An Abaqus Scripting Interface version of FPERT

A Fortran program that reads the Abaqus results file and creates a deformed mesh from the original coordinate data and eigenvectors is described in Creation of a perturbed mesh from original coordinate data and eigenvectors: FPERT. This example illustrates an Abaqus Scripting Interface script that reads an output database and performs similar calculations.

The command line arguments provide the following:

  • odbName: The output database file name.

  • modeList: A list of eigenmodes to use in the perturbation.

  • weightList: The perturbation weighting factors.

  • outNameUser: The output file name (optional).

Use the following command to retrieve the example script: 

abaqus fetch job=odbPert
# Abaqus Scripting Interface version of FPERT, a Fortran
# program to create a perturbed mesh from original coordinate
# data and eigenvectors. FPERT is described in the Abaqus Example
# Problems Manual.

import sys
from odbAccess import *
from types import IntType

# Get input from the user

odbName = input('Enter odb name (w/o .odb): ')
modes = eval(input('Enter mode shape(s): '))
if type(modes) is IntType:
    modes = (modes,)

odb = openOdb(odbName + '.odb')

# Get the undeformed coordinates from the first
# step and frame

step = odb.steps.values()[0]

try:
  coords = step.frames[0].fieldOutputs['COORD']
except:
  err = "The analysis must include a field output request \
      for variable COORD."
  print(err)
  sys.exit(1)

# Perturb the nodal coordinates

factors = []
for mode in modes:
    try:
       frame = step.frames[mode]
    except IndexError:
       print('Input error: mode %s does not exist' % mode)
       sys.exit(1)
    factors.append(float(input(
        'Enter imperfection factor for mode %s: '% mode)))
    coords = coords + factors[-1] * frame.fieldOutputs['U']

# Write new nodal coordinates to a file

outFile = open(odbName + '_perturbed.inp', 'w')
header = \
"""
*******************************************************
** Node data for perturbed mesh.
** Input mesh from: %s
** Mode shapes used: %s
** Imperfection factors used: %s
*******************************************************
"""
outFile.write(header % (odbName, modes, factors))
format = '%6i, %14.7e, %14.7e, %14.7e\n'
for value in coords.values:
    outFile.write(
        format % ((value.nodeLabel,) + tuple(value.data)))
outFile.write('** End of perturbed mesh node input file.')
outFile.close()