×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Rotations

Rotations

Rotations

(OP)
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.

RE: Rotations

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.  

RE: Rotations

(OP)
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

RE: Rotations

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....

RE: Rotations

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.

RE: Rotations

Problem solved ....I guess.

RE: Rotations

(OP)
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.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources