Simle plate problem 1

[sasa2k]

I am trying to get accustomed with STAAD and I started with simple plate 15 cm thick, dimension 5x5 m fixed on all four sides.

I used concrete for material (E=21700 N/mmsq, Poisson 0.17) and plate has quad division of 10x10.

Results I obtain above supports are not very similar with theoretical and results from another programs.

Moment above support is Mx=0.796 kNm/m what is significantly less than theoretical result (1.30 kNm/m). In AxisVM and SAP2000 I got 1.27 kNm/m

In the middle of plate I got Mx=-0.49kNm/m, which is more close to theoretical (-0.525).

What is wrong?

Thanks.


Version: STAAD Pro 2004, WIN2k

 

[sasa2k]

I forgot load: 1 kN/m sq

 

[Lutfi]

sasa,

Keep in mind that STAAD applies/transfers loads at the supports and or nodes only. The more elements you have the better are the results.

Be careful using STAAD concrete design!! I would use it to obtain moments and shears and then select reinforcement manually. Trust me on this one. I use the plate rebar selection only to verify and check my manual selection.

This may come as a surprise to many fellow engineers who use STAAD, it does not size rebars for weak axis bending!!! only for gravity and torsion.

Good luck


Regards,
Lutfi

 

[RAYC1]

You are looking at the element center stresses. The element corner stresses would be a better location for comparison. The STAAD element center stress resultant, in this case, is -.529 kN-m/m. The STAAD element stress resultant at the center of the edge is 1.147 kN-m/m. These results are closer to what you are looking for.

Other reasons for differences in results between programs are:
(1) There may be a difference between the shell theories (thin shell theory or thick shell theory).
(2) There may be a difference in the the number of nodes per element.

STAAD uses thick shell theory [a 4 node, hybrid, thick plate element].
AxisVM and SAP2000 may be using thin shell theory.

STAAD uses 4 node elements.
The elements chosen in AxisVM and SAP2000 may be 8 or 9 node elements.

A test was run using 4 node, thin plate theory elements and the STARDYNE option in STAAD, the result at the center of the edge was 1.224 kN-m/m. This 6% higher stress tends to show that the thin shell theory stress result is higher than the thick shell stress result.

The elements chosen in the other programs (AxisVM and SAP2000) may be higher order (8 or 9 node) elements. If so this would explain the remaining difference (1.224 versus 1.27).

 

[sasa2k]

Rayc, you are right, I was looking at plate center stress table and color legend to identify max moments. Plate corner stress table gives the same max moment as you got 1.147 kNm/m.

Since I am doing concrete design manually, I need maximum stresses and forces.


BTW in Axis I used plate element (eight/nine node) suitable for thin and thick shell, and in SAP I used 4 node thin shell.

Thanks for both answers.