Nonlinear analysis convergence problem

[koenigsegg]

Hi all,

I'm currently trying to run a nonlinear static analysis of an engine mount using this simplified 3D geometry:

http://files.engineering.com/getfil...49-401a-8379-c0a354242aa3&file=Undeformed.JPG

The material model is assumed to be a linear elastic one with a Young's Modulus of 2.5 MPa and a Poisson ratio of 0.45 (I'm using hybrid linear elements to prevent the problems related to the almost incompressible behavior of the material).

Although the fact that I've tried several material properties and analysis controls, I've not been able to achieve a complete analysis (there are frequent negative eigenvalues warnings and the analysis fails due to a excessively small "time" increment being used).

A curious aspect is the fact that the analysis always stops in the same deformed position:

http://files.engineering.com/getfil...6253-400b-826c-b5b33573f5c2&file=Deformed.JPG

(Please note that I've removed all contact interactions in order to simplify the model)

Does anyone have any idea for what might be wrong?

Thanks in advance,

koenigsegg

 

[corus]

Negative eigenvalues suugests you don't have it constrained properly. I don't understand where the non-linearity is though as you have linear elastic materials and have removed contact interactions? If you do have contact interactions somehow then use a first step to move the two (or more) objects together by fixed displacements, and then apply your real loads in further steps. It's sometimes better to use rough friction too to prevent any sliding when the surfaces are moving together in the 'normal' direction, and better to use zero friction if they are sliding across each other dynamically.

corus

 

[koenigsegg]

Hi all,

The non-linearity is purely geometrical (due to large deformations). As to the boundary conditions, I've applied an encastre to the peripheral cylindrical surface and there is a concentrated load applied in the x marked point (a reference point associated to a rigid discrete surface). Although some of my previous analysis had contact interactions, this one doesn´t have any (apart from the tie contraint between the 3D solid body and the discrete rigid surface mentioned).

Thanks in advance,

koenigsegg

 

[rstupplebeen]

The gap may be too large for the tied constraint. Check for things similar to warning or error sets saying that not all tied elements were within tolerance. This would indicate that the gap between surfaces is greater than what you specified. Hope this helps.

Rob Stupplebeen

 

[corus]

Of course with large deformation you can get buckling in some form where at some load you get infinite deformation. That may be why your analysis always fails at the same time, or equivalently, the same load. You could always replace your load with a fixed displacement to get a result and then plot the reaction force at the rigid body reference point to establish at which part of the step you have reached your desired load, if it ever reaches that point.

corus

 

[koenigsegg]

Hi Rob,

Unfortunatly no such messages appear.

Thanks,

koenigsegg

 

[koenigsegg]

Hi corus,

I've also thought of that, but when I tried applying a fixed displacement instead of a load the analysis stopped in the same position as before.

Thanks,

koenigsegg

 

[corus]

If you're tieing a rigid body to the elastic body and applying fixed displacemnts to the rigid body then you may as well remove the rigid body and apply the fixed displacements directly to the elastic body. If there's a problem with the elastic body then you'll see it if you get no converged solution. If it works then the problem must be with the tied constraints or the rigid body. Make sure you restrain the rigid body in the rotational freedoms as well as the translational freedoms as that's a common mistake.

corus