# odbRead.py
# A script to read the Abaqus/CAE Visualization module tutorial
# output database and read displacement data from the node at
# the center of the hemispherical punch.
from odbAccess import *
odb = openOdb(path='viewer_tutorial.odb')
# Create a variable that refers to the
# last frame of the first step.
lastFrame = odb.steps['Step-1'].frames[-1]
# Create a variable that refers to the displacement 'U'
# in the last frame of the first step.
displacement = lastFrame.fieldOutputs['U']
# Create a variable that refers to the node set 'PUNCH'
# located at the center of the hemispherical punch.
# The set is associated with the part instance 'PART-1-1'.
center = odb.rootAssembly.instances['PART-1-1'].\
nodeSets['PUNCH']
# Create a variable that refers to the displacement of the node
# set in the last frame of the first step.
centerDisplacement = displacement.getSubset(region=center)
# Finally, print some field output data from each node
# in the node set (a single node in this example).
for v in centerDisplacement.values:
print('Position = ', v.position,'Type = ',v.type)
print('Node label = ', v.nodeLabel)
print('X displacement = ', v.data[0])
print('Y displacement = ', v.data[1])
print('Displacement magnitude =', v.magnitude)
odb.close()
The resulting output is
Position = NODAL Type = VECTOR
Node label = 1000
X displacement = -8.29017850095e-34
Y displacement = -76.4554519653
Displacement magnitude = 76.4554519653