STAAD.Pro Response Spectrum [FAQ] - Structural Analysis and Design - Wiki - Structural Analysis and Design - Be Communities by Bentley

Structural Analysis and Design

Structural Analysis and Design
This is where you can find and contribute to discussions, ideas, and other information about Bentley Structural Analysis and Design products.

STAAD.Pro Response Spectrum [FAQ]

Structural Analysis and Design - Wiki

STAAD.Pro Response Spectrum [FAQ]

   
  Applies To 
   
  Product(s): STAAD.Pro
  Version(s): All
  Environment:  N/A
  Area:  Analysis
  Subarea:  Response Spectrum Analysis
  Original Author: Bentley Technical Support Group
   

 

 

 

 

 

 

 

 

  1. I want to analyze my model for a response spectrum in X, Y and Z directions. I am specifying all the 3 direction factors as 1.0 ...Is my correct approach correct?
  2. In the output file of a response spectrum analysis, there is the section that shows the mass participation factors in the x, y, and z directions. Then it shows the 'base shear' in all 3 directions. What is the reference point for this? I mean, does Staad select a 'base' or is the value just the sum of all forces in that particular direction?
  3. This is a question dealing with response spectrum analysis. I know that if a force is applied in the response spectrum load case, it will be converted to a mass that will in turn affect the modal response. My question is, will that input force still be applied as a static force in the analysis? Or, would I have to apply the force in a different load case to account for it?
  4. I am currently working on a seismic model which requires a response spectrum input.
    What I am finding is that regardless of the value I specify for damping, the displacements and forces appear the same. Is this right?
  5. I am attempting to run a spectral analysis of a structure. I have a design spectrum in terms of %ground acceleration and i am trying to determine how the scale factor works. Could you direct me on what the scale factor is? Also should I be entering the % ground acceleration into the chart or the actual acceleration? 
  6. I need to know how to input the missing mass correction command as too much mass is missing even after increasing the number of modes.
  7. As I understand The Rayleigh method is used for natural Frequency calculations (first mode only) in the command CALCULATE NATURAL FREQUENCY & also in the command DEFINE UBC LOAD or 1893 load. Whereas the matrix method of iteration (like Staddola method) is used in the Response Specterum method of analysis . Does this mean the values which we got by define 1893 load or Calculate natural frequency are wrong?
  8. The natural frequencies obtained during a Response Spectrum Analysis do not match the values calculated using the CALCULATE RAYLEIGH FREQUENCY command. Why is that?
  9. Are the joint displacements (Inch, Radians) reported in example 11 the static displacements? If these are amplitudes (for example, at joint 5 for load case 2, X trans = 1.94384 inch) doesn't that mean this joint is failing in amplitude since it is very high?
  10. In a response spectrum analysis, the base shear does not match the summation of shears I get at the base of the columns. Which one should I use as base shear ?
  11. I am doing a response spectrum analysis and getting an error "No unsupported masses entered ...". What is the problem ?

1. I want to analyze my model for a response spectrum in X, Y and Z directions. I am specifying all the 3 direction factors as 1.0.

SPECTRUM SRSS X 1 Y 1 Z 1 ACC SCALE 32.2 DAMP 0.05

0 0.375; 0.881 0.375; 0.9 0.3375; 1 0.328; 1.1 0.3; 1.2 0.27; 1.3 0.2475

1.4 0.24; 1.5 0.2325; 1.592 0.2175

Is my correct approach correct?

If the direction factors for X, Y and z are all specified as 1, it indicates an earthquake of full intensity in all 3 directions simultaneously. This is an unlikely scenario. An earthquake which is occuring at its full intensity along X cannot act with full intensity in Y and Z also at the same time.

Instead, you ought to have 3 separate load cases, with the spectrum applied in each of those 3, and the direction factors being X=1,Y=0,Z=0 for the first case, X=0,Y=1,Z=0 for the second case, and X=0,Y=0 and Z=1 for the third case, as shown below.


