×
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

time increment error

time increment error

time increment error

(OP)
Hello,

Am trying to get displacement results of a plate by using static step with nonlinear and applying point load near the end of plate and other end is fixed.

The point load should be 15.3376 Newtons in negative Z direction but when I apply it fully by setting amplitude too it shows time increment error so I reduced to 11.3376 N and it worked then I increased to 12.3376 N too it shows the same time increment error like before saying too many attempts made for this increment even when I apply load slowly by setting in amplitude .I even tried splitting into two steps and applied still did not work. Am I applying plastic strain values wrong? i have attached image for detail description. See it and help me

RE: time increment error

The last result before the abort, are the max mises stresses at app. 135.2?

RE: time increment error

(OP)
Yes that was the max von mises stress value approx 135. Now I removed the yield stress and plastic strain value after 135.2 (max yield stress) and it works fine but when I increase load further it gives error again. Does it have to do with plasticity values?

RE: time increment error

Decreasing plastic data usually make no sense, because with increasing load you need increasing stresses.
With a nondecreasing curve, after the highest stress value in the plasticity table, the behavior is perfect plastic. So same issue here - with increasing load the stress can't increase, which prevents finding an equilibrium.

You have to make sure that the stresses in your plastic data are higher than the stresses that are reached in the analysis.

If you want to have damage in your material, you have to use damage initiation and damage behavior. Or other damaga and failure methods.

RE: time increment error

(OP)
Yes my stress values after analysing are exceeding than the maximum yield stress specified in plastic data. Is there anyway of reducing it? the displacement values are also high in abaqus (6.8 cm) when comparing to physical test which is 5.3 cm. I cannot change stress strain graph either so have no idea what is causing this..

RE: time increment error

As mentioned, either you add damage or you add additional increasing platicity data. Make assumptions if necessary.

Is NLGEOM active? Is the shell thickness correct? Check everything that can effect the results.

RE: time increment error

Points loads on a node and plasticity together are not a good idea. You'll probably find that you have excessive yielding around the load. That's perhaps why your displacement (at load point?) is larger than the test value.

Try distributing the point load over a larger area, or make a small region surrounding the load elastic material so it doesn't yield.

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