When defining a beam cast integrally with a slab I had initially thought the best way to do it would be to offset the beam down to correctly represent the true stiffness of the system. However upon seeing the results, I was puzzled as to the "saw tooth" shape of the bending moment diagram in the beams, and alot of membrane force in the slab.
After reading the following post http://forums.autodesk.com/t5/Autodesk-Robot-Struc
Left is no offset, right is offset to match slab level. Note saw tooth bending diagram on right.
Membrane force in local x, and panel cut of bending in x direction, overlaid on bending map.
So in the "no offset model" (left), I get peak beam hogging over the first support of 2320kNm, versus only 1485kNm in the centre beam on the right model with offsets.
My question is, which method of modelling produces results which are closer to "reality". I'm running the same system as a monolithic 3D volumatric element in the background as a comparison. I'll post stress maps when it finishes running.
Solved! Go to Solution.
Artur, yes I knew you would say that too ............
Well, I waited 1/2 an hour for my model to run and now I have some results from my 3d solid version;
I added 3 solid cuts, one along the edge beam centrline, one across the slab parallel to the beam, and one perpendicular to the beams.
First is x-direction. You can see that the slab midspan is in tension on the bottom and compression top
The entire slab is in tension all the way back past the first internal support. This disagrees with my previous post where the membrane force in the panel was zero for no bar offset.
So back to my original point. I understand that for design of the beams, it's far easier to make the simplification that they do all the work and the slab does none (in the beam span direction), then reinforce the beam accordingly. However if i was trying to really optimise the system and not reinforce over conservatively, can I assume that the slab takes some of the load in tension / compression. Is the real kNm value of beam hogging somewhere in between the saw tooth and the idealised "no offset" method, or should I be doing 3d models of everything that take 30 mins to run, and converting stresses into mm2 of reinforcement?
Thanks for your comments!
oh OK another sexy pic for you Artur
Tony, I'm sure the slab will take some tension /compression (due to bending) but you should display stresses for the top or bottom layer rather than in plane forces The in-plane forces for such model with vertical loads and linear static cannot occur in the model (mind that in the solid you have real heights of a slab (and beams) so that the top and bottom layers 'move' with respect to each other under vertical load whereas surface elements and bars are dimensionless in this 'direction'.
If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.
another edit hmmmm,
If I use the peak stresses above the 1st support on the edge beam (just picking rough numbers for this example);
4MPa tension, 12MPa compression.
I assume linear and triangular distribution of the stress in the edge beam (750 wide * 1200 deep) from top to bottom.
From the map it looks as if the zero stress point is somewhere above mid height so I guess 500 down from the top of the slab, (just guessing).....Then I calculate the following;
4MPa x 500mm x 750mm x 0.5 = 750kN
12MPa x 700mm x 750mm x 0.5 = 3150kN
(2/3 x 500mm) x 750kN + (2/3 x 700mm) x 3150kN = 1720kNm.
In my beam and slab model my edge beam had 1780kNm.
Now I'm really confused
Tony, please mind that the method with the use of arbitrary increase of beam moment of inertia (the decision what coefficient should be used is opened for discussion) is the approximate method I adopted for myself rather than the exact solution (a solid model ).
The solid model includes effects that are not the part of the shell one (real shapes of beams and slab rather than lines and flat surfaces that influence model deformation). The difference of 3-4 % seems to me the perfect result.
One more idea that I just came to my mind: modeling the slab you 'overlapped' part of the slab with beam ('double cross section') making this part more rigid than it is the the solid model. More rigidity -> larger bending
how can I get the moment of inertia option? See attached.
And how do you choose or calculate the factor (in your example 1.7, it is the total height / slab height?
Very interesting topic, tanks for you help.
It is clear now for the no-cracked behavor but how could it possible to design renforcement and control real deflection, based on this value ?
The TT floor is a good example. How to make a safe reinforcement design If the part of bending crossing among beams/slab is calculated with the non craked rigidity. What is the RSA method to take into account the rebar rigidity and cracks.
For this case I prefer to design manually but after, in general case of slabs and beams, how to determine modifiers on beam stiffness to render true calculations ?
I am a beginer on this kind of design so, to be safe when I design a floor where I canot said slabs are supported by beams, I use 2 models, one for the slab design, second for the beam design. Run reinforcement design on each one, adjusting the deflection insite beam modulus and slab modulus to make it compatible.
So complicated to do in reality.
Any solution ?
Log into access your profile, ask and answer questions, share ideas and more. Haven't signed up yet? Register
Start with some of our most frequented solutions to get help installing your software.
|AutoCAD Land Desktop|
|AutoCAD Plant 3D|
|AutoCAD Raster Design|
|AutoCAD Structural Detailing|
|Ecotect Analysis - Desktop Tools|
|Green Building Studio - Web-Based Service|
|Robot Structural Analysis|