FEM analysis on flat slabs peak top moment extremely high 5

[BST-98]

Good day,

When modelling a flat slab with columns in the middle to create column strips, the top moment is extremely high (the peak moment increase with smaller mesh size).
Comparing this to running a beam strip as a column strip the moments are more realistic (but way less than FEM analysis) and this is what I design for, I guess my question is how do I get FEM to give me the same answers as modelling in FEM software is more time efficient than doing manual strips in a flat slab.

For reference I'm using Robot Structural Analysis.
If anyone has any literature on this that would be great as well,
Thanks in advance

 

[Celt83]

If I remember correctly the FEM solution will trend to infinity at a point support.

Robot has an option to smooth out the moment in these locations, it’s called something like reduce peak moments. Have also seen recommendations to add rigid links from the column center out to the column perimeter to locally stiffen the area.

Robot doesn’t provide any shortcuts to any of these modeling techniques and panel cuts for column middle strip need to be done manually as well. You might be better off using something like RAM Concept or CSI SAFE.

 

[KootK]

..how do I get FEM to give me the same answers as modelling in FEM software is more time efficient than doing manual strips in a flat slab.

You don't. Taking the high localized stresses from FEM and converting them to the values typical of design is usually a matter of post-processing the results. That, regardless of whether it's you doing the post processing or a software package like SAFE or ConcePT doing it for you.

Our design methods for concrete slabs rely heavily on the ability of those slabs to redistribute bending stresses laterally. There are limits to how much redistribution is appropriate and those limits can often be found in you governing concrete design standard. Too much redistribution can result in excessive strain the reinforcement.

 

[JoshPlumSE]

I guess my question is how do I get FEM to give me the same answers as modelling in FEM software is more time efficient than doing manual strips in a flat slab.

If I remember correctly the FEM solution will trend to infinity at a point support.

Yes, this is a common difficulty with FEM modeling of slabs. My thoughts (based on my past involvement in the development of structural analysis and design programs):

1) This happens because a place "force" isn't really a force it's a force per unit width. Right? So, if the slab connect to a column at an infinitesimally small joint, the force per unit width at that joint is infinity. Right?

2) The most basic way to account for this is to average the plate force over a representative width. Below is a link to a manual section that I wrote back when I worked for RISA. It discusses how an engineer might choose this "representative design strip width".

https://www.risa.com/risahelp/risafoundation/Content/Slabs/Slabs - Design Strips.htm

3) Another thing you can do to help is to make it so that the slab is rigid in the region where the column exist. By that, I mean you can create rigid links that connect from the column center node out to mesh point at the corners of the column. Essentially spreading out the connection so that it distributes over a wider area. Not perfect, but it genuinely helps.

 

[BST-98]

Thanks a lot for the input

 

[Tomfh]

That’s how FEM works. You have to average it out across a sensible strip width.

We tried to use ROBOT for a few years however eventually rejected it in favour of more usable software.