I am doing a case study comparing the fundamental period of a 20-story reinforced concrete building with dual system in both directions and compared the results from SAP 2000 and Midas Gen. The reference building is from the book of SK Ghosh Seismic Design using Structural Dynamics. here is the link of the book http://secure.skghoshassociates.com/product/show_book.php?isbn=9781580017485.
The example problem in the book is solve by the author manually and the modal analysis was done using SAP 2000 and I wanted to verify the accuracy of the result by comparing them with midas gen and staadpro, Midas Gen result is very close with the book's output within 1 to 2 % difference however, staadpro output is way off, Here is the tabulated result,
In Section 18.104.22.168.3 of the Technical reference manual, there is an example shown for considering the PDELTA effect during dynamic analysis. It says that if you provide the commands in that sequence, the frequency will be calculated using the [K+Kg] matrix.
Also, I don't have that book that you are referring to. Can you attach the pages of the book describing that example, and the STAAD model?
The P-delta KG analysis is the one I used in the staadpro analysis and I'm well aware of this analysis. I already posted this before that Etabs, Sap and Midas Gen have been using P-delta with Response spectrum analysis for quite a long time. This has to be implemented because ASCE 7-05 section 12.9.6 has specific requirement that modal response spectrum has to be analyzed together with P-delta. I also remember you did ask me how are those program doing it since the output from RSA are all positive values after the modal combination like CQC, SRSS etc are done.
It can be done as explained in the book of Wilson which is also the technical reference used for Etabs,Sap and Midas Gen by incorporating global geometric stiffness KG into the global lateral stiffness K (K +KG) which is now also implemented by staadpro using P-delta KG analysis. The difference with the implementation between Staadpro and Etabs or Midas Gen for that matter is that the last two has an added parameter called P-delta load combination in which that particular combination is used to calculate the initial p-delta analysis in order to derive the geometric stiffness to be incorporated into the succeeding analysis. By doing this the P-delta analysis is actually being linearized and superposition method can then be applied. That is why in Etabs or Midas gen combinations can be done after the analysis because you do not need primary load cases (repeat load) anymore for the combination simple load combination will do. This has been shown by raycxx of Bentley support in one of his posts here where he used load combination for P-delta KG. This is just not properly documented in Staadpro.
Is there any method in Staad by which one can know whether the net support reaction generated due to Response Spectrum analysis is positive or negative i.e. upward or downward?
Please make another thread for your query so that you can not destruct the good arguments here. It is not belong to the topic presented. You are acting like a student are you???
thanks for the clear explanation Kris
Can you share the explanation friend from kris. Tnx!
Kris will post a detailed explanation here for the benefit of all staadpro users.
As we do not have a copy of this book in our office, here are some aspects to pay attention to when modeling such structures.
1) Floor slabs
To simulate the high in-plane stiffness contributed by floor slabs, many programs have a rigid diaphragm feature. In STAAD.Pro versions V8i SELECT series 3 and older, this is possible using the command SLAVE ZX MASTER aa JOINT slave-joint-list. When a frequency and mode shape extraction is involved, it is important to set the master node to a point that is at or very close to the center of mass of the weights that are assigned to the slave joints. The farther the master node is from the center of mass, the more approximate the results will be.
Depending upon the complexity of the floor plan, the center of mass can be tedious to calculate. So, this method of assigning a rigid diaphragm can be tedious. There are 2 workarounds.
a) Model the floor slab using plate elements, even a coarse mesh should be OK. Make sure that the elements connect to all joints (beam ends) of the floor. To ignore the bending stiffness (as in the case of rigid diaphragms), declare the elements as PLANE STRESS. As plane stress elements have no out-of-plane shear or bending capacity, make sure every plate node is attached to a beam or a column, else there will be instabilities along FY. To simulate the inplane rigid effect of the slab, assign a modulus of elasticity that is say, a 100 times that of concrete. In this method, one doesn't need to worry about the center of mass. The stiffness and mass distribution are automatically reflected in the respective matrices.
b) If you have STAAD.Pro V8i SELECT Series 4 (Build 20_07_09_11), there is a feature called the RIGID FLOOR DIAPHRAM. Using that, all the nodes of a floor can be declared as being part of a rigid diaphragm. During the analysis, the program finds the center of mass based on the weights defined at those nodes and creates a master node at the center of mass. The engineer doesn't have to manually calculate the correct position of the master node.
For complex floor plans - L-shaped, Z-shaped, etc., method (a) is still probably more accurate.
2) Doubly symmetric structures
If the stiffness and mass are identical along global X and Z, the frequencies and participation factors should reflect that. This will be evident in the form of pairs of modes with identical values for frequencies, and transposed values for the mass participation factor and base shear (in a response spectrum analysis). However, in those pairs, the mode shape and participation factors will not necessarily be entirely in one direction alone, but will be at an angle to (and hence have a component along) both plan directions. In the example below, modes 2 and 3 form a double root mode, and, modes 5 and 6 form another.
In each pair, for any given direction, some mass participation is from one of those double root modes and the remaining participation is from the second mode in that pair. So, both modes in a pair must be used together, which means, the participating mass, base shear, etc. must be added up from those two. Thus, in the example shown, the mass participation factor along X for the first double root mode is equal to 72.52 (contribution from mode 2) plus 1.43 (contribution from mode 3), = 73.95%.
Both modes of the double root mode should be used in the response spectrum or time history solution. For example, if the 8th and 9th mode are double root modes, the CUT OFF MODE SHAPE value should be at least 9, not 8 for a response spectrum analysis.
Whether a certain software reports double root modes or not depends upon the solver it uses for eigensolution. If the engineer wants the response to be entirely in one direction alone, he/she can
i) Make the seismic weights along the X direction to be marginally different from those in Z. This will cause the frequencies and participation factors for X to be slighty different from those for Z, but the variation should be small. Hopefully, each mode will be for a specific direction only.
ii) Apply the masses along one direction only. If you apply them only in X and none along Z, the participation for the lateral modes will be fully in X and zero in Z.
3) PDELTA effect
raycxx has pointed out in the following thread how the geometric stiffness can be considered during the eigensolution.
We will elaborate on this either through a new discussion in this forum or through a Q&A on the STAAD FAQ page.
Here is the final result of the case study that I am doing. Staadpro yield a close agreement with SAP2000 and Midas Gen.
SAP 2000 3D MODEL MIDAS GEN 3D MODEL STAADPRO 3D MODEL (Plate Modeling Method) MODE PERIOD MASS PARTICIPATION PERIOD MASS PARTICIPATION PERIOD MASS PARTICIPATION1 2.485 71.2% 2.418 72.19% 2.390 72,94% 2 0.659 14.8% 0.658 14.19% 0.657 14.24%3 0.300 6.1% 0.308 5.98% 0.316 5.87% 4 0.178 3.1% 0.184 3.16% 0.200 2.76%
I am still exploring the orphan node method in staadpro, I believe the plate modeling is more accurate.
Many thanks for the explanation Kris.
The images below are coming from Midas Gen and Staadpro,