Error in shell forces calculation using layered shells 1

[ugoveri]

I am using SAP2000 10.0.1, but have tryed versions 10.0.7 and a beta version of SAP2000 v11...

I tried to model a very simple square slab, working as a one way slab, and so having supports only on two parallel sides

The dimensions are not relevant...

I tried 2 situations:
- simply supported (lets call solution 1)
- with full bendind restrain in both sides... (solution 2)

For each of those I tried:
- a regular thin-shell with the concrete shell design option (solution ".a");
- the new layered shell option (solution ".b");

A very strange thing happened...

While for the models 1.a and 1.b the results where both similar around p.L^2/8 (being p the load, and L the span), for the models 2.a and 2.b the results where quite different...

For the model 2.a the result as expected was around p.L^2/12 at the supports and p.L^2/24 at the span.

For the model 2.b the result was around p.L^2/24 at the span, but more or less 67% of p.L^2/12 at the support...

How can one trust such a result... Everybody knows that if you use a thick-shell model (which takes account for shear deformation energy, Mindlin model) the results come slightly different from those using kirchoff theory of thin plates... But that difference is related to the relative distribution of the stresses, but the overall difference between the support and the span has to be around (p.L^2/8)...

And with the layered shell model it wasn't... It was a terrifying discovery...

Of course, besides this, the reinforcement is well calculated... But having a wrong force distribution as base...

So be carefull with your models... If you use the regular concrete design for slabs, you are assuming some king of simplification - the force in the steel is calculated by:
- Fbottom = + M/z + N/2
- Ftop = + M/z + N/2,

assuming M as positive and being:

- z = h - h1 - h2;
- h the overall depth of the slab;
- h1 e h2 - the distance from top or bottom of the slab to the bottom or top reinforcement centers;

It gives probably a slightly bigger area of reinforcement as it should but for thin shells it gives more or less good results, and even because it is calculated based with the right forces...

If you use the layered shell model, the results are supposed to be correct in what concerns to reinforcement area, but because they are based on a stress distribution which isn't correct it should not be trusted...

Would be great if someone would pass this information to CSI... I tried to send several information in the past, but it seems you are speaking to a wall

 

[stressed]

Hi, I copied your post on an email to CSI technical support because I was curious about it, and I had a problem to ask them about on another matter. When they replied to my problem, they also gave this reply to your post which I will copy & paste for you below in italics:

The layered shell element is lower order for plate bending than is the thick/thin shell (layered is quadratic, thick/thin is cubic). When you have only a few elements in a span, the layered shell is more sensitive to support conditions. For the fixed condition (his/her solution 2), 6 to 8 elements in the span is recommended. My guess is that he/she is using 4 elements. For the simply-supported condition (solution 1), 4 elements is enough for either element type. The quadratic formulation for the layered shell is really very good, but adequate meshing is required. Meshing is easy enough using automatic meshing options.

 

[ugoveri]

I was modeling a square plate with 4 by 4 m and using a mesh of 0.5m which means dividing each side by 8...

And 4 meters is an intermediate and more or less common span... And 0.5 is a more or less usual size for the mesh...

I used a slab height of 16cm because if one just made a preliminary dimensioning we would probably be led to a height of 13-14cm... 16cm would maybe had some transverse force behavior...

Anyway they should warn you of such a difference... If I got reasonable results with the same mesh for the regular (old) shell formulation, one should get similar results, if not they should warn you...

To be reproducible I used the following... with kN/m/C

Concrete: E=30e+6 kN/m2
poisson=0.20
fc=30000 kN/m2

Rebar: E=200e+6 kN/m2
poisson=0.30
fy=500000 kN/m2
fu=550000 kN/m2
fye=550000 kN/m2
fue=605000 kN/m2

The self weight isn't relevant since I used 0 as the self weight multiplier...

The slab used had 16cm of height for bending and axial behavior...

For the layered shell, I used the previously mentioned materials disposed like:

Concrete: distance=0
thickness=0.16 (with 2 integration points)

Rebartop1: distance=0.05
thickness=0.000785 (equivalent to 10mm diameter with distance between bars of 10cm)

Rebartop2: distance=0.05
thickness=0.000785

Rebarbottom1: distance=-0.05
thickness=0.000785

Rebarbottom2: distance=-0.05
thickness=0.000785

The slab is 4x4m2 and is restrained on the x borders to the following displacements: u1,u2,u3 and r1

I tried meshing 8x8, 16x16, 20x20 and 24x24...

load: p=10kN/m2
span: L=4m

The results were:

M22-(kN.m/m) 8x8 16x16 20x20 24x24
Exact(*): p*L^2/12=13.33 (without shear deformation energy)
Standard: -12.90 -13.08 -13.09 -13.10
Layered: -8.62 -10.80 -11.26 -11.57 (signals come swithed)

M22+(kN.m/m) 8x8 16x16 20x20 24x24
Exact(*): p*L^2/24=6.67 (without shear deformation energy)
Standard: 6.77 6.61 6.59 6.58
Layered: 6.15 6.47 6.50 6.53 (signals come swithed)

(*) It will not match exactly because only with a poisson coefficient of zero we would get the same result as if it was a beam...

Note1: The shear forces V23 comes vry similar for both...

Note2: Standard is using shell-thin formulation...

Note3: Another creepy result is that although the absolute results of the moments are correct, the signal is switched when using layered shells... So the positive moment comes negative and the negative comes positive!!!

Just by curiosity if one used the shell-thick formulation the results would be M22+=6.58 and M22-=-13.12...

As you could see, the standard solution gives you more or less accurate results for a common used mesh (0.50mx0.50m) while the layered shell solution only gives you a rough match with the 24x24 for the negative moment... And I don't imagine anyone using a mesh of .167mx0.167m in a building, unless on a very particular situation...

And with this I am not blaspheming SAP2000... It's a good program... the offices where I work or have worked used it and in general I like it... But this black box type results (with almost no help or tutorials), without any explanation gives me the creeps...

Best regards. Can you send this also? Because it seemed you had quite fast access to CSI... It takes a bit longer here...

 

[ugoveri]

Ah! One other thing, I got alarmed, when trying to model a simple building situation and comparing the results... On top of a column there was almost a 50% difference in one case... So as you can imagine, is quite difficult to believe such a result... I mean If the positive moment come bigger, one could say there was some kind of relaxation...

If there was something that I always liked about SAP2000 is that, at least for elastic analysis, the forces are the forces, and the design is the design... So the layered shell should be used (at least while on elastic analysis) only to dimension the area of reinforcement... The forces should be the same no matter which model you used... You should choose between shell-thin, shell-thick, plate-thin or plate-thick and then, if you chose an extra option of layered shell you would be able to design the reinforcements...

If you mix it like this one starts to become suspicious about the results...

As far as I am concerned if I can't trust those results in simple models, how can I trust them in more complex models where you can't of course get exact or close aproximations by hand to compare?

Best regards.