The following sections describe how you can access the data in an output database. Examples are included that refer to the ABAQUS/CAE Visualization module tutorial output database, viewer_tutorial.odb. This database is generated by the input file from Case 2 of the example problem, “Indentation of an elastomeric foam specimen with a hemispherical punch,” Section 1.1.4 of the ABAQUS Example Problems Manual. The problem studies the behavior of a soft elastomeric foam block indented by a heavy metal punch. The tutorial shows how you can use the Visualization module to view the data in the output database. The tutorial describes how you can choose the variable to display, how you can step through the steps and frames in the analysis, and how you can create X–Y data from history output.

You are encouraged to copy the tutorial output database to a local directory and experiment with the ABAQUS Scripting Interface. The output database and the example scripts from this manual can be copied to the user's working directory using the ABAQUS fetch utility:

abaqus fetch job=name

abaqus fetch job=viewer_tutorial

To make the Odb commands available to your script, you first need to import the odbAccess module using the following statements:

from odbAccess import *
from abaqusConstants import *

from odbMaterial import *
from odbSection import *

You use the openOdb method to open an existing output database. For example, the following statement opens the output database used by the ABAQUS/CAE Visualization module tutorial:

odb = openOdb(path='viewer_tutorial.odb')

The following list describes the objects in model data and the commands you use to read model data. Many of the objects are repositories, and you will find the keys() method useful for determining the names of the objects in the repository. For more information, see “Using dictionaries,” Section 4.6.2, and “Repositories,” Section 5.3.3.

myAssembly = odb.rootAssembly

for instanceName in odb.rootAssembly.instances.keys():
  print instanceName

PART-1-1

print 'Node sets = ',odb.rootAssembly.nodeSets.keys()

Node sets = ['ALL NODES']

print 'Node sets = ',odb.rootAssembly.instances[
    'PART-1-1'].nodeSets.keys()
print 'Element sets = ',odb.rootAssembly.instances[
    'PART-1-1'].elementSets.keys()

Node sets =  ['ALLN', 'BOT', 'CENTER', 'N1', 'N19', 'N481',
              'N499', 'PUNCH', 'TOP']
Element sets = ['CENT', 'ETOP', 'FOAM', 'PMASS', 'UPPER']

topNodeSet = odb.rootAssembly.instances[
    'PART-1-1'].nodeSets['TOP']

allMaterials = odb.materials
for materialName in allMaterials.keys():
    print 'Material Name : ',materialName

for material in allMaterials.values():      
    if hasattr(material,'elastic'):
        elastic = material.elastic
        if elastic.type == ISOTROPIC:
            print 'isotropic elastic behavior, type = %s' \
            % elastic.moduli
            title1 = 'Young modulus  Poisson\'s ratio  '
            title2 = ''
            if elastic.temperatureDependency == ON:
                title2 = 'Temperature  '    
            dep = elastic.dependencies
            title3 = ''
            for x in range(dep):
                title3 += ' field # %d' % x                
            print '%s %s %s' % (title1,title2,title3)
            for dataline in elastic.table:
                print dataline

if hasattr(material,'hyperelastic'):
    hyperelastic = material.hyperelastic
    testData = hyperelastic.testData
    if testData == ON:
        if hasattr(hyperelastic,'biaxialTestData'):
            biaxialTestData = hyperelastic.biaxialTestData  
            print 'smoothing type : ',biaxialTestData.smoothing 

allSections = odb.sections
for sectionName in allSections.keys():
    print 'Section Name : ',sectionName

for mySection in allSections.values(): 
    if type(mySection) == HomogeneousSolidSectionType:
        print 'material name = ', mySection.material
        print 'thickness = ', mySection.thickness

allProfiles = odb.profiles.values()
numProfiles = len(allProfiles)
print 'Total Number of profiles in the ODB : %d' \
    % numProfiles 

for myProfile in allProfiles:  
    if type(myProfile) == CircularProfileType:
        print 'profile name = %s, radius = %8.3f' \
            % (myProfile.name,myProfile.r) 

instances = odb.rootAssembly.instances
for instance in instances.values():
    assignments = instance.sectionAssignments
    print 'Instance : ',instance.name
    for sa in assignments:
        region = sa.region
        elements = region.elements
        mySection = sa.section            
        print '  Section : ',mySection.name
        print '  Elements associated with this section : '
        for e in elements:
            print '  label : ',e.label 

The following list describes the objects in results data and the commands you use to read results data. As with model data you will find it useful to use the keys() method to determine the keys of the results data repositories.

for stepName in odb.steps.keys():
  print stepName

Step-1
Step-2
Step-3

step1 = odb.steps.values()[0]
print step1.name

Step-1

lastFrame = odb.steps['Step-1'].frames[-1]

