Is it possible to combine *imperfection and *initial stress Keywords? 1

[Martensite_Steel]

Hello everyone,

I'm currently working on buckling analysis of steel columns. I performed a simple linear buckling analysis as a linear perturbation step and let abaqus write the node displacements of the first Eigenform into a node-File via *NODE FILE keyword. My initial geometric imperfections should then be added in the following nonlinear buckling analysis via the *IMPERFECTION keyword. That worked out as planned.

I am also able to create the desired initial stresses in my cross-section in 3-direction with a sigini Subroutine in a seperate simulation.

So, everything for itself works fine.

Now I wanted to have both kinds of imperfections in my model and just can't get it to work. My plan was, to first put the initial stresses on my model, let Abaqus calculate an equilibrium in a static step, THEN add the imperfections with the *IMPERFECTION keyword just before the Riks Step. But it seems, that would have been too easy and abaqus just aborts my job during the data check and says the imperfection keyword is misplaced (which isn't true, so I guess the combination of *INITIAL CONDITIONS and *IMPERFECTION is the problem).

Is there a way or maybe a workaround to have both kinds of initial imperfections (residual stresses and geometric) in one model?

I appreciate any idea.

 

[FEA way]

Take a look at this video:

https://www.youtube.com/watch?v=QeN5KYcXVKc

It seems to show the same problem being solved. Maybe you will notice some differences between this and your simulation. Otherwise we will have to see your INP file to find errors.

 

[Martensite_Steel]

Thank you. This is basically it and the video helped me with the keyword placing. I've obviously been wrong and my keywords were misplaced for the combined model. I placed them in the order where I wanted them to be executed. So: Initial stress before the static step and *imperfections at the beginning of the riks step. This doesn't work and leads to the following:

The Abaqus manual recommends, to let Abaqus calculate an equilibrium after applying an initial stress field to a model. This should be performed via a general static step preferably in only one increment (max time step=initial time step).

My SIGINI Subroutine has the initial stresses applied via a function of position of integration points on the undeformed model shape (a simple I-profile). When I apply stresses+imperfections like shown in the video, my model will be deformed and then the initial stress field will be added on the already deformed shape of the model. I wrote my subroutine in such a way, that the residual stresses are in a one dimensional equilbrium so that Abaqus will have to adjust them just a little in the static step. The deformations caused by the *Imperfection keyword cause that my subroutine doesn't work as perfectly anymore, because the geometric imperfections are applied before the stresses. And to change the script in such a way, that it applies to any given deformed shape is pretty hard (if possible at all) because of the function I use for residual stresses.

So I asked myself, if there is a possibility to apply the stresses first in the initial step, then let Abaqus compute an equilibrium state in one increment (via general static step as stated in the user manual) and then add the initial imperfections just before the nonlinear buckling riks step? So that my subroutine could still use the undeformed shape of my model. I'm pretty unfamiliar with the keyword manager, so I'm not sure if there's a way to control in which order the actions will be executed. At least changing the order of keyword appearance didn't solve my problem.

In the YouTube video there is no equilibrium step performed. I'm not sure if this is the right way, since Abaqus always had to change my stress field a little bit.

A workaround might be, to seperate all that in two simulations. The first one where the initial stresses are applied to an undeformed shape and the equilibrium state is being calculated and then import that mesh as an orphan mesh in the next simulation with the stresses applied to it, so that the initial imperfections can be applied and the nonlinear buckling Riks step can be performed. I'm not sure if this would work, but its just my idea. Although I would of course prefer a direct method where everything works in one simulation.

 

[Mustaine3]

When you apply the initial stresses and run an equilibrium step, then you will get deformations. Then you want to apply the imperfections? I'm not sure if that makes sense (physically). The imperfections are the deviations from the perfect initial shape. But you don't have a perfect shape anymore after the initial stresses are in.

But if you want to apply both things at the same time, then I might have a idea.

 

[Martensite_Steel]

You got that right and I'm aware of the fact, that the equilibrium step causes little deformations. The thing is, I want to seperate the cases that lead to a lower buckling load. On the one hand, I have imperfections caused by the out-of-straightness of the sheet metals. On the other hand I have residual stresses caused by a welding process. The out-of-straightness is relatively easy to measure, but residual stresses are not. So, I want to investigate the influence of different residual stress patterns on the buckling load of my columns. My aim is to always apply the same initial geometric imperfection with the maximum value of - let's say - L/1000 (where L is the length of the column) to take into account the out-of-straightness of the column.


Modern design codes apply all kinds of imperfections via an artificial deformation. So I'd just scale the shape of the eigenmode of interest to the desired value. But this is exactly what I want to avoid, since I wouldn't be able to apply different residual stress patterns directly. I hope, I was able to explain the problem I want to solve.

May I ask, what idea you have in mind?