Can I use a static linear perturbation step in ABAQUS?

[Bradley_123]

Hello,

When should I use a static linear perturbation step? I get the same stress results between my general static step and my static linear perturbation step. If so, then what is the difference. Please let me know.

 

[SWComposites]

are you running linear or non-linear analysis?
are you running stress solution or buckling solution?

 

[FEA way]

Static linear perturbation step is mostly useful when using the load case feature or when ensuring fully linear solution (general static step supports all nonlinearities).

 

[Vishakh_Rajendran]

Hello,

For the same model features, should the conditions support the usage (if we don’t have a complex load path / nonlinear load path / any non-linearity), a static linear perturbation step is faster than a general static step (and a static linear perturbation should be used in such cases).

Note that the name of the step itself is static LINEAR perturbation and hence it does not support any form of non-linearity (material, geometry or contacts). In simpler words, the stiffness matrix does not change in a linear perturbation step.

So, if you do a linear procedure and think that a single increment is enough in the step (that is, no complex load paths or amplitudes), then a static linear perturbation makes more sense than a general static procedure (note that the principle of superposition holds true in a LP step).

But, if you have succeeding general steps, then a static LP should not be used. This is because stresses in a LP step are peturbation stresses and are local to that step (around the base state at the begininning of the step) and so the stresses are not carried forward. So if you have a sequence like ' LP step > General static step ', then it is better not to use the static Linear Perturbation step.

Best Regards,

Vishakh Rajendran.