the model, the time in the domain is reset to 0.0 and the current value of all loads acting are held constant. A new load pattern with a linear time series and horizontal loads acting at nodes 3 and 4 is then added to the model.

The static analysis used to perform the gravity load analysis is modified to use the DisplacementControl  integrator. At each new step in the analysis the integrator will determine the load increment necessary to increment the horizontal displacement at node 3 by 0.1 inches. 60 analysis steps are performed in this new analysis.

For this analysis the nodal displacements at node 3 will be stored in the variable u for post-processing.

At the end of the analysis, the state of node 3 is printed to the screen.

A plot of the load-displacement relationship at node 3 is shown in the figure below.

Dynamic Analysis  

The concrete frame which has undergone the gravity load analysis is now subjected to an earthquake load.

After performing the gravity load analysis, the time in the domain is reset to 0.0 and the time series for all active loads is set to constant. This prevents the gravity load from being scaled with each step of the dynamic analysis.

model.loadConst(time=0.0)

loadConst -time 0.0

Mass terms are added to nodes 3 and 4. A new uniform excitation load pattern is created. The excitation acts in the horizontal direction and reads the acceleration record and time interval from the file ARL360.g3. The file ARL360.g3 is created from the PEER Strong Motion Database  record ARL360.at2 using the Tcl procedure ReadSMDFile contained in the file ReadSMDFile.tcl.

The static analysis and its components are first deleted so that a new transient analysis procedure can be defined.

The integrator for this analysis will be of type Newmark with a $\gamma = 0.25$ and $\beta = 0.5$ .

The integrator will add some stiffness proportional damping to the system, the damping term will be based on the last committed stifness of the elements, i.e. $C = a_c K_{\text{commit}}$ with $a_c = 0.000625$ .

Once all the components of an analysis are defined, the Analysis object itself is created. For this problem a Transient analysis is used. 2000 time steps are performed with a time step of 0.01.

In addition to the transient analysis, two eigenvalue evaluations are performed. The first is performed after the gravity analysis and the second after the transient analysis.

For this analysis the nodal displacenments at Nodes 3 and 4 will be stored in the file nodeTransient.out for post-processing. In addition the section forces and deformations for the section at the base of column 1 will also be stored in two seperate files. The results of the eigenvalue analysis will be displayed on the screen.

The two eigenvalues for the eigenvalue analysis are printed to the terminal. The state of node 3 at the end of the analysis is also printed.

Element response quantities can be used to generate the moment-curvature time history of the base section of column 1 as shown below.

Summary  

Summarizing, we now have the following functions:

A complete analysis may look as follows:

def main():
    # Create the model
    model = create_portal()

    # perform analysis under gravity loads
    status = gravity_analysis(model)

    if status != ops.successful:
        print(f"Gravity analysis FAILED ({status = })\n")

    status = pushover_analysis(model)
    # Print a message to indicate if analysis successful or not
    if status != ops.successful:
        print(f"Pushover analysis FAILED ({status = })\n")

    # Print the state at node 3
    model.print("node", 3)

if __name__ == "__main__":
    main()