I'm working through some verification problems that I had from Risa 3d. I've recreated a bunch of them in Robot to ensure I'm setting up Robot correctly to get the results I'm expecting. That said, this particular problem has me stumped. It's a dynamic problem and one which involved Response Spectrum results to be combined for multipe directions. I got the modal analysis to calculate exactly the same as both Risa3d and Sap2000. I am having great difficulty setting up the combinations correctly so my base reactions match the expected results. I'm off by a factor of about 30. What / where am I missing? The attached file includes both my Robot file, Risa3d file and the PDF documenting the verification problem along with the expected results. I am making a mistake somewhere after the modal calculations. Any help is much appriciated.
Solved! Go to Solution.
Sorry for delay of response but your request was related to cross-checking with other software and code requirements.
Moreover th code used in your reference example is UBC 1994 and seismic analysis according to this old code is not available in Robot (for American codes it is available starting from UBC 1997).
So it was necessary to:
a/ get access to UBC 1994 to know how to define "The 1994 UBC design spectra for soil type S1" - see the attached screen capture
b/ define spectral analysis equivalent to UBC 1994 with above spectra and considering multipliers mentioned in PDF file
c/ define quadratic combination between seismic directions
I have attached the modification of your model (without results to reduce the size of file), where I have defined:
1/ spectral load cases 12to14 for seismic directions X to Z
2/ in these load cases I have used S1 spectrum which I defined (not too precisely)
basing on FIGURE 16-3 from UBC 1994. Because acceleration spectrum can be defined in Robot is absolute acceleration units (like ft/s2) the conversion to relative acceleration (part of g) and additional multipliers (0.5 for Y and 0.3 for Z) were considered in direction components for load cases 12to14 - see the screen capture below:
3/ I have defined quadratic combination 15 between seismic load cases 12to 14
Reactions and displacements for this combination are shown below:
The results are coherent with analogous results from the reference PDF document supplied by you.
The small differences may result from:
- differences in material and section properties of models used in Robot, SAP2000 and RISA 3D - the results of modal analysis are slightly different in Robot than in SAP2000 and RISA 3D, especially for higher modes. For instance the frequency of 30th mode 84.68 Hz in Robot comparing to 81.55 Hz in RISA 3D and 80.96 Hz in SAP2000
- approximation of spectrum I made - hyperbolic part of the spectrum was approximated by me by the series of lines.
If this post answer your question please click "Accept as Solution". It will help everyone to find answer more quickly!
Thank you, Thank you, Thank you!!! Just to make it clear, when would I need to use the 32.17 factor instead of 1.0? What would I have to do in my seismic analysis parameters or other settings to enable me to use 1.0 in the direction factor?
In case of seismic analysis there is no need to use 32.17 factor instead of 1.0 because automatically generated spectra are coherent with code requirements.
In case of spectral analysis it may be necessary to use 32.17 factor (or other value) instead of 1.0 if the manually defined spectrum (or spectrum imported from external file) is different than expected. For instance in my modification of your test model I have defined the spectrum with the maximum of 2.5 ft/s2. Afterwards I realised that it should be 2.5g, so to avoid re-definition/modification of the already defined spectrum I have decided to use the factor of 32.17 to convert already defined values from relative acceleration to ft/s2.
Analogous situation can occur in case of metric units - in such case it is usually the factor of 9.81 to convert spectrum from relative acceleration to m/s2
I appologize as I have two similar questions posted that you have been answering. I posted an updated file on this post:
The posted file compares my Spectral Analysis results with those obtained by the Seismic Analysis type. I'm not sure how to get the Seismic Analysis type to match (or get close) to the results from the Spectral Analysis. Take a look at the file posted at the location above.