I often need to analyse frames/chassis made from mainly square hollow tubes. Ive used beam elements in proprietary software, and that had been good. I know calculix doesnt allow for much more than solid square/circular beam elements.
I wonder what my options are to get a good working model through Calculix, despite the abive .
My apologies. I was under the impression that CalculiX had that limitation, from reading different posts about the limitations of CalcluliX. Im excited to learn that beam elements with square hollow sections are added.
Iāve been warned about bugs concerning the general section option. Can anyone clarify what these bugs are, and whether they can be avoided?
hello,
beam elements are internal expanded into volumentric elements.
the connection between beam elements are limited. Between translation and rotational,
or only translation (truss-elements) or only rotation.
I have recently been experimenting with custom made beams in CalculiX.
Reading the documentation, I founded the āOffset1ā and āOffset2ā parameter which virtually allows the user to build any desired shape, build composite beams or reinforce just some specific areas of the beam.
You just need to overlap as many elements as rectangles you need to build your custom profile.
Once all the material properties are defined, Offset to position of that rectangles properly to build the new beam section.
I have made an IPE160 with this technique. Iām still working on this so take it carefully. Be sure to test your new beam performance , displacements and stresses as it needs more refinement than a conventional beam to get good results.
B32 elements has shown to perform the best in my case.
If you try Pipe or BOX and you later see a solid section in the postprocess it is ok.
āNotice that, internally, PIPE and BOX cross sections are expanded into beams with a rectangular cross section (this is also the way in which the beam is stored in the .frd-file and is visualized in the postprocessor. The actual cross section is taken into account by appropriate placement of the integration points).ā
I posted some days ago on the MECWAY forum (look up to the end). It can be run in the free version.
It also has a preliminary pdf report on the displacements for different mesh refinements and elements. I will add the inp on the post but I can not warranty it works. As I commented before some inp files generated by Mecway do not work for ccx users, not sure why. Let me know if it doesnāt work and I will try to fix. Shear ZX Stress show some discontinuities in-between elements that dissapear with additional refinement.
this approach has been cited for so long and itās similar to layered shell element by duplicating, but did not recommended since it will generate knot and over stiffening the models.
not recommended does not mean to be restricted and given warning in the solver running.
bellow i copied from manual documents,
The offset of a shell element can be set on the SHELL SECTION card. Default is zero. The unit of the offset is the local shell thickness. An offset of .5 means that the user-defined shell reference surface is in reality the top surface of the expanded element. The offset can take any real value. Consequently, it can be used to define composite materials. Defining three different shell elements using exactly the same nodes but with offsets -1, 0 and 1 (assuming the thickness is the same) leads to a three-layer composite.
However, due to the introduction of a knot in every node of such a composite, the deformation is usually too stiff. Therefore, a different method has been coded to treat composites. Right now, it can only be used for 8-node shells with reduced integration (S8R) and 6-node shell elements (S6). Instead of defining as many shells as there are layers the user only defines one shell element, and uses the option COMPOSITE on the SHELL SECTION card.
Ok. shells and beams expands in similar ways.
The oļ¬set aproach descrived in the manual to construct beams of nearly arbitrary cross section should be used carefully.
Not sure what do you mean sorry. I hope the example is useful to you.
As Xyont has confirmed, this assemblies requires a bunch of nodes to get reliable results but, not recommended doesnāt mean it is restricted.
i known before when reading an articles from STRUCTURE Magazine by Arturo Montalva, P.E., Jeff Baylor and Klaus Wittig (Oct, 2010)
right, i did several test with many section type in the past and found a questionable results in condition near the support, member intersection, stress distribution etc.
i have checked the example,
very interesting. i have checked the buckling modes.
I prefere to work with beam cross-section created with solid elements.
how you fix the boundary, if you use a U-cross-section?
in connection with gravity and shear center!?