how to model Soil Structure Interaction on Etabs,Sap2000
how to model Soil Structure Interaction on Etabs,Sap2000
(OP)
Hi...
I'm trying to model soil structure interaction on sap2000
I'm using George Gazetas rules to replace the (soil and foundation) with a Springs to represent the dynamic stiffness and damping with six DOF
I want to use link element to model the spring but i wonder how i will do that??!
1- at the base of column(one point ?)
2- plain stress strain element OR solid element OR Area spring
what's the correct Approach ?
thanks a lot
Saad
I'm trying to model soil structure interaction on sap2000
I'm using George Gazetas rules to replace the (soil and foundation) with a Springs to represent the dynamic stiffness and damping with six DOF
I want to use link element to model the spring but i wonder how i will do that??!
1- at the base of column(one point ?)
2- plain stress strain element OR solid element OR Area spring
what's the correct Approach ?
thanks a lot
Saad





RE: how to model Soil Structure Interaction on Etabs,Sap2000
You didn't give much information on what type of structure you're modeling. Basemat foundations can be modeled with shell or solid elements.
RE: how to model Soil Structure Interaction on Etabs,Sap2000
I will study The Effect of Soil Structure Interaction on Seismic Behavior of Building Frames Using Nonlinear Static Analysis (Push Over) and i will define nonlinear link property
So i wonder how to assign this link to the frame at the base using appropriate way (but not one point)..
I've read about modelling soil as plain stress,strain element,solid element and Area spring but i couldn't know how!!
Thanks a lot...
RE: how to model Soil Structure Interaction on Etabs,Sap2000
You can assign links, both linear and nonlinear links to areas, either solid or shell areas, by utilizing the "Property is defined for this area in area and solid springs" multiplier which is on each link dialogue. If your units are, for example, kN/m and you type 1, then you can assign that link to an area (either shell or solid) in kN/m2 area units. If you have a basemat foundation supported by soil, using shell elements is probably your best option assuming that you've modeled columns using frame/line elements. If your foundation is pile supported, then you need to model the piles using frame elements and then assign springs or links to joints along the length of the pile.
Soil can be modeled using solid finite elements with the appropriate material property values for the soil. I don't have any experience with that modeling approach, but this link gives further explanation http://www.edwilson.org/BOOK-Wilson/16-SSI.pdf
RE: how to model Soil Structure Interaction on Etabs,Sap2000
The foundation is surface and isolated.
i said before "George Gazetas rules" replaced the soil and foundation Springs to represent the dynamic stiffness and damping with unit (t/m).
I’ve tried to model 2D frame
Foundation dimensions 1.2*1.2 m with depth .25 m
Assigning a plate with depth 1cm (cause don't effect the seismic response) to the column with spring area as Gazetas values after divided stiffness by foundation Area (t/m/m2)
Note that when i used link element and assign it to one joint the period was (T=1 sec)
And when used the plate and area spring the period was (T=1.79 sec)
Therefore, i wonder if it is correct modeling approach
i will send u the sap file to see it
RE: how to model Soil Structure Interaction on Etabs,Sap2000
https://dl-web.dropbox.com/get/2D%20Frame%203Story...
RE: how to model Soil Structure Interaction on Etabs,Sap2000
RE: how to model Soil Structure Interaction on Etabs,Sap2000
RE: how to model Soil Structure Interaction on Etabs,Sap2000
I also noted that you assigned a joint diaphragm constraint. A diaphragm only acts in-plane directions. You might try assigning a joint body type constraint.
I didn't see any NL cases defined.
Since you are comparing results from a link assigned as an area vs. a lumped joint link at the base of the column, could you upload your lumped joint link model? Careful to account for the fact that an area assignment is on a per area unit basis.
