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

[HalaD]

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

 

[Dave442]

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.

 

[Mustaine3]

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.

 

[HalaD]

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?

 

[pdiculous963]

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.

 

[ShadowWarrior]

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.

 

[HalaD]

ok thanks for all of you