Quasi-static Cyclic Analysis with ABAQUS/Explicit

[g.alshamsi]

Hey everyone, I'm running some quasi-static simulations using ABAQUS explicit on a steel shear wall assembly containing 10 parts, my work is basically divided to verifying two experiments, a static pushover and a cyclic experiment. So far I'm getting somewhat acceptable results for the pushover simulation however I have some concerns regarding the cyclic test:

1) How should I define cyclic loads? In the pushover simulation I used the SMOOTH amplitude function to define a displacement load equivalent to the max displacement in the experiment. To ensure minimal inertia effects, I performed a frequency analysis and then applied the displacement load over a period equal to 50*fundamental frequency. Using this procedure I was able to keep the Kinetic energy below 5% of ALLIE and had an acceptable solution time (12hrs). So my amplitude definition was:
*Amplitude, name=Smooth, definition=SMOOTH STEP
0., 0., 12., 100.

I would like to follow a similar procedure for the cyclic simulation, however I'm not sure about the amplitude definition. Lets say for the case of simplicity that I have 5 cycles with the following amplitudes, 10,-10,20,-20,50. Should I define 5 separate steps with 5 different smooth functions for each step? If I do that, do I divide the total time of the simulation (in my case 12 seconds) equally over 5 steps? So the 1st two steps would look something like:
*Amplitude, name=Smooth_1, definition=SMOOTH STEP
0., 0., 2.5, 10.
*Amplitude, name=Smooth_2, definition=SMOOTH STEP
0., 0., 2.5, -20. and so on...

Not sure if I'm following a logical procedure or making my life more complicated, any input from more experienced users would be greatly appreciated.

2) What is your general mass scaling strategy? I'm fairly a beginner when it comes to Explicit finite element so I'm following the manuals recommendations where I run a series of analyses with different fixed mass scaling factor and simply monitor the KE output. A colleague of mine suggests uniformly scaling the mass to meet a target stable time increment, however I'm not sure about how I can do that given that manual calculations for stable time increment are approximate at best.

Thanks for reading, if anyone is wondering why I'm using explicit rather than quasi-static implicit solver, it's because I ran into several convergence issues using the implicit solver due to geometric/material nonlinearities and complex contact conditions.

 

[FEA way]

In Abaqus/Standard you have direct cyclic procedure meant for such scenarios but in Explicit it's necessary to use combinations of amplitudes and multiple steps (the concept of steps is very useful in such cases).

When it comes to mass scaling, usually fixed version is used, with scaling factor or target increment. After the analysis you should check the ratio of kinetic and internal energy to make sure that the simulation is still quasi-static, as it should be.

 

[AndresBM]

1) As FEA way says you need to use combinations of amplitudes and multiple steps. In your case I would suggest to create 5 steps if you have 5 cycles. You can use the same smooth step amplitude if defined with "Step time" (not "Total time").

2) The uniform mass scaling is ok if your inertia effects remain small and you get acceptable calculation cases. This is not always the case, and then you want to use the nonuniformly mass scaling to not get such large inertia effects. You have to consider that with the uniform mass scaling takes the most conservative factor from the most critical element, so it might be too much. I personally use the nonuniform option more often.

It would be interesting to know the convergence issues with the Standard solver. Maybe is worth solving the issues than fighting with mass scaling and explicit.

Andrés

annelysis GmbH | Engineering Excellence |

https://annelysis.com

 

[g.alshamsi]

Hey, thanks for the reply.

1) Yup that's the procedure that I'm following, I'm defining a separate step for every cycle and using the smooth amplitude to prevent sudden jerks in accelerations.

2) So far the uniform mass scaling is working as I'm able to keep the KE below 5% of ALLIE with an acceptable computational cost.

Regarding the convergence issues, I'm not really sure where the problem lies. The model contains several non-linearities and multiple contact conditions in addition to several connector elements to simulate screws.I tried several approaches such as using different dissipation levels/damping/relaxing the convergence criteria and using the unsymmetrical solver without any results. That's what made me jump to explicit.

 

[FEA way]

In such cases convergence issues are usually caused by contact and switching to Explicit helps because it’s better at handling highly nonlinear, difficult contact conditions. In Standard you can try changing the type of contact (pairs vs general contact). This often helps.

 

[g.alshamsi]

That was my initial guess. I've been using contact pairs since my models is an assembly of shell parts (with a few solid elements) so defining contact surfaces and making sure the surface normals point in the correct directions is pretty straightforward. I haven't tried the general contact approach with Standard yet. I'll give it a shot sometime soon and I'll report back if I get any good results.

Cheers,

 

[AndresBM]

I always recommend to add nonlinearities step by step, so you exactly know where the issue lies. Putting all complexities at once is a recipe for nonconvergence.

Although with a good review of results and convergence behavior you can have a good feeling where the problem is. If you share more information as pictures or output files we can check it further.



annelysis GmbH | Engineering Excellence |

https://annelysis.com