Learning Forum

[Andres.Mena]

Hello all!

I am currently developing a wrist model. Following other authors modeling techniques I plan to perform a static simulation. I am new with LS Dyna so I would appreciate some suggestions and general guidance on how to do this.

I previously worked with Abaqus (standard which uses an implicit solver) in which I had the option to enforce a static case by using a keyword and then define a "dummy time" for the load to be applied. I guess the time wasn't really important there because it was a static case.

Within LS Dyna, however, I am not entirely sure what I should do. I am aware that LS Dyna uses an explicit solver by default. I noticed that the results change considerably depending on the time I choose to simulate in *CONTROL_TERMINATION and the curve load defined in *DEFINE_CURVE (a ramp curve together with *LOAD_NODE_SET). I am not sure if this is right so I started exploring the implicit solver since I saw that I can use a static option. So my questions are:

• Can I use both explicit and implicit solvers to perform a static simulation or is there a preferred option?
  • What kind of parameters should I choose for an implicit solver?
  • If possible with explicit (what I have done so far), what variables do I need to check so that this simulation represents a static case or at least a quasi-static one? What about the time I need to simulate until the results stop changing?

Thanks, 

Andres

 

[Andreas Koutras]

Hello Andres,

With the implicit solver you can run a purely static (or a quasi-static dynamic) analysis, while with the explicit solver you can run a quasi-static analysis if you apply the loading sufficiently slowly. For the solution to be considered quasi-static, the kinetic energy in the part of interest should be only a small percentage of the part internal energy (say 5%). The energy components of each part are available through *DATABASE_MATSUM.

Guidelines for implicit analysis including a checklist are available here:

https://www.dynasupport.com/howtos/implicit

[Armin]

Hi Andres,

To add to what Andreas provided, you may also find the course below helpful for explicit analysis:

Explicit Dynamics Theory - Ansys Innovation Course - YouTube

[Andres.Mena]

Thank you so much for your replies! I will check these keywords and the course mentioned.

One question though, what did you mean exactly by applying the load sufficiently slowly? Are there any recommendations to apply loads like step functions or something similar?

[Andreas Koutras]

A linear ramp can be used (in the *DEFINE_CURVE refererced by your loading keyword) to gradually increase the load from zero to its ultimate value. The kinetic energy can be used as the criterion to determine whether the ramp duration is sufficiently long in order to avoid significant dynamic effects, as mentioned above.

[Andres.Mena]

Hello! A follow-up question... what is the difference between the energy values provided in *glstat and *matsum?

I checked the kinetic energy vs internal energy in *glstat (which I guess would be total energy sum) and the kinetic energy is indeed less than the internal energy, but in *matsum this is not the case.

I am using a lot of discrete elements to represent ligament connections (see picture for reference) and I guess this is why I get total energy higher than the kinetic one, but all the remaining parts containing solids or shells have kinetic energy higher than internal energy in *matsum... I suppose this means that I need to simulate a longer time? Or is the *glstat total energy enough for confirming quasi-static behavior?

[Andreas Koutras]

Hello, I would judge based on the kinetic over internal enery ratio in matsum for the parts of interest. 

[Andres.Mena]

Thank you so much! I will do that. By any chance you know why the kinetic energy of the discrete elements is so low compared to solid and shell ones?