Dear Ls_DYNA experts,
Your advice on the following topic is appreciated!
I have a flexible slender tool made of beam elements, and I am interested in measuring the tip force of the device in contact with a surface (an automatic_node_to_surfcae contact type is used). I have used the nodfor output to read the relevant data. However, there are severe high-frequency oscillations in the output which distort the real data. I have already used a (15%) global damping keyword to reduce oscillations. What is the way to remove the oscillations and read the true data? Should I use another more reliable output to read the tool's tip force?
Hi ANA,
I will come right out and say I'm not exactly one of the experts 'round these parts, but I do have some suggestions.
To my understanding these sorts of issues can have a ton of reasons, the man himself answered a question about something similar a little while ago: https://feassistant.com/forums/hypermesh/how-to-reduce-oscillations-in-a-graphic/
If you hadn't read the post already. One comment suggested applying proper filtering and mentioning it in your discussions.
There are two things I wanted to mention were how timestep and/or more direct contact stiffness control can do a lot for these things. I didn't see this said directly in the dynasupport page for contacts, but there could be a benefit in reducing the TSSFAC in *CONTROL_TIMESTEP, or changing the SFS and SFM values in your contact card. These could be particularly important if you have dissimilar meshes if I remember correctly.
I'm not sure at exactly which time it is mentioned, but these videos go into it way deeper than I can: https://www.youtube.com/watch?v=NUDaiJgQ2CA&t=1477s
I hope some of that helps!
It is better to think more generally than a particular code (LS-DYNA, in this case). "Oscillations" are inherent to explicit analyses because the explicit code solves the governing equations as a wave propagation problem. So, when you apply an external load or BC, it has inertia associated with it (thanks to conservation of momentum F=dp/dt or F=ma for point masses) which creates a pressure wave that travels through the domain (your mesh that is connected to the site of load/BC application). That wave bounces all over the medium and those reflections show up as oscillations - in part. [Imagining 1D first is easier, before imagining 2D and beyond].
The oscillations also arise due to the fact that, often times, we do not specify any material damping. So, a numerical pendulum will continue swinging forever after an initial nudge (except that there is numerical dissipation of energy so it will slow down but that's another matter).
Finally, there is another subtle source of oscillations in explicit schemes and that is there are no force residual or displacement norm or energy checks (as you do with an implicit scheme). So, the explicit code (think bullet train) simply charges ahead in very tiny steps (in the hope that that is good enough and the solution makes physical sense).
Notice I did not bring up LS-DYNA or any other explicit code for that matter. If you are solving governing equations with an explicit scheme, oscillations are something you just have to get used to.
Now, and this is your real question: how do you know which oscillations are real and which ones are just numerical "noise"? That will come from your understanding of the frequency content in the forcing function (external load/BC) and the natural frequencies of the system you are studying (eigenvalues). If you have a structure connected to a base that is vibrating, then you do not want the structure to have natural frequencies close to that base vibration because resonance could potentially destroy the structure. By the way, resonance need not be bad; there are situations where you want good energy transfer where "resonance" is helpful. If you know that loading frequency is a small fraction of the natural frequency of the structure (say, in a quasi-static analysis), then all you need to is filter out the oscillations using a favorite low-pass filter.
Thanks for the complete reply. I could reduce the oscillations significantly by adding global damping around 10-15% of the critical damping.
Hi @ana,
@icebreakersours is laying down some fundamental FEA advice. A lot really comes down to your understanding of what "should be normal" in your case. And that will come from reading and experience.
Now to applications. You can try adding viscous damping (VDC) to your contact instead of global damping. This is usually a better first approach then applying global damping so that you don't negatively affect the other parts of your simulation that might be performing perfectly fine. I've used VDC=40 in the past for certain situations.
From the help page below:
https://www.dynasupport.com/tutorial/contact-modeling-in-ls-dyna/contact-parameters
"Viscous Damping, VDC (Card 2, *CONTACT_option)
The viscous contact damping parameter, VDC, on card 2 of *CONTACT is zero by default. Originally, contact damping was implemented to damp out the oscillations that existed normal to the contact surfaces in sheet metal forming simulations. It has been found that contact damping is often beneficial in reducing high-frequency oscillation of contact forces in crash or impact simulations.
Viscous Damping Recommendations
In contacts involving soft materials such as foams and honeycombs, frequent instabilities exist due to contact oscillations. Using a value of VDC between 40-60 (corresponding to 40 to 60% of critical damping), it is found that the model stability improves; however, it may be necessary to reduce the scale factor for the time step size. Generally, a smaller value of 20 is recommended when metals, which have similar material constants, interact."
Alternatively, forces from contacts can be so varied depending on the type of contact, parameters, or the entities that you are using in the contact (segments vs parts vs nodes etc). So something else you can try is to take your force directly from the bean that is contacting the surface using elout. This thread might help explain how to set up *Database_history_beam so that you can access elout data.
https://feassistant.com/forums/ls-dyna/database-functionality/
Glad to know.
You can reduce damping in a few ways - as long as you understand the reasoning. Is global damping of up to 15% appropriate? I cannot say but you have to understand the implications of the option you have chosen.