## General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

#### Drop Test on Rollers

• Victor Silk
Subscriber
Hi again guys I have already posted a problem but now the same problem has to be solved differently - the box is dropped on rollers and the resulting deformation, stress, etc., have to be analysed. Since each rollers and boxare at different temperatures from the ambient conditions, I am unable to use Explicit Dynamics solver. So, when I tried using Transient, it went on for 7 hours and this message appeared - "internal solution magnitude exceeded". The rollers are supported on fixed frames and they are driven by gears. No video tutorial was I able to find out. Can someone please guide me with the proper steps? I'm in kind of a hurry for theories, sorry.
• peteroznewman
Subscriber

Hi Victor,

Different temperatures of bodies is no impediment to using Explicit Dynamics, but Explicit Dynamics is difficult to get useful results from. I would advise using Transient Dynamics.

What height are the boxes dropped from?  Did you calculate the impact velocity of the box with the roller? Once you have calculated that value, you assign that as an initial condition on the box, and you position the box at the point of impact, that is, just touching the roller.  That is the proper way to setup an impact problem.

If you setup the problem with the box at some height above the roller, the solver has to do a lot of useless computation moving the box down to the impact point.

• Bhargava Sista
Ansys Employee

Hi Victor,

The drop test is a short-time dynamic response so you may need to use a small time step, especially at the beginning when the contact is established. If the time step is not small enough, then the contact detection might fail and therefore the falling part might just fly through the rollers and therefore its displacement can increase rapidly (hence the error message).

Based on the initial gap (h) between the two bodies you can predict the time to initial impact (t = sqrt(2*h*g); g is the acceleration due to earth gravity). Make sure that the initial time step is less than the time to initial impact. This should help you resolve the error "internal solution magnitude exceeded". Also, you may want to increase the pinball radius under the details of the contact.

• Victor Silk
Subscriber
Thanks. That's very specific ?. The box is dropped from a height of 100mm. Is it possible to specify the exact time step, please? Sorry, but I'm not good at setting up transient analysis and I need to submit it by today itself.
• peteroznewman
Subscriber

Victor,

I expected you would calculate the impact velocity from the height.  Lookup the simple formula for uniformly accelerated motion. Lookup the acceleration due to gravity. I find most of what I want to know in a simple Google search.

• Victor Silk
Subscriber
Sorry and thanks petrezonewman, I have done the analysis using the initial velocity calculations and I have the results. It's just I would like to conceptualize the impact loading through the drop motion of the box to my professor.
• peteroznewman
Subscriber

Okay, did you position the box to be just touching the roller and assign the impact velocity to the box?  What impact velocity did you calculate?

If you use a 0.001 second initial time step, and simulate for 0.1 seconds, you can check that the contact was not missed.

• Victor Silk
Subscriber
V = 1.7155 m/s and the box is placed tangetially on the rollers.
Thanks for the time step tip.
• peteroznewman
Subscriber

V = 1.4 m/s for 0.1 m drop height for g = 9.8 m/s^2.

• Victor Silk
Subscriber
Sorry, actualy there are two 100mm and 150mm drops. Thanks anyway?
• Bhargava Sista
Ansys Employee

Victor,

As peteroznewman suggested, try to reduce the gap and define an initial velocity to save on computational time. You can use Newton's laws of motion to calculate the velocity. Also, to see if the contact is established during the solution, you can use a contact tracker to monitor the contact stiffness on the go. It must be a non-zero value when the contact is established. To do this, drag and drop the contact onto Solution Information and in the details of the Contact tracker, change the variable to max. normal stiffness. If you already have the simulation running, right click on Solution Information > Insert > Contact will insert a contact tracker. Then you can pick the contact of interest and start tracking the contact normal stiffness.

• Victor Silk
Subscriber
Thanks for the idea, bsista. Good to see people coming to help pretty soon on this site.