Is it possible to simulate actual damage such as splitting? For example if I simulated a sheet of ABS that’s 1 mm thick, and got a 2 mm diameter sphere made of S420 steel, then over the time frame of 1 second it moved into the ABS by 100 mm, the ABS gets stretched to where the sphere is, instead of actually breaking. Is it possible to simulate this damage?
No, CalculiX doesn’t offer any damage modeling with element deletion (actual fracture). There are only simple crack propagation analysis procedures. But element deactivation is possible with *MODEL CHANGE, TYPE=ELEMENT, REMOVE. It’s just a step-wise element removal without damage criteria but maybe you could partially achieve your goal this way. It’s not available in PrePoMax so you would have to use the keyword editor.
This method seems similar to one I saw in Abaqus. In the video in field outputs it was made so that if the element has a certain level of stress or above it would disappear.
Abaqus has *MODEL CHANGE too but also built-in damage criteria based on which elements can be deleted (without the need for the model change feature). Johnson-Cook criterion is often used. CalculiX has the JC model in the newest version but without damage (only plasticity and rate dependence).
How would I implement the model change keyword? I’m not really sure how to use the keyword editor. Though this may be a question for a different topic.
I show its usage here: https://www.youtube.com/watch?v=MXrQBQH7Ecw
You just have to follow the CalculiX syntax described in the documentation: https://www.dhondt.de/ccx_2.21.pdf
there’s few of models in damage material for brittle with MFront, it seems none of ductile type. Someone create independently of Gurson Tvergaard Needleman 1982 (GTN) models, video and code links
Yeah, but this is only for the damage calculation without material (element) deletion. It seems that the OP is mainly interested in the element removal itself.
it’s frequently misuse between damage and fracture, separation means cracking due to fracture.
In Abaqus nomenclature, there’s material damage (stiffness degradation) leading to material failure (complete loss of load carrying capacity) and optional fracture if element removal is enabled. Damage is usually modeled as progressive damage with initiation and evolution criteria. Of course, there are also crack propagation simulations where element removal is not necessary to model the fracture (e.g. with XFEM).
This seems right. I’m interested in element deletion. For example the hole a bullet creates after penetrating a material. What I’m thinking is that if I can get the elements to delete if the stress is a certain threshold then it could create that kind of effect.
It should be possible to divide the analysis into multiple steps and manually remove the elements with large stress/strain values using *MODEL CHANGE. The problem is that you would have to run part of the steps, find those elements and include them in the model change definition. Restart feature can help with that (continue the partially completed analysis). I wish it was as easy in CalculiX as it is in Abaqus.
related to this, it seems CalculiX has better approach by generate of specific purpose of surrounding face between solid element connectivity instead of removing the solid element itself, but i’m not tried yet personally.
Are you talking about the way *MODEL CHANGE works in CalculiX or about a different functionality ?
crack growth analysis has been supported by CalculiX in later versions, it’s community contribution if i remember properly. I’m not clearly understand at all, only known behind the concept basically. Also, i did not know how to generate mesh of internal triangular face between tetrahedral element connectivity. Most of my case are in damage not fracture, so i did not yet go further testing these keywords feature.
Yes, fatigue (LCF or HCF) crack propagation based on the Paris law is available in CalculiX (and in Abaqus):
Though this still doesn’t allow a mesh to be broken up, correct?
It only predicts the crack shape and extrapolates the shell mesh of the initial crack. The structure in which the crack propagates doesn’t even have to be modeled.
well i read again, it seems the problem need to solve is look like ballistic bullet impact… i’m not sure CalculiX have capability to exploding the model, but OpenRadioss seems capable and the mesh need to be converted before.
That’s right. And OpenRadioss might indeed be a better choice. Also considering the explicit dynamics limitations in CalculiX.