What is a static implicit solution scheme in Abaqus?

[StructuralCivilFEA]

I am reading about explicit and implicit solution method in Abaqus, and for the purpose of what I am doing the paper recommended using a static implicit solution scheme. Which step would that be? Because its not gonna be dynamic explicit or implicit step? - if so which one is it, and how does one go about applying the loads?

 

[FEA way]

Abaqus offers two main solvers - Explicit and Standard. First one utilizes explicit time integration scheme and is used to perform dynamic simulation (it can solve quasi-static problems though). Second one utilizes implicit time integration and is more versatile - it can perform both dynamic and static simulations. Dynamic analyses with this solver are done using dynamic implicit step (it can solve quasi-static problems too). Static analyses are done using static general step (or static linear perturbation if you want to assume strict linearity).

So you should use general static step for your purpose. That’s the most common type of step in Abaqus. In this case step time is not a physical time but some artificial measure used for load incrementation.

 

[StructuralCivilFEA]

A colleague of mine told me that I need to apply load very slowly if I am using static implicit solution scheme? Do you know what he could have meant by that?

 

[FEA way]

He was probably talking about static simulation done with dynamic implicit solver (quasi-static). In such case sudden load application would cause significant inertial effects and thus invalidate one of the main assumptions of static analyses. With general static step it won't be a problem since this procedure doesn't include inertial effects anyway.

 

[StructuralCivilFEA]

And if I have to apply dynamic loads (time history loads) on to my model, can I still use general static step?

 

[FEA way]

You can use amplitude in static general step to vary loads based on this artificial time measure. Real time (in implicit dynamics step) will be necessary only if you want to include inertia effects.

 

[IceBreakerSours]

Every once in a while I find an excuse to go back to the basics so here we go:

Firstly, with regards to the underlying mathematics, there are a few methods to solve governing partial differential equations and numerical analysis is one of those methods. Although there is a wide spectrum of methods, there are two major classes of schemes: implicit and explicit. With the exception of the finite difference method, the governing PDEs have to be reformulated in a way suitable for a given method (e.g., finite element or finite volume or immersed boundary .. .. method). In principle, either implicit or explicit scheme should give you the exact same result (simply because you are solving the same underlying set of equations). In practice, that rarely happens and one is forced to choose one or the other class of methods to numerically solve a given problem. Software vendors working on real problems from some industries end up coming up with their tweaks on their specific implementation of versions of these methods. Abaqus/Standard (implicit) and Abaqus/Explicit (explicit) are two major commercial versions from Simulia. Abaqus/Standard lets you choose to disregard inertia (static analysis) or take it into account (implicit dynamic, as one example). So far, I did not bring up any particular physics (elasticity, fluid dynamics, electromagnetics, etc.) in this discussion.

Now, to the physics, as part of a tall pile of approximations one makes in a numerical model, inertia may play little role in a specific phenomenon of interest perhaps because, say, the natural frequency of the structure is too high compared with the loading frequency. In such a case, you may want to perform a static analysis or a pseudo/quasi-static (using either implicit dynamic or explicit scheme) analysis. In the former case, physical time has no meaning and the "time" simply is a proportionality constant for the external load/BC being applied i.e., at "time" = 0, no load is applied whereas at "time" = 0.5, 50% of the load/BC is applied. In the quasi-static case, time carries meaning and inertia comes into play.

To reiterate, in principle, whether you choose Abaqus/Standard static analysis or Abaqus/Standard implicit dynamic (with quasi-static) analysis or Abaqus/Explicit, you will get the exact same answer. However, depending on the model, it can be anywhere from straightforward to a daunting task.


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

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

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