

May 1, 2024 at 12:43 amAli KomaieSubscriber
Hi, I am modeling a 3D object that is part of a hollow sphere which radius is 7.8 mm and its thickness is 0.536mm. From the side view, it makes a circular arc equal to 120 degrees. It is made of a linear elastic material with E = 0.3 Mpa. At the top vertex, a chain of steel spheres sits on this object, and their displacement is limited to the Y axis. The bottom corner face of the object is fixed and a constant pressure of 2400pa is applied on the interior surface of the object.
At first, I did a Static Structural analysis to find deformations related to gravity and the constant pressure, and then I wanted to do an explicit analysis for an impact through the chain using Ls Dyna for about 1 millisecond. Even though everything is the same for the Ls Dyna analysis, the curved object starts oscillating. I have used dynamic relaxation for Standard Earth Gravity and also option "Both" for Dynamic Relaxation Behavior of applying the pressure. So the oscillation amplitude is not too large according to the scale of the whole model. However, It is enlarging over time, and even this small oscillation will significantly affect my final results since I need high accuracy. Two attachments show the oscillation. The image below contains a graph showing deformation of the top vertex of the curved object. Why at the beginning of the Ls Dyna analysis, its deformation suddenly reduces from 0.0573mm (which is the result of the Static Structural analysis) to 0.055024mm and then gradually goes up again?
To solve the oscillation issue, is it a good idea to use an Ls Dyna Restart analysis for the impact after the Ls Dyna analysis and reduce the first Ls Dyna analysis end time from 1 ms to 0.2 ms to have the minimum oscillation amplitude before the impact (This approach significantly increases the ansys file size and I don't know why!?)? If not, what should I do to completely dampen this oscillation?
Also, I should mention that since I need to measure Nodal Contact Force through this analysis, my only option is to do a 3D analysis in Ls Dyna. 
May 3, 2024 at 3:06 amReno GenestAnsys Employee
Hello Ali,
The problem here is that you are using the Ansys solver to find the static equilibrium position under gravity and constant pressure and the LSDYNA solver for the explicit dynamics impact simulation. The Ansys solver and the LSDYNA solver are different solvers with different element technologies, material models, etc. and so results with the same mesh may differ a little bit between the 2 solvers. So, the static equilibrium position of 0.0573mm that you find with the Ansys solver is probably a little bit different if you were to do the same implicit static simulation in LSDYNA. In many cases, the difference in solution is small and acceptable for many applications. But, in your case, it seems you are looking for more accuracy.
So, one solution is to find the static equilibrium under gravity and constant pressure using Dynamic Relaxation in LSDYNA. This way, you would use the LSDYNA solver for both the static equilibrium and the explicit dynamicsÂ impact. This way, you should minimize the oscillations that you observe. You can do explicit Dynamic Relaxation which uses the explicit solver and some sort of damping to damp out the vibration and find the static equilibrium position. Explicit Dynamic Relaxation (DR) will usually result in some oscillation left at the end so so Explicit DR may not be the best approach for you. You could use implicit Dynamic Relaxation in LSDYNA which uses the implicit solver in LSDYNA to find the equilibrium position. This should give a result similar to the Ansys Static Structural solution. Note that Dynamic Relaxation (DR) in LSDYNA occurs before time zero such that the model is initialized with deformation and stresses at time=0 due to the applied load (gravity and pressure) during the DR phase. You will find more information about DR here:
https://ftp.lstc.com/anonymous/outgoing/support/FAQ_docs/preload.pdf
You can do Dynamic Relaxation in Mechanical using the Dynamic Relaxation object:
You will need to have only one LSDYNA system in the WB project schematic. No need for Static Structural or LSDYNA Restart:
Â
Let me know how it goes.
Â
Reno.
Â

 You must be logged in to reply to this topic.

456

205

194

177

162
Â© 2024 Copyright ANSYS, Inc. All rights reserved.