LOAD 4 SPECTRUM IN X-DIRECTION
SELFWEIGHT X 1.0
SELFWEIGHT Y 1.0
SELFWEIGHT Z 1.0
JOINT LOAD
10 FX 17.5
10 FY 17.5
10 FZ 17.5
SPECTRUM SRSS X 1.0 ACC SCALE 32.2
0 0.375; 0.881 0.375; 0.9 0.3375; 1 0.328; 1.1 0.3; 1.2 0.27; 1.3 0.2475
1.4 0.24; 1.5 0.2325; 1.592 0.2175


LOAD 5 SPECTRUM IN Y-DIRECTION
SPECTRUM SRSS Y 1.0 ACC SCALE 32.2
0 0.375; 0.881 0.375; 0.9 0.3375; 1 0.328; 1.1 0.3; 1.2 0.27; 1.3 0.2475
1.4 0.24; 1.5 0.2325; 1.592 0.2175


LOAD 6 SPECTRUM IN Y-DIRECTION
SPECTRUM SRSS Y 1.0 ACC SCALE 32.2
0 0.375; 0.881 0.375; 0.9 0.3375; 1 0.328; 1.1 0.3; 1.2 0.27; 1.3 0.2475
1.4 0.24; 1.5 0.2325; 1.592 0.2175


Go to Help - Contents - Technical Reference - Commands and Input Instructions - Loading Specification - Dynamic Loading Specification - Response Spectrum Specification for more details.

2. In the output file of a response spectrum analysis, there is the section that shows the mass participation factors in the x, y, and z directions. Then it shows the 'base shear' in all 3 directions. What is the reference point for this? I mean, does Staad select a 'base' or is the value just the sum of all forces in that particular direction?

Each mode has a base shear that comes from the modal displacement at each joint with mass in the direction being excited by the base acceleration and the input spectral acceleration and the modal frequency. These modal base shears are combined by SRSS or any other method in STAAD that you select. In effect, all supported joint directions form the base where the displacement of every mode is zero.

3. This is a question dealing with response spectrum analysis. I know that if a force is applied in the response spectrum load case, it will be converted to a mass that will in turn affect the modal response. My question is, will that input force still be applied as a static force in the analysis? Or, would I have to apply the force in a different load case to account for it?

Response spectrum analysis is a dynamic analysis based on ground motion spectral acceleration. The acceleration usually varies with the period. Since there is no direct input for masses, what you are entering as forces are weights, and STAAD extracts masses from those weights. Hence, the same weight value should be entered in all 3 global directions for general space structures in order to get the natural modes and frequencies correctly.

The response spectrum result will be an absolute unsigned value for each output quantity which represents the maximum value for that quantity. Because of this, the 6 force/moments at each end of a beam will all be positive. Also given the member forces/moments on one end, you cannot compute those results on the other end because the values are considered independent much the same as if these were peak values in time history that all occurred at different times.

If you want static loading results combined with spectrum results, then use load combinations, possibly with the SRSS option.

4. I am currently working on a seismic model which requires a response spectrum input.
What I am finding is that regardless of the value I specify for damping, the displacements and forces appear the same. Is this right?

The damping factor that one specifies in the input has no effect at all if the combination method is SRSS. For the SRSS scheme, the effect of damping is built into the spectrum values (period vs. acceleration or period vs. displacement) that the user specifies. In other words, if the damping factor is f1, the acceleration that the user should provide ought to be A1 corresponding to period T1. If the damping factor is f2, the acceleration ought to be A2 for the same period T1. In other words, for the SRSS method, the effect of damping has to be reflected on the spectral acceleration or spectral displacement that is being input. The damping coefficient by itself does not have a direct impact on the results. It's effect is indirect.

With the CQC method, it is a different story. Damping will generally have an impact on the results, because, the damping factor is an explicit term in the equation used in CQC.

5. I am attempting to run a spectral analysis of a structure. I have a design spectrum in terms of %ground acceleration and i am trying to determine how the scale factor works. Could you direct me on what the scale factor is? Also should I be entering the % ground acceleration into the chart or the actual acceleration?