Field output data are stored in the fieldOutputs repository under the OdbFrame object. The key to the repository is the name of the variable. The following statements list all the variables found in the last frame of the first step (the statements use the variable lastFrame that we defined previously):

for fieldName in lastFrame.fieldOutputs.keys():
    print fieldName

COPEN    TARGET/IMPACTOR
CPRESS   TARGET/IMPACTOR
CSHEAR1  TARGET/IMPACTOR
CSLIP1   TARGET/IMPACTOR
LE
RF
RM3
S
U
UR3

You can use the following to view all the available field data in a frame:

# For each field output value in the last frame,
# print the name, description, and type members.

for f in lastFrame.fieldOutputs.values():
    print f.name, ':', f.description
    print 'Type: ', f.type

    # For each location value, print the position.
  
    for loc in f.locations:
        print 'Position:',loc.position
    print

COPEN    TARGET/IMPACTOR : Contact opening
Type:  SCALAR
Position: NODAL

CPRESS   TARGET/IMPACTOR : Contact pressure
Type:  SCALAR
Position: NODAL

CSHEAR1  TARGET/IMPACTOR : Frictional shear
Type:  SCALAR
Position: NODAL

CSLIP1   TARGET/IMPACTOR : Relative tangential motion direction 1
Type:  SCALAR
Position: NODAL

LE : Logarithmic strain components
Type:  TENSOR_2D_PLANAR
Position: INTEGRATION_POINT

RF : Reaction force
Type:  VECTOR
Position: NODAL

RM3 : Reaction moment
Type:  SCALAR
Position: NODAL

S : Stress components
Type:  TENSOR_2D_PLANAR
Position: INTEGRATION_POINT

U : Spatial displacement
Type:  VECTOR
Position: NODAL

UR3 : Rotational displacement
Type:  SCALAR
Position: NODAL

In turn, a FieldOutput object has a member values that is a sequence of FieldValue objects that contain data. Each data value in the sequence has a particular location in the model. You can query the FieldValue object to determine the location of a data value; for example,

displacement=lastFrame.fieldOutputs['U']
fieldValues=displacement.values

# For each displacement value, print the nodeLabel
# and data members.

for v in fieldValues:
    print 'Node = %d U[x] = %6.4f, U[y] = %6.4f' % (v.nodeLabel,
    v.data[0], v.data[1])

Node = 1 U[x] = 0.0000, U[y] = -76.4580
Node = 3 U[x] = -0.0000, U[y] = -64.6314
Node = 5 U[x] = 0.0000, U[y] = -52.0814
Node = 7 U[x] = -0.0000, U[y] = -39.6389
Node = 9 U[x] = -0.0000, U[y] = -28.7779
Node = 11 U[x] = -0.0000, U[y] = -20.3237...

fieldValues[0].__members__

['instance', 'elementLabel', 'nodeLabel', 'position',
 'face', 'integrationPoint', 'sectionPoint', 
'localCoordSystem', 'type', 'data', 'magnitude',
 'mises', 'tresca', 'press', 'inv3', 'maxPrincipal',
 'midPrincipal', 'minPrincipal', 'maxInPlanePrincipal',
 'minInPlanePrincipal', 'outOfPlanePrincipal']

After you have created an OdbSet object using model data, you can use the getSubset method to read only the data corresponding to that region. Typically, you will be reading data from a region that refers to a node set or an element set. For example, the following statements create a variable called center that refers to the node set PUNCH at the center of the hemispherical punch. In a previous section you created the displacement variable that refers to the displacement of the entire model in the final frame of the first step. Now you use the getSubset command to get the displacement for only the center region.

center = odb.rootAssembly.instances['PART-1-1'].nodeSets['PUNCH']
centerDisplacement = displacement.getSubset(region=center)
centerValues = centerDisplacement.values
for v in centerValues:
    print v.nodeLabel, v.data

1000 array([0.0000, -76.4555], 'd')

topCenter = \
    odb.rootAssembly.instances['PART-1-1'].elementSets['CENT']
stressField = odb.steps['Step-2'].frames[3].fieldOutputs['S']

# The following variable represents the stress at 
# integration points for CAX4 elements from the 
# element set "CENT."

field = stressField.getSubset(region=topCenter, 
    position=INTEGRATION_POINT, elementType = CAX4)
fieldValues = field.values
for v in fieldValues: 
    print 'Element label = ', v.elementLabels,     
    if v.integrationPoint:
        print 'Integration Point = ', v.integrationPoint
    else:
        print
# For each tensor component.

    for component in v.data:

# Print using a format. The comma at the end of the 
# print statement suppresses the carriage return.

        print '%-10.5f' % component,

# After each tuple has printed, print a carriage return.

    print

Element label =  1 Integration Point =  1
S : 0.01230    -0.05658   0.00892    -0.00015  
Element label =  1 Integration Point =  2
S : 0.01313    -0.05659   0.00892    -0.00106  
Element label =  1 Integration Point =  3
S : 0.00619    -0.05642   0.00892    -0.00023  
Element label =  1 Integration Point =  4
S : 0.00697    -0.05642   0.00892    -0.00108  
Element label =  11 Integration Point =  1
S : 0.01281    -0.05660   0.00897    -0.00146  
Element label =  11 Integration Point =  2
S : 0.01183    -0.05651   0.00897    -0.00257  
Element label =  11 Integration Point =  3 ...

