How to introduce plasticity in a nonlinear analysis with nonlinear materials?

[danielhoyos24]

Hi,

I have some problems by simulating an object wich forces induces plasticity on the element.

My analysis is a nonlinear analysis with nonlinear materials. I have created a specific material (steel) with a specific stress-strain curve.

The simulation I have is actually simple, I have a steel bar wich is loaded by an axial force in tension and this force goes upper the yield stress, therefor the material have plastic deformations. But the analysis I run, it doesn´t schow a plastic deformation, it goes always linear with the elasticity moduls.

How can I simulate this object to obtain plastic deformations?

Thanks.

Daniel

[AstroJohnPE]

Hi Daniel,

I suggest that you create an archive of your model and attach it to your reply. (See "Create, Post, or Provide an Archive of your model")

Also indicate which version of Simulation Mechanical you are using.

Also, what result are you using to determine whether it has gone plastic or not? A plot of the axial displacement should show a nonlinear behavior. (Select a node, right-click, Create a New Graph)

Otherwise, my guess is that the analysis type might be set to small deformation; that setting is under the element definition.

[danielhoyos24]

Hi John,

I have already solve the problem of the plasticity in tension. I used brick as element type, von misses with isotropic hardening as element definition and a specific strain-stress curve on the material. 

I had excelent results by tension, but in compresion it doesn´t converge. Is there a specific function or type to analys the same element in compresion upper the yield stress (having plastic deformations)?

My element to analys is simple; it is a metal block of two meter long with a cross section of b=200 mm and h=100 mm. I have a fixed restriction on one of the lateral edges faces and a load on the other side wich goes upper the yield stress.

Do you have any types to simulate this in compression?

Thanks.

Daniel

[zhuangs]

I have two points:

First, you can select "Enforced" option of "compatibility" and check "selective reduced integration".  "Included" midside nodes can also help.

Second, for the same model, compression can result in collapse, compared with tension.  To obtain better convergence, you can add more constraint on the center point of the side, which has the load.  For example, the load is along z-direction, you can add x- and y- constraint on the center.

These two points should help.

-Shoubing

[danielhoyos24]

I tried the combination of the two options you gave me and it didn´t converge again. It converge and show results until it goes under the yield stress, but on the step that it rises the yield stress it stop showing results.

Is there something else I can do?

I have tried using MES with nonlinear materials and Static stress with non linear materials with the same conditions, but neither of them converge upper the yield stress in compresion. In tension both of them show good results.

[zhuangs]

Could you share your model or send it to me?

Shoubing

[danielhoyos24]

Here it is.

The yield load with the material properties and geometry is 7720000 N and the ultimate load is 9920000 N. On this model I´m aplying a compression load of 8000000 N wich goes upper the yield stress. 

It shows results until the last step of the elastic region. After, it doesn´t converge.

Firt of all I´m trying to simulate a plastic behavior on this element in compression. But what I need exactly is to simulate this element with a cyclical load wich goes in compression and in traction. And it will be upper the yield stress and may accur buckling. Does this parameters allow also buckling?

Daniel

[zhuangs · Accepted solution]

Hi Daniel,

Both "Enforced" plus "selective reduced integration" and "Included" midside nodes are the best options for compression.  They usually can provide best convergence than other options.  Certainly, compression usually has difficult convergence, compared with tension.

However, your model has a different story, and even ABAQUS will have trouble to simulate it.  In youre model, all the nodes on the sections parallel to y-z plane in the bar have the same state.  Let's assume the force reachs Fy (yield) at time T, and

At T- (suppose the section area is A) , the model is still in elastic state (Young's modulus Ee).

At T+ (suppose the section area is A as well) , the model yieds (Hardeing modulus Eh).

form T- to T+, it is instaneous, and modulus changes from  Ee to Eh.  Though the force is the same, the strain change is huge, since usually Eh is much smaller than Ee.  For your model, Eh is about equal to Ee/800.  No matter how small the time step is, the time step is still larger than (  (T+) - (T-) ).

In the lab, tention/compression are usually controlled by prescribed displacement, which will not result in huge change (strain, displacement) instaneously.

-Shoubing