Limit Load Analysis in Abaqus

[JG MechEng]

I am trying to learn how to do limit load analysis and haven't been able to figure out how to define an elastic-perfectly-plastic material. I am in the beginning stages of figuring this process out so anyone feels like supplying general guidance with this analysis in addition to the material set up it would be appreciated.

Specifically, how to i make the program not assume continuous slope (E) to the right of my yield stress and force it to zero slope? I know it should be strait forward but for some reason it's not liking my inputs into the stress strain table.

 

[Dave442]

Abaqus assumes constant slope beyond the last stress-strain point you define under *PLASTIC. So for perfect plasticity I think you can just define the yield stress at zero plastic strain.

*PLASTIC
YIELD, 0.0

 

[BenStewart]

For elastic-perfectly-plastic analyses I apply a small gradient after the yield strength so to avoid zero stiffness issues and assist with convergence i.e. yield strength at zero plastic strain then yield strength + 1MPa at unity plastic strain.

There are also procedures for including a stress-strain curve up to true UTS then perfectly plastic afterwards, but the load factors will be higher.

 

[JG MechEng]

BenStewart, is this material curve what you are describing? I am a bit confused about the "unity plastic strain" comment. Does this mean E=(Stress/0)? My understanding of reaching unity is (actual/allowable)=1.0. Neither of which match up with what I think of as perfectly plastic (E=0) Please provide a more in depth explanation. Thanks for the help in advance!

 

[BenStewart]

For perfectly plastic material properties you require only one point, as Dave442 indicated, i.e. the yield strength at zero plastic strain and as you said beyond this there is no stiffness. My suggestion of using two points is optional and could be thought of as "good practice" to assist with convergence i.e. include a small stiffness beyond the yield strength.

As an example...for an isotropic material with a yield strength of 300MPa (using N, mm units...) you could use:

*Plastic, type=isotropic
300, 0.
301, 1. (this line is optional)

Best to look at the keyword reference, user's and example problem guides...

 

[TGS4]

If you are performing a Limit Load analysis for compliance with ASME Section VIII, Division 2, Part 5, then I would strongly recommend to NOT follow the advice of BenStewart in regards to adding a small gradient after the yield point. While that may "help" the numerical issues with zero tangent modulus, it is those numerical issues that you are actually trying to find - not to mention that it violates the Code.

 

[JG MechEng]

TGS4, I am trying to learn how to do the limit load analysis per ASME Section VIII, Division 2, Part 5. My understanding is that the yield strength should be set to 1.5 S, and then E=0. The code is very clear in this, but I am having trouble setting up the non linear analysis in the software. It seems that the material data points should be (in US units and E=29E6):

Stress Strain

30,000 0.0010
30,000 0.0011


Not sure if this is correct

 

[TGS4]

Not correct.

Follow the above advice from Dave422.
30000 0.0

That is all.

 

[StefCon]

ASME Section VIII (Division 2) also specifies small deformation theory (NLGEOM=OFF), right?

 

[BenStewart]

For the limit load analysis method (elastic-perfectly plastic), yes.

 

[Mustaine3]

Running into perfect plasticity, even with the +1MPa advice, should be avoided. Even when there is convergence, results beyond the yield stress are kind of random, so I don't see a reason why to do that.

 

[JG MechEng]

The idea is that when you reach the plastic point, you have global instability of the model and the load that generated that instability is the limit load. There is no investigation beyond the yield point.

 

[TGS4]

Mustaine3 - not random, just that the displacements and strains are non-physical. There is much written in their literature about this type of analysis b