Failure of a steel 1

[trabu]

I've a problem.
I must study the load capacity of a steel.
I must use an elasto-plastic costitutive law.
My problem is that: i'm not able to define the failure of my steel. When i launch the job, the program continues to increase the plastic deformation without that the material crashes!!!
I want that when the material arrives to a deformation that i define, the element crashes and the analysis stops.
How can i define this failure criteria?
Please help me!

 

[mrgoldthorpe]

trabu,

The "failure" of your steel depends on many things:
* the type of steel,
* the temperature,
* the structure or component it is made into,
* detailed geometrical detail: such as the presence of a stress concentrating feature, or even a crack.

There are damage models and facilities available in ABAQUS that allow "failure", but you must first consider the above and decide the damage mechanism(s) that operate in your circumstances.

Regards,
MRG

 

[bassmanjax]

Hi Trabu

I concur with what MrG said.

Also, if you want material failure in your model, you need to be looking at the *DAMAGE INITIATION and *DAMAGE EVOLUTION options. These are only available in Explicit though (section 11.6.1 of the Analysis Users Manual)

I assume that you are using a *ELASTIC and *PLASTIC material model? The *PLASTIC model will not give failure at the last specified *PLASTIC point - ABAQUS will extrapolate the data forward, so the material never actually 'fails' as we would expect in real life.

Martin

 

[trabu]

But is it possible with the standard version?
I have only this version

 

[corus]

Surely there's the *failure criteria option

corus

 

[trabu]

Where are the failure criteria option in the standard version?

 

[bassmanjax]

Hi Trabu

There is *FAIL STRESS and *FAIL STRAIN - but these are generally used with composites (see section 10.2.3 of the ABAQUS Analysis Users Manual).

It sounds to me like you want to have the elements removed from the model as they fail by setting a failure stress. As far as I know, this is only possible in Explicit with the dynamic failure models. If there is a way to do it in Standard, I can't find one.

Martin

 

[trabu]

I want that when an element reach the failure stress, the analysis stops so taht i have the failure load.

 

[bassmanjax]

Hi Trabu

Now I see what you're trying to do

Unfortunately, I don't think there is any way of stopping an ABAQUS/Standard analysis at a specific value of stress. If anyone else knows a way, then I will learn something new aswell.

You may have to fall back on examining the principal stresses and plastic strains (PEEQ) to figure out how close you are to failure of the material.

Regards

Martin

 

[as3029]

i am not sure, but look at plasticity option on *static

 

[xydrex]

If it is a tension test, then you can use the necking event to determine that it is 'about' to fail. For this you must design into your model a small imperfection such as a small notch, otherwise it will never neck. In reality breaking occurs quickly after necking has occured, but in ABQ the stretching will continue indefinately so its up to you to interpret the results & decide if rupture would have occured.

The strain at which necking occurs is called the 'instability' strain, look up plasticity books on it, Im not sure if ABQ manuals say anything about it. There is a formula to determine it based on the plastic properties of the metal defined by the Ramberg-Osgood plasticity formula.

 

[gurmeet2003]

Trabu,

Couldn't you let the results run past failure and then plot the stresses vs. load to determine at what load the failure occurs?

Gurmeet