Hello, I’m working on my final year project about an impact attenuator and I’m starting with PrePoMax. To ensure the simulation is accurate, I’m redoing a dynamic simulation I saw in a scientific article.
The problem I’m having is that I run a simulation up to 0.01s, and it stops at 0.0029s. My theory, and my professor’s, is that my material is only undergoing elastic deformation, and when plastic deformation begins, the simulation stops. I don’t know if I’m configuring the material incorrectly or if it’s another simulation setting.
Case configuration:
Top plate (Will absorb the impact): 100 mm with 5 kg
Attenuator (Middle piece): 20 mm high and 0.075 mm
Image 1: FE Model
Image 2: Results
Image 3: My results graph
Image 4: Literature results graph
Please share the .pmx file and possibly also the title of the paper that you are replicating here. If you don’t want to share them on the public forum, you can contact me via private message (or I can reach out to you first).
Ok, so it’s based on the thesis “Otimização ao impacto de estruturas do tipo honeycomb via funções de base radial” by Matheus Toneli Rodrigues.
Why is the whole honeycomb fixed in all 3 translational directions in your model ? The BCs should be applied only to the rigid plates - one is completely fixed, the other one has U3 free and initial velocity applied in this direction.
Contact pair and tie constraints have only a few slave edges highlighted, but it might be a visualization issue (I’ve seen something like that before):
You are using the explicit dynamics procedure, so it should always converge unless you specify too high max increment size. Incrementation settings in this procedure are very important and I explained them here: https://www.youtube.com/watch?v=-X0Shj7UXE0
I have to warn you that the explicit dynamics procedure in CalculiX is currently underdeveloped - very slow and problematic. So I would consider using OpenRadioss instead for this kind of an analysis. Then you could get much closer to Abaqus analysis and even include some damage models.
Thank you very much for analyzing my case.
I hadn’t realized that I had fixed the honeycomb in all three directions, that was my mistake. I will change that and run the case again to see what happens.
And thank you for pointing out the limitations of explicit dynamics; I had no idea. If I continue having problems, I will discuss with my professor the possibility of switching software.
Your videos are very good, I carried out all the simulations based on them.
Thanks, I’m glad to hear that. I have experience with similar problems in Abaqus, so I can help you more via pm, e-mail or Discord if you want.
One of the worst limitations of this procedure in CalculiX is that rigid body constraints can’t be used with 2D elements, including shells (although, in ccx 2.23, they can’t be used this way even outside of explicit dynamics). Normally, I would advise you to apply rigid body constraints to the plates used to crush the honeycomb. Increasing the Young’s modulus is a workaround, but it affects the stable time increment, forcing you to use mass scaling more extensively (which should be done very carefully, especially in quasi-static analyses).
The plates are normally modeled as rectangular surfaces (not hollow cuboids). Make sure the mass is correct.
it’s look during impact the parts is in contact and meet shell element with knot exist, this can be problematic in CalculiX and recommended to use solid element.
Yes, it might be better to just use the Thicken Shell Mesh tool and run the analysis with solids having one or more layers. Shells can be very problematic in CalculiX, especially in nonlinear and dynamic analyses. Fortunately, they can be easily converted to solids in PrePoMax. The Thicken Shell Mesh tool doesn’t want to work on this honeycomb, though. It shows an error about non-manifold geometry. And indeed, there seems to be some overlap of the surfaces (they are duplicated). You should fix that in CAD software first.
I performed the simulation in two ways: using a solid model and a shell model, and both stop at the same time step, 0.0029 s. I sent you the shell model because, in the academic papers I researched, nearly all of them use this approach (although not in PrePoMax), so I assumed it was the most appropriate. However, I also have the solid model simulation available.
Indeed, normally shells are recommended and used in such cases. But in CalculiX, it’s often safer to use solids instead since shells are not true elements of this kind - they are internally expanded to equivalent solids. This expansion is nonlinear and very often causes issues, especially when combined with other nonlinearities (including nonlinear constraints such as rigid body) in the model.
If it still stops after the aforementioned corrections, have a look at the job monitor and see if there are any relevant warnings/errors. Also, have a look at the results at this time frame. Energy output is very helpful in dynamic analyses and allows you to track the progress of explicit dynamics run in CalculiX.
Still, I would probably just switch to OpenRadioss. There are even ways to convert CalculiX .inp files to its format and some simple preprocessing utilities for it.