The spectral accelerations entered, after multiplication by the scale factor, must be in the current length units of the STAAD input. For example, if the spectral acceleration is in g's (%ground acceleration) and the current units are inches, then the scale factor must be 386.088; or 32.17 for feet; or 9.80665 for meters. The scale factor is simply the conversion factor from the units of the spectral acceleration to the current units of the STAAD input data.

6. I need to know how to input the missing mass correction command as too much mass is missing even after increasing the number of modes.

The answer to your question is available in Section 5.32.10.1 of the STAAD.Pro Technical Reference manual. Just use the keyword MIS along with the SPECTRUM command. For example,

SPECTRUM CQC X 1.0 ACC DAMP 0.05 SCALE 32.2 MIS

Please refer to example 11 in the Examples manual for information on the commands required for doing a response spectrum analysis.

7. As I understand The Rayleigh method is used for natural Frequency calculations (first mode only) in the command CALCULATE NATURAL FREQUENCY & also in the command DEFINE UBC LOAD or 1893 load. Whereas the matrix method of iteration (like Staddola method) is used in the Response Specterum method of analysis . Does this mean the values which we got by define 1893 load or Calculate natural frequency are wrong?

It is not true that the lowest frequency is the one which is associated with significant amount of participation of the masses of the model. That may be true of structures which look like a cantilever. But if the spatial distribution of masses is extensive, there is no guarantee that the fundamental mode is the most critical mode.

The statement that the Rayleigh frequency is associated with the first mode of the structure too is not correct.

A structure has several modes of vibration. If the structure were free to vibrate, the modes of vibration will follow the ascending order of strain energy. Consequently, if Y is the weakest direction of the structure, a Y direction mode will be the first mode. If the next weakest direction is Z, then the second mode will be a Z direction mode. Structures have local modes, where a small region within the model vibrates while the rest of the model remains stationary. It is entirely possible that a local mode is the lowest energy mode.

In many cases, torsional modes happen to be the lowest modes. Local and torsional modes are associated with negligible mass participation. You should look at the mode shapes of all the modes to get a sense of all the major vibration modes.

Since when using the Rayleigh method, one tends to load the structure in a manner which generally resembles a large mass participation mode, there is no sense in comparing the Rayleigh frequency with the lowest frequency from the eigensolution. Instead, you have to try to compare the displaced shape of the model used in the Rayleigh calculations with the various modes from eigensolution until you find a mode shape which resembles the displaced shape. When you do find a match, you will find that the Rayleigh frequency will be similar in value to the frequency of the matching mode.

If you do not like the frequency being used in the IS 1893 load generation, which is Rayleigh based, there is an option in STAAD for the user to provide his/her own value of the frequency. This is done using the PX and PZ options, as in the following example.

ZONE 0.05 K 1.0 I 1.0 B 1.0 PX 0.4 PZ 0.8

The values you provide for PX and PZ will be used in place of the one calculated by the Rayleigh method.

8. The natural frequencies obtained during a Response Spectrum Analysis do not match the values calculated using the CALCULATE RAYLEIGH FREQUENCY command. Why is that?

In STAAD, there are 2 methods for obtaining the frequencies of a structure.

  1. The Rayleigh method using the CALCULATE RAYLEIGH FREQUENCY command
  2. The elaborate method which involves extracting eigenvalues from a matrix based on the structure stiffness and lumped masses in the model.

The Rayleigh method in STAAD is a one-iteration approximate method from which a single frequency is obtained. It uses the displaced shape of the model to obtain the frequency. Needless to say, it is extremely important that the displaced shape that the calculation is based on, resemble one of the vibration modes. If one is interested in the fundamental mode, the loading on the model should cause it to displace in a manner which resembles the fundamental mode. For example, the fundamental mode of vibration of a tall building would be a cantilever style mode, where the building sways from side to side with the base remaining stationary. The type of loading which creates a displaced shape which resembles this mode is a lateral force such as a wind force. Hence, if one were to use the Rayleigh method, the loads which should be applied are lateral loads, not vertical loads.

For the eigensolution method, the user is required to specify all the masses in the model along with the directions they are capable of vibrating in. If this data is correctly provided, the program extracts as many modes as the user requests (default value is 6) in ascending order of strain energy. The mode shapes can be viewed graphically to verify that they make sense.

