OpenSees Examples Manual Examples for OpenSeesPy

OpenSees Example 1a. 2D Elastic Cantilever Column -- Static Pushover

You can find the original Examples:
https://opensees.berkeley.edu/wiki/index.php/Examples_Manual
Original Examples by By Silvia Mazzoni & Frank McKenna, 2006, in Tcl
Converted to OpenSeesPy by SilviaMazzoni, 2020

Simulation Process

Each example script does the following:

A. Build the model

  1. model dimensions and degrees-of-freedom
  2. nodal coordinates
  3. nodal constraints -- boundary conditions
  4. nodal masses
  5. elements and element connectivity
  6. recorders for output

B. Define & apply gravity load

  1. nodal or element load
  2. static-analysis parameters (tolerances & load increments)
  3. analyze
  4. hold gravity loads constant
  5. reset time to zero

C. Define and apply lateral load

  • Time Series and Load Pattern (nodal loads for static analysis, support ground motion for earthquake)
  • lateral-analysis parameters (tolerances and displacement/time increments)
  • Static Lateral-Load Analysis

  • define the displacement increments and displacement path
  • Dynamic Lateral-Load Analysis

  • define the input motion and all associated parameters, such as scaling and input type
  • define analysis duration and time increment
  • define damping
  • analyze
  • Introductory Examples The objective of Example 1a and Example 1b is to give an overview of input-file format in OpenSees using simple scripts. These scripts do not take advantage of the Tcl scripting capabilities shown in the later examples. However, they do provide starting a place where the input file is similar to that of more familiar Finite-Element Analysis software. Subsequent examples should be used as the basis for user input files.

    OpenSees Example 1a. 2D Elastic Cantilever Column -- Static Pushover

    Introduction Example 1a is a simple model of an elastic cantilever column. Objectives of Example 1b

    - overview of basic OpenSees input structure<br>
    - coordinates, boundary conditions, element connectivity, nodal masses, nodal loads, etc.<br>
    - two-node, one element
    

    In [1]:
    ############################################################
    #  EXAMPLE: 
    #       pyEx1a.Canti2D.Push.tcl.py
    #          for OpenSeesPy
    #  --------------------------------------------------------#
    #  by: Silvia Mazzoni, 2020
    #       [email protected]
    ############################################################
    # This file was obtained from a conversion of the updated Tcl script
    ############################################################
    
    # configure Python workspace
    import openseespy.opensees as ops
    import eSEESminiPy
    import os
    import math
    import numpy as numpy
    import matplotlib.pyplot as plt
    ops.wipe()
    # --------------------------------------------------------------------------------------------------
    # Example 1. cantilever 2D
    # static pushover analysis with gravity.
    # all units are in kip, inch, second
    # elasticBeamColumn ELEMENT
    # Silvia Mazzoni and Frank McKenna, 2006
    #
    # ^Y
    # or
    # 2 __
    # or  |
    # or  |
    # or  |
    # (1) 36'
    # or  |
    # or  |
    # or  |
    # =1= ---- -------->X
    #
    
    # SET UP ----------------------------------------------------------------------------
    ops.wipe()     #  clear opensees model
    ops.model('basic','-ndm',2,'-ndf',3)     #  2 dimensions, 3 dof per node
    if not os.path.exists('Data'):
        os.mkdir('Data')
    
    # define GEOMETRY -------------------------------------------------------------
    # nodal coordinates:
    ops.node(1,0,0)     #  node , X Y
    ops.node(2,0,432)
    
    # Single point constraints -- Boundary Conditions
    ops.fix(1,1,1,1)     #  node DX DY RZ
    
    # nodal masses:
    ops.mass(2,5.18,0.,0.)     #  node , Mx My Mz, Mass=Weight/g.
    
    # Define ELEMENTS -------------------------------------------------------------
    # define geometric transformation: performs a linear geometric transformation of beam stiffness
    # and resisting force from the basic system to the global-coordinate system
    ops.geomTransf('Linear',1)     #  associate a tag to transformation
    
