Obtain Load-displacement curve from Abaqus/Explicit analysis via Python

Hi Aaron,

I happened to write some code that may be the kind you want. Please save the following code into a file XX.py and execute the file as:

 

abaqus python XX.py -o *.odb -n nodeLabel -v variableName > filename

 

 

"""

NodeField.py

Author: Fan Yang Dec2011 at Utoronto

Code to extract the values of the specified node

Variables from Field output of an output database.

Usage: abaqus python NodeField.py -odb odbName

       -node Node -var(optional) Var

Requirements:

1. -odb   : Name of the output database.

2. -node  : Node label

3. -var   : Name of the Variable to extract.

            If this parameter is not provided,

            default displacement output will be processed.

4. -help  : Print usage

"""

#~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~

from odbAccess import *

from sys import argv,exit

#~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~

def rightTrim(input,suffix):

    if (input.find(suffix) == -1):

        input = input + suffix

    return input

#~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~

def getNodeHist(odbName,Node,Var):

    """ Print values of the Variable Var(optional) for node Node

    """

    """ Open the output database """

    print 'Extract variable %s for node %d' %(Var,Node)

    odb = openOdb(odbName)

    assembly = odb.rootAssembly

    if Var:

        Variable=Var

    else:

        Variable='U'

        print 'Default displacement output'      

    for step in odb.steps.values():

        print 'Processing Step:', step.name

        print '%6s%10s%14s'%('Frame','Time','Values')

        for frame in step.frames:

            isVarPresent = 0

            Vardata=0.

            lendata=0

            incFrame = -1

            valFrame = 0.

            allFields = frame.fieldOutputs

            if (allFields.has_key(Variable)):

                isVarPresent = 1

                VarSet = allFields[Variable]

                for VarValue in VarSet.values:                

                    if (VarValue.nodeLabel == Node):

                        Vardata = VarValue.data

                        lendata = len(Vardata)

                        incFrame = frame.incrementNumber

                        valFrame = frame.frameValue

                if lendata==1:

                    print '%6d%10f'%(incFrame,valFrame),'%14.7e'%Vardata[0]

                elif lendata==2:

                    print '%6d%10f'%(incFrame,valFrame),'%14.7e %14.7e'%(Vardata[0],Vardata[1])

                elif lendata==3:

                    print '%6d%10f'%(incFrame,valFrame),'%14.7e %14.7e %14.7e'%(Vardata[0],Vardata[1],Vardata[2]) 

    """ Close the output database before exiting the program """

    odb.close()

#==================================================================

# S T A R T

#    

if __name__ == '__main__':

    

    odbName = None

    Node = 0

    Var = None

    argList = argv

    argc = len(argList)

    i=0

    while (i < argc):

        if (argList[i][:2] == "-o"):

            i += 1

            name = argList[i]

            odbName = rightTrim(name,".odb")

        elif (argList[i][:2] == "-n"):

            i += 1

            Nodestr = argList[i]

            Node=int(Nodestr)

        elif (argList[i][:2] == "-v"):

            i += 1

            Var = argList[i]

        elif (argList[i][:2] == "-h"):            

            print __doc__

            exit(0)

        i += 1

    if not (odbName):

        print ' **ERROR** output database name is not provided'

        print __doc__

        exit(1)

    if Node==0:

        print ' **ERROR** Node label is not provided'

        print __doc__

        exit(1)

    getNodeHist(odbName,Node,Var)

Hi,

It is fairly simple. 

A simple way to learn python scripting for ABAQUS is by reading *.rpy files in your odb folder. Any operation that you do in ABAQUS Visulization module is stored in the file. You can read the file to get an idea on how to fetch and plot the data. Let me know if you have questions

 

 

Use this to fetch the nodal displacements and forces for the nodeset 'ALL NODES'

from abaqusConstants import *
from odbAccess import *
from math import *
import sys

path='<>'
odbfile='*.odb'
outputfile='*.dat'
odb=openOdb('%s/%s'%(path,odbfile))
file1 = open('%s/%s'%(path,outputfile),'w')

#-------------------------------------------------------------------------------
framelen=len(odb.steps['Step-1'].frames)
nodes=odb.rootAssembly.nodeSets[' ALL NODES']

#Displacement

disp=session.xyDataListFromField(odb=odb, outputPosition=NODAL, variable=(('U',NODAL, ((COMPONENT, 'U1'), (COMPONENT, 'U2'), )), ), nodeSets=(' ALL NODES', ))

force=session.xyDataListFromField(odb=odb, outputPosition=NODAL, variable=(('RF',NODAL, ((COMPONENT, 'RF1'), (COMPONENT, 'RF2'), )), ), nodeSets=(' ALL NODES', ))

you can write the data ito .dat file and open it in matlab using 'dlmread' and plot the data