Abaqus => Calculix, generalized plane strain

[gsal]

Hi, everybody...long time Fortran supporter, first time FEA poster.

I do computer program support/development; for the present task, the engineers are using Patran/Abaqus combination for meshing, thermal and structural analysis...very slowly. The desire is to carry out some optimization by running many processes (in parallel?) at a time triggered by a single user, let alone others working on similar things...but we just don't that kind of numbers in licenses!

So, somebody tasked me with replacing licensed software with "non-licensed" one, in other words, open source.

I have looked into the inherited Patran-mesh files that are produced for Abaqus and have been able to have Salome produce a mesh that can be solved by Calculix for the thermal analysis; but, for the structural analysis, there is this thing called the "generalized plane strain" element that they use in Abaqus and I don't see it in Calculix.

Does anybody know if it is possible in Calculix to setup an element to behave like the "generalized plane strain" element in Abaqus?

Any hints greatly appreciated.

gsal

 

[corus]

Generalized plane strain is a 2D element that allows out of plane strains to remain constant. As far as I'm aware Calculix doesn't do 2D elements however if the 2D elements of your model were extruded out of plane (in the Z direction) by a single element to form a 3D shape then the same effect could be achieved by coupling all of the nodes on the extruded plane to a single node on that plane so that the UZ freedoms were equal. In Abaqus the equivalent command would be achieved using the *equation card. I don't know if Calculix does the same.

The opposing surface to that of the extruded surface would also be restrained in the Z direction so that for all nodes UZ=0.

Under a thermal load, for example, thermal expansion in the Z direction would be allowed for the extruded plane but the strains would all be equal and the extruded plane would remain parallel as it expanded.

 

[gsal]

corus:

Thank you very much for such a quick reply.

There is some learning ahead as I don't do mechanical or FEA analysis for a living, but your answer gives me hope; it sounds like it is possible.

I posted this question ahead of looking into the inherited Abaqus input file thinking it may take some time before anybody replies; so, I am not yet familiar with what the model looks like and how it is loaded. To be sure, I should have a working Abaqus model which I then need to tweak for use by Calculix and attempt what you suggest...at the end, if it works, I should get the same answers.

With the thermal case, I was very, very surprised to get the same temperatures for every node from both Abaqus and Calculix...but I digress...

As you yourself said it, Calculix does not seem to do 2D elements; even the (shell) S6 element that I ended up using for the thermal model seems to turn into some kind of brick or wedge and a 1-element thick "2D" model...at least, this is kind of how I understood it.

So, for as long as Calculix plane strain element CPE6 is already a cube, couldn't I simply create a 1-element thick "2D" model and do as you suggested? Or do you think I may need to let the model be 2, 3 or more elements thick for some reason? to capture something?

Thanks again and looking forward to your reply.

gsal

 

[corus]

You don't need 2, 3 or more elements through the thickness as there's no variation of stress in the out of plane direction. Of course what you could do is create a model that had a significant thickness in the out of plane direction as plane strain conditions relate to an infinite thickness of material. If you applied no boundary conditions to either face in the out of plane direction then the results you'd get would be plane stress (zero out of plane stress) at the free surfaces, and approximately plane strain conditions at the centre plane of the model (constant axial strain across the section). This is a more expensive alternative to just applying appropriate boundary conditions to a single element, given there are no 2D generalised plane strain elements in calculix.