Projectile Collision

mog

I'm attempting to model how a panel deforms over time due to the impact of a projectile, this is a simple version of what I'll eventually be modelling but I figured I'd start off with an less complex model. To be more specific I'm trying to simulate a bulletproof shield. The final model will use a much smaller projectile and a panel made up of many thin layers, (not too sure how this would impact the elements I should use, potentially by layering shell elements? For now I've just used Automesh 3D on a thin-ish cuboid). The goal is to model the point of failure and then simulate again using lower energy impacts.

Values for material properties and forces will be changed, just stuck some numbers in for now whilst I'm trying to get things started.

I've been fiddling round with it and going through tutorials from the manual but I can't seem to get the two objects to interact. I've used ABAQUS in uni before and have a basic understanding of FEA software but I'm a bit rusty so it might just be a simple solution that I'm overlooking.

I'm also using the free version, so I only have 1000 nodes to play around with right now, however if I can get something working then I'll definitely be wanting to upgrade so I can properly refine the mesh and get some better results. Just gotta convince my boss that it will be a worthwhile purchase.

Any pointers in the right direction would be much appreciated

kennethfugate

Search for "Explicit Analysis" or "Bouncing Sphere" in the forum for some impact examples.

Victor

Contact stiffness is so low that it looks like they aren't interacting. Units are Pa/m but should probably be GPa/m.

You can set the entire surface of the plate as contact face instead of a patch in the middle.

JohnM

I think I've posted this before, but couldn't find it, so here it is (again I think):

Think small - small models, small time steps. Model sizes can grow after things start making sense.

Very stiff models are hard to run/converge. Run a modal analysis on your system to determine the time step requirements. For example, if your first mode is 1000Hz, you probably want a time step of 1/(10x1000).
The first mode in your test model is about 4000Hz, pretty "stiff", and requires very small time steps to characterize anything but the very first responses.

Use gravity.

Use an initial velocity through custom model definition, this can be the impact velocity and the model can be moved a small distance from impact.

Lately the PASTIX solver works great, but if there is an issue always check by using PARDISO.

Learn how to use Ralyeigh Damping


Attached is a drop test test model that should give you some guidance.

Video of drop test:

https://drive.google.com/file/d/1YoOZL2CkIpOp4VWZYrkHO1ogdi1oV8IQ/view?usp=sharing

mog

We have contact!

Getting back into FEA has had me really scratching my head but I've managed to make some progress on this model. Still got a way to go but I'm definitely getting a better grasp of Mecway and how it differs to ABAQUS.

~~~~~

kennethfugate, I found some impact examples and made the following changes.

- Turned automatic time stepping on with no lower bounds and restricted upper bounds. (Smallest maximum time step seemed to be 0.0001, smaller than this resulted in solver errors)
- Set up model at moment of impact instead of letting projectile travel through empty space
- Added gravity
- Suppressed all stresses whilst playing around with any changes

~~~~~

Victor, I set the whole surface to contact face instead of a patch in the middle. Initially, I did actually try this before posting but changed to the small patch after reading in the manual (page 61) where it states that:

"The surface with the larger area should be the master. If the slave surface overhangs the edge of the master surface then slave nodes which are too far from the edge won't be connected. However a small tolerance of about 4% of an element face's width in its in-plane direction is allowed. Slave nodes within this distance of the edge of a master face are still connected."

Since the projectile is obviously smaller than the panel, I just used a central patch for the 'Impact Zone' but I changed it back after reading your comment.

Not too sure what the optimum value for this would be but the highest I seemed to be able to run it without the 'too many cutbacks' error was 1000GPa.

~~~~~

JohnM, you're a saint! Found another one of your comments when searching for 'Explicit Analysis' (https://mecway.com/forum/discussion/comment/7094). Some of the advice I followed I commented on in my response to kennethfugate.


Do I need to download any additional software to use the PaStiX solver? Just reading the ccx documentation about the *DYNAMIC step, it says I need to download the solver. I attempted using the below text in the custom model definition but there are too many unknowns for me right now to fully understand where I'm going wrong. How does this look....

*DYNAMIC,ALPHA=(not sure what value to use),EXPLICIT,SOLVER=PASTIX
1.E-4,0,1.E-3

Do I need to include details about materials, node locations, element types... or am I able to just input the values as above?

Also, please could you instruct me on how to run a modal analysis or let me know where I can find out more about it?

~~~~~

I think that covers everything for now, thank you everyone, really grateful for the community on here.

mog

Just in the middle of running the solver again but I'll post the updated file when it's done

mog

Here is the file

JohnM

Use the Pastix solver, available pre-compiled on the Calculix website ( the "files" link). Link to the ccx_dynamic.exe executable. You can use the CCX solver switch to change to Pardiso if necessary.