Possible values for the position argument to the getSubset command are:

History output is output defined for a single point or for values calculated for a portion of the model as a whole, such as energy. Depending on the type of output expected, the historyRegions repository contains data from one of the following:

The history data object model is shown in Figure 8–5.

The output from all history requests that relate to a specified point is collected in one HistoryRegion object. A HistoryRegion object contains multiple HistoryOutput objects. Each HistoryOutput object, in turn, contains a sequence of (frameValue, value) sequences. In a time domain analysis (domain=TIME) the sequence is a tuple of (stepTime, value). In a frequency domain analysis (domain=FREQUENCY) the sequence is a tuple of (frequency, value). In a modal domain analysis (domain=MODAL) the sequence is a tuple of (mode, value).

In the analysis that generated the ABAQUS/CAE Visualization module tutorial output database, the user asked for the following history output:

The history output data can be retrieved from the HistoryRegion objects in the output database. The tutorial output database contains HistoryRegion objects that relate to the rigid body reference point and the integration points of the corner element as follows:

from odbAccess import *

odb = openOdb(path='viewer_tutorial.odb')
step2 = odb.steps['Step-2']
region = step2.historyRegions['Node PART-1-1.1000']
u2Data = region.historyOutputs['U2'].data
dispFile = open('disp.dat','w')
for time, u2Disp in u2Data:
    dispFile.write('%10.4E   %10.4E\n' % (time, u2Disp))
dispFile.close()

The following script illustrates how you can open the output database used by the ABAQUS/CAE Visualization module tutorial output database and print out some nodal and element information. Use the following commands to retrieve the example script and the tutorial output database:

abaqus fetch job=odbElementConnectivity
abaqus fetch job=viewer_tutorial

# odbElementConnectivity.py
# Script to extract node and element information.
#
# Command line argument is the path to the output
# database.
#
# For each node of each part instance:
#     Print the node label and the nodal coordinates.
#
# For each element of each part instance:
#     Print the element label, the element type, the
#     number of nodes, and the element connectivity.

from odbAccess import *
import sys

# Check that an output database was specified.

if len(sys.argv) != 2:
    print 'Error: you must supply the name \
        of an odb on the command line'
    sys.exit(1)

# Get the command line argument.

odbPath = sys.argv[1]

# Open the output database.

odb = openOdb(path=odbPath)

assembly = odb.rootAssembly

# Model data output

print 'Model data for ODB: ', odbPath

# For each instance in the assembly.

numNodes = numElements = 0

for name, instance in assembly.instances.items():
    
    n = len(instance.nodes)
    print 'Number of nodes of instance %s: %d' % (name, n)
    numNodes = numNodes + n

    print
    print 'NODAL COORDINATES'

    # For each node of each part instance
    # print the node label and the nodal coordinates.
    # Three-dimensional parts include X-, Y-, and Z-coordinates.
    # Two-dimensional parts include X- and Y-coordinates.

    if instance.embeddedSpace == THREE_D:
        print '    X         Y         Z'
        for node in instance.nodes:
            print node.coordinates
    else:
        print '    X         Y'
        for node in instance.nodes:
            print node.coordinates
             
    # For each element of each part instance
    # print the element label, the element type, the
    # number of nodes, and the element connectivity.
       
    n = len(instance.elements)
    print 'Number of elements of instance ', name, ': ', n
    numElements = numElements + n

    print 'ELEMENT CONNECTIVITY'
    print ' Number  Type    Connectivity'
    for element in instance.elements:
        print '%5d %8s' % (element.label, element.type),
        for nodeNum in element.connectivity:
           print '%4d' % nodeNum,
        print
   
print
print 'Number of instances: ', len(assembly.instances)
print 'Total number of elements: ', numElements
print 'Total number of nodes: ', numNodes

The following script combines many of the commands you have already seen and illustrates how you read model data and field output data from the output database used by the ABAQUS/CAE Visualization module tutorial. Use the following commands to retrieve the example script and the tutorial output database:

abaqus fetch job=odbRead
abaqus fetch job=viewer_tutorial

# 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