Achieving static equilibrium in Abaqus/Explicit

[compabaq]

I'm trying to model a dynamic process, but in the first step I need to start by pre-straining my model to a static equilibrium. I have attempted to achieve this equilibrium by applying the displacement in a very gradual way. I have done this using a smooth amplitude, spread over a relatively long time. If I take this time long enough, then I can avoid major stress wave propagation. Nevertheless, I still get stress variations on the order of 10%, where they should all be exactly the same in the static equilibrium. I have also tried adding linear and quadratic bulk viscosity, but that did not seem to help at all.

What can I do to achieve static equilibrium more accurately in Explicit, with less residual stress waves propagation at the end?

Kind regards,
Compabaq

 

[IceBreakerSours]

Try applying the deformation at a constant velocity (so, the acceleration is zero).

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[compabaq]

This is what I did before I started using the smooth amplitude function. If you do this, then you create shock waves the moment you start and stop applying the constant velocity. This is normal, as you need to apply an infinite acceleration to get to your target velocity in an infinitely small time.

Do you have any other suggestions?

 

[IceBreakerSours]

I suspect you could break the analysis in to steps which have smooth amplitude deformation histories at the beginning/end and constant velocity deformation history in between.

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[Mustaine3]

Using a Smooth Step Amplitude is correct.
Did you used any Mass Scaling? Maybe too much?

How large is your kinetic energy compared to the internal energy?

 

[compabaq]

I was not using any mass scaling. In the meantime, I was able to resolve the issue by spreading the displacement over a large time.

In my improved simulations, the kinetic energy is negligible compared to the internal energy (at most 1/1000). Are there any other energy-related checks that I should/can make?

 

[Mustaine3]

No.

For other informations and tips see:
Getting Started with Abaqus: 13. Quasi-Static Analysis with Abaqus/Explicit

 

[jmetzy34]

Hi Compabaq,
Another solution to your problem is to run two analyses. Although you can't go from a static implicit step to a dynamic explicit step in one analysis, you can first run a static implicit job to get to your static pre-strained state. You'll need to make sure you request a restart file that contains at least the last frame of the analysis. Then you can import those results as an "initial state" using a predefined field. If you are using Abaqus/CAE see 16.11.11 "Defining an initial state field." If you are manually editing the input deck, when defining the part instance use:

*Instance, library=[job name of previous analysis], instance=[instance name]
**
** PREDEFINED FIELD
**
** Name: Predefined Field-1 Type: Initial State
*Import, state=yes, update=no
*End Instance

When you run the explicit job, make sure that all the files from your static analysis are in the same directory, most importantly the .odb and .res (the restart file).
Hope this helps.

 

[compabaq]

Thanks for the advice Mustaine3 and jmetzy34.