RESPONSE SPECTRUM MODAL ANALYSIS

The member loads have been defined correctly. The only thing you need to do is to move the loads ahead of the spectrum data. A modified file is attached. There is a difference in base shears when the member loads are included vs when they are not, which is one of the ways to confirm that the member loads are being considered for the mass calculation.

Good morning,

I have adjust STAAD Model introducing in the correct order different load case with the aim to consider, in seismic calculation, also non structural loads, as reported below:

LOAD 4 LOADTYPE Seismic  TITLE SEISM X

*

SELFWEIGHT X 1

SELFWEIGHT Y 1

SELFWEIGHT Z 1

*

MEMBER LOAD

5 6 13 14 21 22 29 30 UNI GX 2

5 6 13 14 21 22 29 30 UNI GY 2

5 6 13 14 21 22 29 30 UNI GZ 2

*

MEMBER LOAD

5 6 13 14 21 22 29 30 UNI GX 1.8

5 6 13 14 21 22 29 30 UNI GY 1.8

5 6 13 14 21 22 29 30 UNI GZ 1.8

SPECTRUM CQC X 1 ACC DAMP 0.05 LIN

*

0 2.483; 0.154 2.541; 0.463 2.541; 0.551 2.137; 0.639 1.844; 0.726 1.621;

0.814 1.447; 0.901 1.306; 0.989 1.191; 1.077 1.094; 1.164 1.011; 1.252 0.941;

1.339 0.879; 1.427 0.825; 1.515 0.777; 1.602 0.735; 1.69 0.697; 1.777 0.662;

1.865 0.631; 1.952 0.603; 2.04 0.577; 2.128 0.553; 2.215 0.532; 2.303 0.511;

2.384 0.477; 2.464 0.446; 2.545 0.419; 2.626 0.393; 2.707 0.37; 2.788 0.349;

2.869 0.345; 2.949 0.345; 3.03 0.345; 3.111 0.345; 3.192 0.345; 3.273 0.345;

3.353 0.345; 3.434 0.345; 3.515 0.345; 3.596 0.345; 3.677 0.345; 3.758 0.345;

3.838 0.345; 3.919 0.345; 4 0.345;

*

LOAD 5 LOADTYPE Seismic  TITLE SEISM Z

SPECTRUM CQC Z 1 ACC DAMP 0.05 LIN

*COMBIBATION

0 2.483; 0.154 2.541; 0.463 2.541; 0.551 2.137; 0.639 1.844; 0.726 1.621;

0.814 1.447; 0.901 1.306; 0.989 1.191; 1.077 1.094; 1.164 1.011; 1.252 0.941;

1.339 0.879; 1.427 0.825; 1.515 0.777; 1.602 0.735; 1.69 0.697; 1.777 0.662;

1.865 0.631; 1.952 0.603; 2.04 0.577; 2.128 0.553; 2.215 0.532; 2.303 0.511;

2.384 0.477; 2.464 0.446; 2.545 0.419; 2.626 0.393; 2.707 0.37; 2.788 0.349;

2.869 0.345; 2.949 0.345; 3.03 0.345; 3.111 0.345; 3.192 0.345; 3.273 0.345;

3.353 0.345; 3.434 0.345; 3.515 0.345; 3.596 0.345; 3.677 0.345; 3.758 0.345;

3.838 0.345; 3.919 0.345; 4 0.345;

1- Is it correct to defined for SEISM Z only the response spectrum without introduce SELF WEIGHT AND THE OTHER MEMBER LOADS?

2 - If I want to define rigid diaphragm, which procedure is better to follow? In particular, considering the attached file, I have introduced FLOOR DIAPHRAM specifying the floor level and selecting also MASTER NODE. Running the analysis, STAAD calculates in the output section, only the coordinate of the centre of rigidity but there are no information regarding centre of mass. How can I obtain these results?

I have tried to define masses through REFERENCE LOADS DEFINITION, an error message occurs “REFERENCE LOAD CASE OF TYPE MASS/GRIVITY/DEAD/LIVE IS DEFINED FOR MASS MODELING. CENTRE OF MASS CALCULATION IS NOT POSSIBLE”. How can I solve this problem?

If I introduce Mass as references loads, is it still necessary to define SELFWEIGHT and MEMBER loads as load cases before RESPONSE SPECTRUM INPUT DATA?

3 - In STAAD file attached, I have changed some beam size (at the first and second floor), and, running the analysis, I noticed that, while z-coordinates remain the same because in Z – directions the structure, at each elevation, is symmetric in term of stiffness distribution, in X-direction, X-coordinate change, not only for the first and the second level, where I have modeled two beams with different geometry, but this modification affects also results relating to X-coordinates of the thirds and the fourth elevations, where, in my opinion, the structure is symmetric in term of stiffness distribution (all the beams and all the columns have the same size). How is it possible to explain this results?

 4 - if I want to assign torsion moments due Shift in Position of Centre of Mass and Centre of Rigidity, and combine these actions with seismic loads, how can I operate?

