## LS Dyna

#### Which analysis to use for dynamic and quasi-static compression of auxetic structures?

• YashIITD
Subscriber

I want to simulate the compression of auxetic structures under dynamic and quasi-static conditions. Which analysis systems should I use. Also kindly guide me through the process. Should I impart some force also or only velocity? Kindly help me.

I am using different kinds of auxetic structures like re-entrant honeycomb, S-shaped, star, etc.

I am using ANSYS Mechanical.

Thank you in advanced.

• peteroznewman
Subscriber
It can be done in Static Structural, as shown in this discussion:
https://forum.ansys.com/discussion/2522/defining-self-contact-in-static-structural
This issue is you have to create each contact pair manually.
If you do it in Explicit Dynamics, then all the contact is automatically found
• YashIITD
Subscriber
Yeah. This is exactly what I want to do. I even did it. But not sure if I used all the parameters correctly. Like what velocity should I use. Also should I apply a force?
Finally, my main goal is to calculate the absorbed energy and Specific energy absorbed. I don't know how to do that. Kindly help me with that too.
Also, it would be great if you can send me a screenshot of your parameter or if you have a video for the process of the whole simulation.
• peteroznewman
Subscriber
In Explicit Dynamics, you want to ramp the velocity up from zero to some value. If you apply an instantaneous velocity at t=0 then you are introducing a huge shock into the structure. Don't do that because it will create a lot of noise in the results. You can request the reaction force to the velocity boundary condition.
If you apply a force, it will create an acceleration on the mass. You must have enough mass to avoid creating a huge acceleration. If you don't apply enough force, the motion will stop when the resistance of the structure pushes back with an equal force.
There are several output results concerning Energy. You will have to do some research on this site. Others have asked this question. Here is a Google Search result for this question:
Unfortunately, the post that had a copy of this model did not get transferred when the site was upgraded.
• YashIITD
Subscriber

I've got my figure like this. I've attached a slab to my structure, and now I want to push it to calculate the absorbed energy - for both dynamic and quasi static cases. For quasi static I believe I don't have to give any velocity and only force. And for dynamic, I feel I have to give a velocity at t=0 only, along with a force.
You mentioned that I'll be introducing a shock if I apply some instantaneous velocity at t=0. But Suppose if the slab were at a distance, and then it started there and reached the certain velocity, then also it would have hit the structure with a velocity. And that velocity will be at t=0 locally for the structure. Isn't it? Correct me if I'm wrong.
Also, in analysis settings, there are so many setting as to what should be turned on and off, the number of steps, end time, energy error, etc. I tried many of those, but still not sure about the perfect combination.
I have to calculate for velocities 10 m/s, 20 m/s, 60 m/s.
Kindly help me with this too.
Thank you
• YashIITD
Subscriber
I also found this TYPE in analysis settings. Should I change it accordingly?
• YashIITD
Subscriber
Maybe if I can send you my CAD file in mail, you can try doing that and tell me how to do it. I have to submit it as a project and the deadline is in 2 days.
If that's okay, kindly drop me a mail at yashendra.mohan007@gmail.com
Thank you
• peteroznewman
Subscriber
Yashendra In Workbench, use File, Archive to save a .wbpz file and attach that to your reply, but use Clear Generated Data on the Mesh before you save the file to reduce file size.
You need to mesh with at least 4 elements through the wall thickness and it is better if you have more.
You can have a plate impact the structure at those three constant velocities, it will just create some noise in the solution, however, since you are plotting energy, that will average out over the structure.
Why do you need 3 velocities? It might not be possible to finish this project in 2 days.
• YashIITD
Subscriber
I have uploaded the file.
I was initially performing the compression without plate, but it was giving different results as to what we were performing experimentally. So I added the plate.
Also 3 different velocities for 3 different structures will help us compare which has better energy absorption at which stage.
So basically I'll have to perform simulation for dynamic and quasi static cases on these auxetic structures. I believe I can run the simulation and finish it before 2 days. But if you say it will take some more time, I believe I can take some extension. But I'm really excited for this project. It's just this part is new for me. Earlier I did my simulations in Autodesk, but they were not very accurate I guess. Also there we cannot get these charts to calculate the energy absorbed.
Thank you
• YashIITD
Subscriber
I've done simulations previously. But there are just way too many parameters here. I was taking 316 stainless steel for my structures and any other (e.g. Structural Steel) for the slab. I'm not sure about the various parameters in analysis settings, or in which way to use force. I used a constant one, but it just didn't give me the desired results, due to the resistance from the structure. So I made the force a function of time. But then I wasn't sure of the velocity. I've watched various videos too.
• peteroznewman
Subscriber
Attached is an archive where the first analysis system was edited and I ran if for a little while. The density was increased by a factor of 100 and the velocity is 5 m/s.
• YashIITD
Subscriber
Thank you so much!
• YashIITD
Subscriber
I too was using displacement, but I kept it free along X-axis instead of putting a value. And since I used actual materials instead of artificial, so I wasn't getting enough deformation.
So I was thinking, to find out the energy absorbed, should I use this contact energy in energy probe, and take the integral with time?
Or should I plot the stress-strain curve here and calculate the area under that?

• peteroznewman
Subscriber
Look at the Energy Probe results for the body being crushed.
Internal Energy = elastic strain energy
Plastic Work = plastic strain energy
Kinetic Energy = 1/2 m v^2
I don't know what contact energy is, you will have to do some research.
Note that in the file I attached above, I didn't make the density artificially high on the structure, only on the block.
I just ran a case at 50 m/s with 10 times higher density and it looks a lot smoother.
• YashIITD
Subscriber
Oh okay sure. Anyway thanks for your help. It kind of verified my results and now I'm a lot more confident of my results.
For the high density case. Maybe I'll just increase the dimensions of the slab to get more mass instead of increasing the density.
For energy absorbed by the structure contact energy made the most sense to me so I thought it might help. But I'll do some research. Thanks!

• peteroznewman
Subscriber
50 m/s result.