Calculating E from stress and strain in ABAQUS?

[spintwo]

Hello everyone,

Is there a way to calculate E from stress and strain in ABAQUS? The reason I ask is because there is no field like that in the field output or history output requests list...

Thanks in advance.

 

[deyentl]

Hey spintwo,

I have done this before. Below you can find a script that works for my output database. You can adjust it to make it work for yours as well.

If you have any more questions, don't hesitate to ask.



# Import the necessary libraries from Abaqus

from Numeric import *
from Matrix import *
from LinearAlgebra import *
from abaqusConstants import *
from abaqus import *

import odbAccess

## calculate the average stiffness ####

# Calculate the entire volume of UC

LenX=100
LenY=100
LenZ=1
UVol=LenX*LenY*LenZ

# These values will be needed later in the program

Cord100=0
Cord010=0
Cord001=0
Cord200=1

# Enter the correct name of the job in the next line

JobName='Dirichlet_d5_10'
OdbName=JobName+'.odb'
myodb=odbAccess.openOdb(path=OdbName)

# Enter the correct step name in the next line

mystress=myodb.steps['Step-1'].frames[-1].fieldOutputs['S']
mystrain=myodb.steps['Step-1'].frames[-1].fieldOutputs['E']

# Transform the stress to the global coordinate system. The stresses were originally in local coordinates, you have to transform them!

odb = session.odbs[OdbName]
scratchOdb = session.ScratchOdb(odb)

# Build up the global coordinate system

scratchOdb.rootAssembly.DatumCsysByThreePoints(name='AGlobalSys',
coordSysType=CARTESIAN, origin=(Cord100, Cord010,
Cord001), point1=(Cord200, Cord010, Cord001), point2=(
Cord100, Cord200, Cord001))

# The actual transformation happens in the next three lines
s_AGlobalCoord = session.scratchOdbs[OdbName].rootAssembly.datumCsyses['AGlobalSys']
tmpField1 = mystress.getTransformedField(datumCsys=s_AGlobalCoord)
mystress=tmpField1
tmpField2 = mystrain.getTransformedField(datumCsys=s_AGlobalCoord)
mystrain=tmpField2

# Make sure IVOL is defined in the fieldoutputs!

myivol=myodb.steps['Step-1'].frames[-1].fieldOutputs['IVOL']

# Give the instance the correct name!

myelement=myodb.rootAssembly.instances['PART-1-1'].elements

# Home made for exercise 1 - calculation for all boundary conditions

############# Actual calculations ##############
strain11 = 0
strain22 = 0
stress11 = 0
# Loop over all elements
for j in range(len(mystress.values)):
# data[0] means S11, values[j] indicates the element
stress11 = stress11 + mystress.values[j].data[0]*myivol.values[j].data



for j in range(len(mystrain.values)):
# data[0] means E11, values[j] indicates the element
strain11 = strain11 + mystrain.values[j].data[0]*myivol.values[j].data
strain22 = strain22 + mystrain.values[j].data[1]*myivol.values[j].data



# Take the average over the volume
stress11 = stress11/UVol
strain11 = strain11/UVol
strain22 = strain22/UVol
# Calculate stiffness
stiffness = stress11/strain11
poisson = -strain22/strain11

# Print the values for verification

print strain
print stress
print stiffness
print poisson

 

[spintwo]

Is this just a Pearl script that you open in Abaqus?

 

[deyentl]

No, it's 100% python script.

You can probably leave out the transformation part in your case. I was working with a local and global CSYS which were different.

 

[spintwo]

Thanks so much!

 

[deyentl]

You're welcome.