×
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

Why I have a stress that exceed the yield one in an elastc perfectly-plastic simulations?

Why I have a stress that exceed the yield one in an elastc perfectly-plastic simulations?

Why I have a stress that exceed the yield one in an elastc perfectly-plastic simulations?

(OP)
Hello
I started with a simple model a column in 3D, fixed at the bottom and the top expect a horizontal direction where a displacement was added along the edge equal to 3 cm(in the X direction).
I defined the properties of the steel elastic E 210 000 MPa , perfect plastic fy=235 MPa plastic strain= 0.
The values of S22(the vertical axis reached 285 MPa)
I've tried to change the boundary conditions also but it doesn't work.

Any one can help please
Thanks in advance


RE: Why I have a stress that exceed the yield one in an elastc perfectly-plastic simulations?

You're plotting nodal output. Is it just an issue with extrapolation/averaging? Switch to a quilt plot.

Also, look at von Mises stress and/or equivalent plastic strain. Mises yield surface is used to define isotropic yielding in Standard.

RE: Why I have a stress that exceed the yield one in an elastc perfectly-plastic simulations?

Use Tools > Query > Probe Value to check the results at the integration points. Here you'll find the yield stress.
The higher displayed values come from extrapolation of these values to the nodes.

Make sure you don't reach the ultimate yield stress at the integration points and that the extrapolation does not alter the results significantly. Refine the mesh to minimize the last effect.

RE: Why I have a stress that exceed the yield one in an elastc perfectly-plastic simulations?

(OP)
thanks for your response
In fact I've checked the results of the integration points and the values exceed the yielding stress in the vertical direction in all the simulations even though the Mises stress gives always the correct values and present an elastic perfect plastic behaviour.
I've performed static and dynamic simulations with different structures and the same problem appear each time.
Finally I think that it's related to the boundary conditions that I applied since the high stresses are located at the edges.
I've checked my model several times at there is no mistakes.
Can a found a solution? or I should just ignored and check my model by only referring to the Mises stress?

RE: Why I have a stress that exceed the yield one in an elastc perfectly-plastic simulations?

I think you are missing the point on the yield surface pointed out by Dave442 above. You can have directional (S11, S22, S33) stresses above yield, but the material will not be considered to be actively yielding until the mises stress meets your perfectly plastic yield strength. As you noted, the mises stresses are correct. It seems Abaqus is functioning correctly.

RE: Why I have a stress that exceed the yield one in an elastc perfectly-plastic simulations?

What you are observing is just one component of the stress tensor, you have to observe the Mises stress which combines all six components of the stress tensor.

Read carefully what Dave442 and pdiculous963 said.

RE: Why I have a stress that exceed the yield one in an elastc perfectly-plastic simulations?

(OP)
ok thanks for all of you

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