    # connectivity: (make A very large, 10e6 times its actual value)
    # element elasticBeamColumn eleTag iNode jNode A E Iz transfTag
    ops.element('elasticBeamColumn',1,1,2,3600000000,4227,1080000,1)     # element elasticBeamColumn 1 1 2 3600000000 4227 1080000 1;
    
    # Define RECORDERS -------------------------------------------------------------
    ops.recorder('Node','-file','Data/DFreeEx1aPush.out','-time','-node',2,'-dof',1,2,3,'disp')     #  displacements of free nodes
    ops.recorder('Node','-file','Data/DBaseEx1aPush.out','-time','-node',1,'-dof',1,2,3,'disp')     #  displacements of support nodes
    ops.recorder('Node','-file','Data/RBaseEx1aPush.out','-time','-node',1,'-dof',1,2,3,'reaction')     #  support reaction
    ops.recorder('Element','-file','Data/FColEx1aPush.out','-time','-ele',1,'globalForce')     #  element forces -- column
    ops.recorder('Element','-file','Data/DColEx1aPush.out','-time','-ele',1,'deformation')     #  element deformations -- column
    
    # define GRAVITY -------------------------------------------------------------
    ops.timeSeries('Linear',1)     # timeSeries Linear 1;
    # define Load Pattern
    ops.pattern('Plain',1,1) # 
    ops.load(2,0.,-2000.,0.)     #  node , FX FY MZ -- superstructure-weight
    
    ops.wipeAnalysis()     # adding this to clear Analysis module 
    ops.constraints('Plain')     #  how it handles boundary conditions
    ops.numberer('Plain')     #  renumber dofs to minimize band-width (optimization), if you want to
    ops.system('BandGeneral')     #  how to store and solve the system of equations in the analysis
    ops.test('NormDispIncr',1.0e-8,6)     #  determine if convergence has been achieved at the end of an iteration step
    ops.algorithm('Newton')     #  use Newtons solution algorithm: updates tangent stiffness at every iteration
    ops.integrator('LoadControl',0.1)     #  determine the next time step for an analysis,   apply gravity in 10 steps
    ops.analysis('Static')     #  define type of analysis static or transient
    ops.analyze(10)     #  perform gravity analysis
    ops.loadConst('-time',0.0)     #  hold gravity constant and restart time
    
    # define LATERAL load -------------------------------------------------------------
    # Lateral load pattern
    ops.timeSeries('Linear',2)     # timeSeries Linear 2;
    # define Load Pattern
    ops.pattern('Plain',2,2) # 
    ops.load(2,2000.,0.0,0.0)     #  node , FX FY MZ -- representative lateral load at top node
    
    
    # pushover: diplacement controlled static analysis
    ops.integrator('DisplacementControl',2,1,0.1)     #  switch to displacement control, for node 11, dof 1, 0.1 increment
    ops.analyze(1000)     #  apply 100 steps of pushover analysis to a displacement of 10
    
    print('Done!')
    
    Done!
    
    In [2]:
    eSEESminiPy.drawModel()
    
    In [3]:
    # plot deformed shape at end of analysis (it may have returned to rest)
    # amplify the deformtions by 5
    eSEESminiPy.drawDeformedShape(5)
    
    In [4]:
    ops.wipe() # the wipe command here closes all recorder files
    plt.close('all')
    fname3 = 'Data/DFreeEx1aPush.out'
    dataDFree = numpy.loadtxt(fname3)
    plt.subplot(211)
    plt.title('Ex1a.Canti2D.Push.tcl')
    plt.grid(True)
    plt.plot(dataDFree[:,1])
    plt.xlabel('Step Number')
    plt.ylabel('Free-Node Displacement')
    plt.subplot(212)
    plt.grid(True)
    plt.plot(dataDFree[:,1],dataDFree[:,0])
    plt.xlabel('Free-Node Disp.')
    plt.ylabel('Pseudo-Time (~Force)')
    plt.show()
    print('End of Run: pyEx1a.Canti2D.Push.tcl.py')
    
    End of Run: pyEx1a.Canti2D.Push.tcl.py
    
    In [ ]: