Square hollow section chassis

Hello there,

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 .


as documented in page 129, circular hollow (Pipe) and rectangular hollow (Box) are available


CalculiX offers the following types of beam sections:

  • elliptical
  • circular
  • pipe
  • rectangular
  • box
  • general

The last one is an arbitrary section which is defined by specifying section constants.

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.

I’ve been warned about bugs concerning the general section option. Can anyone clarify what these bugs are, and whether they can be avoided?

1 Like

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.

This bug still persists: Problem using U1 element (general beam section)

But the dev will likely take a look at it in the near future.

Hi Tor,

I have recently been experimenting with custom made beams in CalculiX.

Reading the documentation, I founded the “Offset1” and “Offset2” 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. I’m 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.

“Notice 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).”


hello disla,
is there a possibility to share your example. I’m very interested in beam calc.,
it would be a awesome
wbr dichtstoff


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 doesn’t 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 it’s similar to layered shell element by duplicating, but did not recommended since it will generate knot and over stiffening the models.

Thanks Xyont,

That’s good to ear. This approach is descrived in the manual without any warning (ccx 2.20 pag 648):

“The offset can take any real value and allows to construct beam of nearly arbitrary cross section and the definition of composite beams.”

I will review the forum to find out the citation.

During my first tests I have noticed the method has its limitations and that’s why I recomend to check carfully the beam performance first.

Additionally, from the manual too, U and C shapes could be build from the BOX beam setting thickness of removed side to cero.

When you say this approach is similar to layered shell elements, ¿do you mean you don’t recomend to use layered elements neither?

what do you want to have for result?
or what are your intentions?

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.

This is for shells. I’m using beam elements.

right, did your beam not expanded and works in similar ways?


Ok. shells and beams expands in similar ways.
The offset 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 doesn’t 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!?

right, as CalculiX taken advantages in uniformity of the solver. even though still required many test to validate and improvement the codes.

A bit of caution. Beams have a variety of bugs so you have to tread carefully. For instance:

  • A rotational DOF constraint on a transformed node of a beam can act in the wrong direction.
  • A rotational DOF constraint on a beam can cause incorrect external force.
  • Some components of external force can be missing.
  • Stress at constraints can be unrealistic. Refine the elements.
  • Section forces on elements connected to non-beam elements can be (are always?) wrong.
  • Concentrated loads create spurious local stress and deformation of the cross-section. Again, use refinement.
  • A truss connected to a beam can disconnect itself in some configurations.
  • A truss connected to a shell can constrain the shell’s rotation in some configurations.
  • Inhomogeneous boundary conditions can cause incorrect stress.
  • Velocity appears as 0 on some nodes for dynamics.
1 Like