Thank you, regards

Silvia

3733.Response_Spectrum_Analysis.std

For a custom response spectrum, there is no automatic way to account for the accidental eccentricity. This is what you can do. Use the SET PRINT 17 command before the JOINT COORDINATES in your input command file and the analysis output file would then report the story forces at each level of the structure ( These are referred to as Floor Modal Base Actions in the analysis output file). These forces are reported for all the modes. To get the force at each story you may use a modal combination method like SRSS. This has to be done manually and once you have the shears at each story level, you can multiply those by the 5% eccentricity value at each floor to compute the accidental torsion. You can create a separate load case for the accidental torsion and use load combinations to combine that load with the seismic loading.

Thank you for the quick answer. 

Once SET PRINT 17 command before the JOINT COORDINATES and run the analysis, in the output file is report the story of the forces at each level of the structure ( indicated Floor Modal Base Actions ). Which procedure I have to follow if I want to get the force at each story with modal combination method like SRSS manually?

What do you mean?

Do I have to calculate the square root of squares sum of Floor Modal Base Actions, for each story per an eccentricity of 5% (obtaining in-plane torsion moment about Y-axis) through for example excel sheet and then insert these single actions combined with the seismic ones?

Is it possible to find shear output forces at each level in the output file?

How can I apply in-plane torsion moment due to eccentricity of 5% in the FE model? Is there a specific command in STAAD?

When floor diaphragm is included, the torsion due to eccentricity between CM and CR is already accounted for in the analysis, but if I have insert in the FE model my torsion moments due to 5% of eccentricity, the ones calculted automatically by the software have not to be considered. How can I exclude these ones?

Regards, 

Silvia

4478.Response_Spectrum_Analysis.std

Yes you have to calculate the square root of summation of squares of the floor modal base actions to get the story forces at each level. There is no direct way to get the story forces reported in the output file for a spectrum loading. You can get that for equivalent static seismic load generations. The accidental torsion moments can then be combined with the seismic loads as indicated in my last post ( put those in a load case and then use load combination). The 5% eccentricity torsion moment that you are talking about is accidental torsion and this is different from the torsion that accounts for the eccentricity between the CM and CR ( inherent torsion). If you have a rigid ( or semirigid) diaphragm then you would have to account for both. 

Thank you for the answer sir.

the 5% eccentricity torsion moment refer to shift in Position of Centre of Mass and Centre of Rigidity is required by italian code. So, how can I consider this effects if the presence of floor diaphragm already includes the torsion due to eccentricity between CM and CR and accouts it in the analysis.

If I want to respect Eurocede or NTC2018 standard indications, I have to impose a 5% eccentricity between CM and CR and assign it to a master node for each floor? How can I do this with STAAD? 

The 5% eccentricity is to account for the fact that center of mass may shift from it's assumed position on either side. This is different from the torsion that is generated due to eccentricity between the CM and CR. So it is not an either or.

The 5% eccentricity is to account for the fact that center of mass may shift from it's assumed position on either side. This is different from the torsion that is generated due to eccentricity between the CM and CR. So it is not an either or.

Correct, I made confusion. I'm sorry and maybe I still don't understand which procedure I have to follow with STAAD to solve the problem.

If I want to consider this 5% eccentricity due to CM shift, how can I model in STAAD these torsion moments? Is it correct to assign torsion moments at Master Joint as nodal load?

If I consider, STAAD output (see an abstract reported below), master joint coordinates are calculated and given directly by the software, but I don't manage to select/find master joint points in modelling section and assign to them  the torsion moments. Can you suggest how can I do?

Thank you

Silvia

When you define a rigid diaphragm, the software calculates the CM and creates a master node at that location. If there is a node already existing at that location, that node is considered as the master node and if there is no existing node, the software internally creates one. These nodes that you are seeing in the analysis output file are internal nodes and so you would not be able to locate these in the model. However you do not need to apply the moments at the master nodes because as the diaphragm is rigid, it would rotate as a whole and so the exact location of the moment is not going to have an effect. You may choose any node in the plane of the diaphragm. I would usually go with the one closest to the center but again, it really does not matter.

Good evening,

considering the attached model, I have calculate, for each floor level, the story forces through the square root of summation of squares of each component according the SRSS method. 

Is it correct to consider the base shear as the sum of single story forces calculated as previous described (see excel file)? If yes, why results does not match with staad pro output?

Considering FX-Component, from hand calculation, I have obtained a base shear force equal to 120.36 kN, Staad gives 99. 24 kN. Why this difference?

IN-PLANE_TORSION_MOMENTS.xlsx4024.Response_Spectrum_Analysis.std

For a response spectrum analysis you cannot add the individual story shears to get the base shear. The reason for that is explained in the following wiki. The base shear is the one reported by the software.

https://communities.bentley.com/products/ram-staad/w/structural_analysis_and_design__wiki/29001/base-shear-does-not-match-the-summation-of-shears

Good evening,

I have some doubts about the use of FLOOR DIAPHRAM command; in particular, if I have to model a structure where at each floor there are not rigid diaphragms, is it possible to obtain from STAAD the output position of CM?

If I have to assign 5% eccentricity due to CM shift, and consequently, the torsion moments at each level, How can I operate?

Thank you!