6
$\begingroup$

I am modelling my structure using FEM, and my structure contains line elements (1D) such as beams and columns and area elements (2D) such as walls and columns.

My question is that, how can I proceed to do modelling, and how can I interpret the results for stress and strain, especially at the places where 1D elements meet the 2D elements? Take for example,

  1. A beam's Center of Gravity might not be located within the slab, but in reality the beam and slab are still touching each other. In other words the beam is offset from the slab
  2. A wall's center of gravity might not be located within the slab, but in reality the wall and slab are still touching each other. In other words the wall is offset from the slab
  3. A beam and a column are supposed to be connected together, except that now the beam is offset in left and column in right. If going by line element, they are no longer touching, although in reality, they still are.

Is this a solved problem? Any research literature that I can refer to, or any software packages that you can recommend that handle this gracefully?

$\endgroup$
  • 2
    $\begingroup$ It would be helpful if you provided a diagram of the problem you are trying to solve. It is possible to connect 1D elements and 2D elements, but the elements must be joined at nodes. $\endgroup$ – OnStrike Dec 3 '15 at 7:42
  • $\begingroup$ @theNamesCross, I've changed the question to illustrate the point better. If this still didn't help, I doubt whether a diagram would. $\endgroup$ – Graviton Dec 3 '15 at 8:56
8
$\begingroup$

Say we have a slab supported on a beam.

Beam composite with slab

The centroid of the slab and the centroid of the beam are not coincident. Fortunately, in FEM software packages the geometric centroid of the element can be offset from the nodes that define the element.

The sketch below shows a case where the shells have been offset such that the nodes are at the bottom face and the beams have been offset such that the nodes are at the top face. This way, the section properties accurately reflect the true geometry but the shell and beam elements are able to share nodes (which is essential).

Extruded 3D view of beam with slab

Now for implementation. Most FEM packages should be able to handle this. I'm familiar with LARSA so my notes below are specific to that software package, but SAP, RISA, MIDAS, LUSAS, ABAQUS, etc. etc. etc. should have equivalent capabilities. Furthermore, there's likely quite a few different ways of solving this problem. What follows is just one of them -- just because it seems like some pictures might help.

Here's a wireframe and extruded view of a quick beam-slab model I put together. The plate elements and beam elements are shown at their centroids. Note that the plate and beam elements share nodes but their centroids are offset from one another.

Wireframe and Extruded Views

In this case, this offset was accomplished in two steps. The beam itself was defined using Section Composer with a geometry that places the node at the top face of the beam. Then, member end offsets were used to offset the top of the beam half the plate thickness downward. The plate elements are defined using nodes at the plate centroid so these two steps shift the beam geometry down so that the top of the beam is 'in contact' with the bottom of the plate.

Member End Offsets

Basically, look for something like "member end offsets" in your FEM package.

| improve this answer | |
$\endgroup$
  • $\begingroup$ (+1) Good answer- the pictures are worth 2000 words. $\endgroup$ – OnStrike Dec 3 '15 at 18:32
  • $\begingroup$ Out of curiosity, what software are your architectural views created with? AutoCAD (Visual Style: 'Sketchy')? $\endgroup$ – OnStrike Dec 3 '15 at 18:37
  • $\begingroup$ @theNamesCross -- I'll take that as a compliment. The top two figures are hand sketches. $\endgroup$ – CableStay Dec 3 '15 at 18:39
  • $\begingroup$ @CableStay, your answer made me ask a subjective question in the chat. Everyone else is also welcome to opine! $\endgroup$ – Wasabi Dec 3 '15 at 19:07
  • $\begingroup$ Definitely a compliment, they're beautiful.- Now if you could just fit in that box under my desk ;{) $\endgroup$ – OnStrike Dec 3 '15 at 19:07
2
$\begingroup$

A good FEM software package will allow the centroid of the geometric property to be offset from the mesh location.

For example, when modelling a beam and slab you may have the mesh at the top of beam/underside of slab level. The line elements then connect to the surface elements at the nodes (which should be fairly regular). The beam geometry will then have an offset of the distance from top of beam to centroid of beam (half the beam's height if it's symmetrical), while the slab will have an offset of half the slab depth.

| improve this answer | |
$\endgroup$
  • $\begingroup$ AndyT, do you have a reference on how this is done? Do you know any software that can do this well? $\endgroup$ – Graviton Dec 3 '15 at 8:15
  • $\begingroup$ And also, how does it handle the case when where the line elements are offset from the area elements? $\endgroup$ – Graviton Dec 3 '15 at 8:18
  • $\begingroup$ @Graviton - Firstly, a disclaimer: I work for a company called LUSAS, which owns/develops/distributes an FEA package called LUSAS. Secondly: LUSAS is very good at this sort of thing! The LUSAS examples manual goes through how to model line/surface element interfaces. [cont] $\endgroup$ – AndyT Dec 3 '15 at 9:33
  • 1
    $\begingroup$ [cont] With regards to offset line/area elements: LUSAS is able to connect them together with joint elements. But the key question is Why are the elements offset anyway? In my answer above I have stated that elements representing composite beams and slabs shouldn't be offset from each other - the elements should be coincident, and offset geometry can be used to offset the centres of gravity. $\endgroup$ – AndyT Dec 3 '15 at 9:35
  • $\begingroup$ lusas is able to handle the few scenario I outlined above? I have clarified the question after initial posting $\endgroup$ – Graviton Dec 3 '15 at 9:50
0
$\begingroup$

This mostly depends on your modelling software. You would definitely have nodes at your supports as well as at locations where you have point loads. For line loads you could create a mesh which has nodes exactly where features are. The line loads would then start/end at these nodes. Alternatively you can create a fairly dense mesh (250 mm x 250 mm aperture). On this you can distribute the line loads, adjusted as an area load per 1/16 sqm.

| improve this answer | |
$\endgroup$
  • $\begingroup$ I know about this, but my question is, how to handle all sorts of cases such as where the line elements are offset from the area elements? $\endgroup$ – Graviton Dec 3 '15 at 8:02
  • $\begingroup$ I am not entirely sure what you need. A sketch would be helpful. It sounds like it might help if you brush up on core FE theory. You need to have a logical connection between the various elements expressed as nodes or boundaries. $\endgroup$ – NamSandStorm Dec 3 '15 at 8:29
  • $\begingroup$ What I need is simple; how would one handle the intersection between 1D elements and 2D elements, especially if the the CG of the 1D element is not located within the boundary of the 2D element? So far the FE books that I browse through don't address this point at all. $\endgroup$ – Graviton Dec 3 '15 at 8:48
0
$\begingroup$

In general, for beams, I look not at the stresses, but at the bending moments (which they separate for the beams v. the panels). Then use s = Mc/I. Then I can offset for the beam off the panel stress.

| improve this answer | |
$\endgroup$
  • $\begingroup$ Mark, can you illustrate how exactly to handle the offset in your meshing/modelling of elements? $\endgroup$ – Graviton Dec 4 '15 at 1:00

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.