Thus, the answer to the question is : If you want to use the Rayleigh method, make sure you provide the right type of loading. If the load you apply causes an arbitrary displaced shape which has no resemblance to the vibration mode you are interested in, the frequency value you get will be wrong.

9. Are the joint displacements (Inch, Radians) reported in example 11 the static displacements? If these are amplitudes (for example, at joint 5 for load case 2, X trans = 1.94384 inch) doesn't that mean this joint is failing in amplitude since it is very high?

For spectrum load cases, they are the absolute maximum displacement that those degrees of freedom will ever experience under the dynamic loading which that spectrum represents. In this example however, the numbers are so large only because the spectrum used is rather unrealistic. The spectral acceleration for mode 1 is 2.8g, which is unlikely even in the most intense earthquake.

10. In a response spectrum analysis, the base shear does not match the summation of shears I get at the base of the columns. Which one should I use as base shear ?
Related query : In a response spectrum analysis, summation of the support reactions does not match the base shear reported. Which one should I use as base shear ?

The one that the software reports as the base shear, is the correct value to use. The column shears ( or support reactions ) reported are all individual maximums and may not occur at the same instant of time. There is a high probability that at the instant when the base shear is maximum, some of the column shears ( or support reactions ) will be less than their individual peak values. Moreover the method used for modal combination, gets rid of signs and hence column shears ( support reactions ) like any other response spectrum output, would be devoid of any sign. Hence one cannot add these up to arrive at the base shear.

11. I am doing a response spectrum analysis and getting an error "No unsupported masses entered ...". What is the problem ?

There are 3 things you need to check

1. You have not defined any seismic masses as part of your seismic load case. You need to add these as loads and the software internally converts these to masses. You may refer to section 5.32.10.1.1 of the Technical Reference Manual for details. There is an example 11 provided with the software which can also be referred to.

2. You may have included Self weight as part of the seismic mass definition but the density of the material you have used may have been set to 0. 

3. All nodes in your model are restrained from vibrating due to supports. You may need to generate additional nodes so that there are some free masses in your structure that can vibrate.

12. Please find attached the attached file, which is the model with the Euro Spectrum. In the box “Design Ground Acceleration” I put 0.075 which is the ag value. Question: Is this value the correct value to input in this box or it should multiplied by g = 9.81m/sec2 ?

 In STAAD Eurocode 8:2004 implementation, if you have specified 0.075 in the box designated to specify the Design Ground Acceleration, the engine takes that value as 0.075g for calculations. It automatically multiplies that value with the acceleration due to gravity.

See Also

Product TechNotes and FAQs

Structural Product TechNotes And FAQs

External Links

Bentley Technical Support KnowledgeBase

Bentley LEARN Server

Comments or Corrections?

Bentley's Technical Support Group requests that you please confine any comments you have on this Wiki entry to this "Comments or Corrections?" section. THANK YOU!

 

Comments
  • dear sir

    for normal structure for instance the building with 10 levels., should we use self-weight on three direction or just Y direction?Note that earthquake load accrue  on X and Z direction.

  • It is always preferrable to have the mass defined on all the three possible directions of vibrations. That the structure is stiffer in the vertical direction, and the probable chance of having the mass vibrating in the vertical direction is only possible in the higher modes which is almost non-practical to consider - will be automatically taken care of by STAAD. You only need to ensure that the lateral modesof vibration reaches at least a mass participation value of 90%.

  • FWIW, you would be better served posting inquiries like this in the community's forum -- click on the Forum tab and then "New Post".

  • Is there any command in Staad " CALCULATE NATURAL FREQUENCY" AS STATED in one of the above postings. Please clarify.

  • can any one teach me staad pro ,,,,,for loading  using IS codes

  • Dear

    Please any one tale me when I define the mass on the all three direction i.e. X, Y, Z for 3D vertical cantilever stack of height 100m and applied response spectra for horizontal X-direction , then how the bending moment and shear force for another direction are come to zero. Whether STAAD automatically considered displacement in another horizontal direction to zero while calculating moment for response in X direction. Is it ant theoretical support is available to prove the same.