I am looking to model a collision. Although the structure I want to model is completely different, a real-world intuitive example might be a car's rear-end with bumper backing into a rigid brick wall. I have looked at the PipeClip.liml example. It has most of the requirements I will need including Nonlinear 3D, frictionless support and contact elements. I see it uses displacement = f(time) to move the parts together. I would like the movement function to be based on F = ma. IOW, set an initial speed and mass and let the reaction with the brick wall to slow the "car" down to a velocity of zero. I would need to gather accelerations, max stresses during the interaction. The "car" would be geometrically non-linear. It would not necessarily get into buckling, but would be great if that could be modeled also.
Is there some way to mimic this scenario?
Thanks.
Comments
The more powerful way is to use Nonlinear Dynamic Response 3D as the Analysis type. But there are a couple of limitations:
Another way, if you don't need dynamic effects like vibration, might be to use Nonlinear Static 3D treating the model as being in the object's accelerating reference frame. The deceleration would be a ramped Gravity load pressing it against the wall.
Thank you for replying. It's been a long time since we last traded messages (2014). I couldn't recover my old logon and thus created this one. No real loss... I might as well be a different person.
Let me elaborate on what I want to achieve. I will be sharing my work on this thread as I go along, so I'm not trying to hide the actual model. For now, I just think anyone that has been near a car understands the concepts intuitively of car bumpers. Probably first hand. There are three phases that are common.
I want to design my part in this 1st phase. I will iterate the design (mostly geometrically) to achieve the highest initial velocity without permanent damage. I won't design for a phase 2 component and the onset of phase 3 will most likely occur due to buckling.
I think the Nonlinear Dynamic Response 3D sounds like it will fit the bill to handle the analysis determination of the deceleration forces. The two caveats you mention: the spreadsheet work and initial velocity doesn't sway me. What I thought I had to do is far more intensive.
Although I'm not concerned about the vibrations, I am trying to wrap my head around how to use the results (stresses, boundary forces, etc) of the finished large deflection state at zero speed to feed into another analysis to predict onset of structural failure due to buckling. I know this type simulation is possible https://youtube.com/watch?v=_HpSaFSnQoY, but I'm unsure of how much is built-in to FEA programs and how much has to be handled outside the program... and more importantly... how close I can get with Mecway and what steps I need to perform outside of Mecway either with spreadsheets or even programming.
CCX allows you to chain several analyses together in steps which sounds like what you're asking for.
But I don't think you need to do that because nonlinear dynamic response already includes buckling and plastic deformation. You may also have to add some imperfection in the geometry to ensure buckling initiates if everything is too symmetrical. You can add additional contacts on areas where you anticipate self-contact might occur.
As far as your problem, while I have not done it, in both actual physical tests and computer modeling for bridge and roadway rail tests a pendulum arrangement is often used to generate the contact velocity. Bogies are also used, but they require modeling of functioning wheels, winches, etc.
In rock fall modeling, which I have done in the deep past, gravity can be used directly with a sliding or rolling rock on a slope.
Please keep this forum posted on your progress as you are quite a bit ahead of me and I find the advice here useful, especially for similar problems, as well as any sample input provided to see how the problem was coded. Fortunately I won't be needing self contact, but I expect you will for higher velocities. There is a fair amount in our crash tests of cars and PU trucks.
If your mesh is sufficiently fine to capture the buckling modes of interest, and you include nonlinear (elastoplastic, for example) materials, then in my experience buckling behavior will be accurately represented.
Expect to need *much* smaller timesteps than you might predict. Best to set them as something something like the time for the "car" to move 5% of an element length, and set this as a max time step or the implicit nonlinear solver will struggle with capturing the collision. You can adjust once you get things running.
Just a few thoughts. Good luck!
-Robert