Rotations

[satyasrinivas]

Hi

I have developed a 3d nonlinear model in abaqus. The mesh consists of modified terahedral elements. Is it possible to obtain the distortional and rotational components of the strain for these elements ? I have the odb file but I am not exactly sure how to go about in getting the rotations. Can anyone please suggest me where I should start to obtain rotations.

Thanks in advance.

 

[xerf]

What exactly do you understand by "rotational components" of the strain tensor ?

ABAQUS provides the logarithmic strain tensor for geometrically non-linear analyses.

If think of polar decomposition of the deformation gradient F=RU, with R=the rotation tensor and U the stretch tensor then probably you need to do some post-processing.

As far as I remember (I might be wrong though), the components of deformation gradient are not available for direct output to the .odb file.

 

[satyasrinivas]

Xerf,

I was referring to the [R] matrix...in polar decomposition. Any thoughts on the 'post-processing' techniques that will allow me to see rotations..

Thanks

 

[xerf]

If you know the deformation gradient F at each integration point (IP) than, the procedure for finding R at each IP is:
1) compute the right Cauchy-Green deformation tensor
C=transpose(F)*F
2)find eigenvalues and eigenvectors of C
3)form the transformation matrix A with columns the eigenvectors of C, such that C'=A*C*transpose(A),
and C' is a diagonal matrix/tensor with the values on the diagonal the eigenvalues of C
4)Compute the stretch matrix along the principal directions U'=SQRT(C')
5)Compute the inverse of the stretch matrix inverse(U')
6)Compute full U=transpose(A)*U'*A
7)Compute full inverse(U)=transpose(A)*inverse(U')*A
8)Compute the rotation matrix
R=F*inverse(U)

However, ABAQUS does not output the deformation gradient to the .odb file but only to .dat file.

I wonder if there is a simpler way, since the CAE is able to plot the rotated material orientations....

 

[xerf]

Or....
you can assign material orientations in CAE->Property.
Abaqus will rotate the material orientations (i.e. R matrix at each IP) with rigid body rotations.

Then you can use the ABAQUS Scripting Interface to get the rotated material orientations...
something like this:

myOdb=session.odbs['my_odb_name']
my_frame=myOdb.steps['step_name'].frame[frame_number]
strain_field=my_frame.fieldOutputs['LE'] #assuming you requested the log strain
values=strain_field.values
for iValue in values:
print "Element=",iValue.elementLabel
print "IP=",iValue.integrationPoint
print "Local system=", iValue.localCoordSystem


Best.

 

[xerf]

Problem solved ....I guess.

 

[satyasrinivas]

thanks so much Xerf.

I was out of station and just checked your suggestions. I am not familiar at all regarding how and where to use the script.
Any suggestions on that ?

Secondly, I am using Patran 2006 for pre-processing. I always used CAE only for post processing.

I totally agree with you. Since CAE is plotting rotated orientations, it should be possible to get at element rotations. I am still continuing my work on the problem. In the meanwhile if you have anymore suggestions, please let me know.