time increment error

[Mechanicslearner]

Hello,

Am trying to get displacement results of a plate by using static step with nonlinear and applying point load near the end of plate and other end is fixed.

The point load should be 15.3376 Newtons in negative Z direction but when I apply it fully by setting amplitude too it shows time increment error so I reduced to 11.3376 N and it worked then I increased to 12.3376 N too it shows the same time increment error like before saying too many attempts made for this increment even when I apply load slowly by setting in amplitude .I even tried splitting into two steps and applied still did not work. Am I applying plastic strain values wrong? i have attached image for detail description. See it and help me

 

[Mustaine3]

The last result before the abort, are the max mises stresses at app. 135.2?

 

[Mechanicslearner]

Yes that was the max von mises stress value approx 135. Now I removed the yield stress and plastic strain value after 135.2 (max yield stress) and it works fine but when I increase load further it gives error again. Does it have to do with plasticity values?

 

[Mustaine3]

Decreasing plastic data usually make no sense, because with increasing load you need increasing stresses.
With a nondecreasing curve, after the highest stress value in the plasticity table, the behavior is perfect plastic. So same issue here - with increasing load the stress can't increase, which prevents finding an equilibrium.

You have to make sure that the stresses in your plastic data are higher than the stresses that are reached in the analysis.

If you want to have damage in your material, you have to use damage initiation and damage behavior. Or other damaga and failure methods.

 

[Mechanicslearner]

Yes my stress values after analysing are exceeding than the maximum yield stress specified in plastic data. Is there anyway of reducing it? the displacement values are also high in abaqus (6.8 cm) when comparing to physical test which is 5.3 cm. I cannot change stress strain graph either so have no idea what is causing this..

 

[Mustaine3]

As mentioned, either you add damage or you add additional increasing platicity data. Make assumptions if necessary.

Is NLGEOM active? Is the shell thickness correct? Check everything that can effect the results.

 

[mrgoldthorpe]

Points loads on a node and plasticity together are not a good idea. You'll probably find that you have excessive yielding around the load. That's perhaps why your displacement (at load point?) is larger than the test value.

Try distributing the point load over a larger area, or make a small region surrounding the load elastic material so it doesn't yield.