I want to model brittle stones in abaqus by brittle cracking behavior, but
my used mesh is a model known to lattice beam model and created by matlab (its image is attached) and in this model, materials are discretized in set of 3d beams and each beam fails if stress in it reaches to failure stress, and when
each beam fails, that beam remove from calculations. But my problem is that
in abaqus manual is mentioned that; we can't use 3d beams element in brittle
cracking and i get this error: The Abaqus/Explicit brittle cracking model
cannot be used with three-dimensional beam/pipe element(there is same disadvantage in concrete damage plasticity model too) . What is the reason
for that we can’t use brittle cracking with 3d beam element and is any idea
that i can model brittle material with that as satisfies the above
condition(removing a beam from mesh as soon as its stress reaches to stress failure?
Thanks in advance,
The short answer might be that it has not been implemented. The long answer says you that actually the model you are using does not use the Finite Element Method (FEM) but the Discrete Element Method (DEM).
As Abaqus is meant to provide a toolbox of algorithms for the solution of FEM problems, you are not able to implement a DEM problem in Abaqus out of the box. They have recently added a few features for the application ot the DEM method, but the user can use only spherical particles for the time being.
There is a workable option, though. You might well write an UEL (user element subroutine) and an UMAT (user material behaviour subroutine) using Fortran to implement your discrete beam elements model for brittle fracture in Abaqus. You will then be able to solve your model in Abaqus.
To know more about the DEM method and discrete beam models applied to brittle fracture, you can have look at the literature on the field, for example http://arxiv.org/abs/1509.00970 and http://arxiv.org/abs/cond-mat/0109231.
Luca
Thanks for your reply Luca.I thought about EUL and UMAT formerly but it is the last option for me. Is there any another constitutive model for that in abaqus that can uses with 3d beam element?or if i use another constitutive models too, this models cannot also use with 3d beam element?
The type of behaviour you're looking for is the one of cohesive elements. These in fact are elements that deforms until a criterion is satisfied; afterwards, fracture is assumed to have occurred and they are removed from the calculations. They are used to model delaminations and in general they model the two surfaces of a crack. Unfortunately, there is no built-in 1D cohesive element in Abaqus. Nor I think they can be meaningfully used with beam elements. Unfortunately, I think the only way is writing the UEL/UMAT routines, if you want to stick with Abaqus. I would be glad to help, if you think this solution could suit your needs.
What is application of UEL for me? I wrote a python code which creates mesh geometry for abaqus and i can assign beam element to that, i don't have any problem with meshing my model and my problem is only about constitutive model.Do you think i have to write EUL yet?
It depends on the constitutive model. If you write only an UMAT, your constitutive law must depend on the fields provided by the elements you choose. If your model uses fields that are not provided by a built-in element, you need to write an UEL. In your case, you want a failed beam to disappear from the simulation. To do that numerically, you need a specific variable (a boolean one, representing the state of the element, i.e. active or failed) which is not implemented in beam elements. It is for example a feature of cohesive elements, which, as a matter of fact, where initially developed as UEL by the researchers who created the model.
- Badges
- Science topic