×
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

Material softening and convergence issues
3

Material softening and convergence issues

Material softening and convergence issues

(OP)
Hey everyone,

I am modeling an isotropic material with an elastic-plastic behavior. I am applying a prescribed displacement. I want to soften the material but the *STATIC analysis never converges. I tried *Static, Riks but it never reaches the prescribed displacement. As soon as the material reaches the yield point, the displacement starts to decrease and I never get to see the softening. I've tried "automatic stabilization" with the *Static procedure but I couldn't get it to run past yield. I also tried breaking it into several steps with a small displacement increment but it still failed. The error is always the same, "time increment required is less than the minimum specified" even though my time increment is currently 1E-10.

Any advice is appreciated,
Thanks!

RE: Material softening and convergence issues

2
Try relaxing the displacement correction criterion using *CONTROLS ....

Once the load/displacement increments are very small the "noise" in nodal displacement corrections during iterations of an increment can easily be the same size as the nodal displacement increments themselves. This leads to further cut-backs and the error you experience.

Furthermore, set an initially small time increment in the load step, and don't allow the maximum increment in a step to become too large.

The following sets a more relaxed displacement tolerance of 10%, i.e. allows corrections to the displacements of 10% compared with the actual displacements.
*CONTROLS, PARAMETERS=FIELD, FIELD=DISPLACEMENT
** R_n^alpha C_n^alpha q_0^alpha q_n^aplha R_p^alpha eps^alpha
, 0.10 , , ,

Restricting the maximum size of the increment:
*STATIC
** init'l time period min. max.
** time of step time time
0.01 , 1.00 , 1.0E-6 , 0.01

RE: Material softening and convergence issues

... by the way: the reason for restricting the maximum size of an increment.

If you let ABAQUS increase it by default, and then it's forced to cut-back because it's rather too large when (say) gross yield or softening cuts in, you can end up completely losing the advantage gained from the previous larger increments.

The slow and steady tortoise often wins against the stumbling hare ....

RE: Material softening and convergence issues

(OP)
Thanks for your help. It helped a bit, but not to the degree of softening that I was looking for. I implemented the Ductile Criterion damage initiation to soften it and found that was a bit more robust than my "manual" softening. Still, had to settle with a "slow" damage.

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