RE: how to model Soil Structure Interaction on Etabs,Sap2000
Spring stiffness vertically (global Z direction (493 t/m2/m')) is't the same with local 2, U1 and U2 represent translation degree of freedom and R3 rotation degree of freedom for 2D frame
i didn't define stiffness link in local 3 cause the frame is 2D frame and the earthquake will affect in global x direction (but i will define and see what will happen)
i will see the diaphragm too…
So did you know what i need?? Just knowing the correct way to model the link in an area instead of one joint cause one joint is not enough to represent the soil and foundation…
Tfixid=0.443 sec
T=1.0546 (Spring one joint)
T=1.574 sec (Area Spring Shell-Thick With Diaphram 1cm) note that the area thickness is 1 cm
THAAAANKS...
RE: how to model Soil Structure Interaction on Etabs,Sap2000
RE: how to model Soil Structure Interaction on Etabs,Sap2000
Yes, you are right about body constraint I have read about it in sap's help
So i will try and tell you what will happen
RE: how to model Soil Structure Interaction on Etabs,Sap2000
My name is Malek, iam a Phd student in civil engineering
i read all what you have written and allow me to participate with your disscution that i juge very important
i read an article that describe a new approach to take in to account the soil structure interaction in the procedur of pushover analysis
i understand what the auther of the article done but in the modeling in sap 2000 it was not clear for me
this is the link of the article
http://www.iitk.ac.in/nicee/wcee/article/WCEE2012_...
he write :
In SSI model, the base soil is simulated by a horizontal spring-dashpot systems. And the damper is simulated by
LINK element.
can you explain to me what he had done please
Regards Malek
RE: how to model Soil Structure Interaction on Etabs,Sap2000
Do not confuse Pushover analysis with soil-structure analysis. Although they can be coupled, they are separate modeling issues. For example, you can run a NL Pushover analysis using either linear soil springs or restraints or nonlinear links.
RE: how to model Soil Structure Interaction on Etabs,Sap2000
I have done a lot of Pushover analysis on structures and to involve SSI i replace the fixe base by links
i calculate horizontal and roking stifnesses and damping in 2D with Gazetas & Kausel formulates or ATC ,FEMA
and to choose what kind of link i saw this artical
so i will assign link non linear or damper and i will define in 2D stifnessis and damping but i have just horizontal and roking (u2,r3) valus so i will fixe the third DOF (vertical u1)
of course with pushover analysis i will define all steps
but there is one problem in lateral loads, in the artical above he applied the force on the foundation masse also with floors
so what can you explain that stressed?
Malek
RE: how to model Soil Structure Interaction on Etabs,Sap2000
I looked over the paper that you linked to. It appears they assign loads on the structure as a function of height and story/floor weight and mass. Unfortunately, the paper doesn't define all the terms used, so it seems that you would have to look up the referenced Mengfu paper for more details.
Interesting to read the conclusions in their paper. Consideration of soil-structure interaction can have a significant impact not only on pushover analysis results, but on results of any dynamic analysis of a structure supported by soil or piles, and any static analysis of lateral loads. Using a more realistic "softer" base can save money in design and construction.
RE: how to model Soil Structure Interaction on Etabs,Sap2000
but i think its the same as gazetas formule
for lateral loads they said in the artical "For the SSI system, the lateral load should be applied on each floor of the superstructure, and on foundation." so there is a force applied in the foundation mass but how??
for mengfu article i found it in chineese only and i could'nt read it.
for the conclusion in te artical there is a very intersting article of Gazetas and mylonakis
http://ssi.civil.ntua.gr/downloads/journals/2000-J...
Regards
RE: how to model Soil Structure Interaction on Etabs,Sap2000
RE: how to model Soil Structure Interaction on Etabs,Sap2000
I am working on soil structure interaction in my thesis
i modeled RC buildings frame ( 5,10,15,20) storeys i want to include the effect of SSI using SAP2000
First i assumed that the base of structures is fixed and use the response spectrum analysis (you can include the Ss and S1 and also you can choose the soil class)
Now, I want to include the soil stiffness in the model using Gastase equations to compute the SSI effects
Any one can help how can i model these springs
RE: how to model Soil Structure Interaction on Etabs,Sap2000
you can represent the Equivalent stiffness and damping of soil by using link element Instead of springs..
Read the above and download the file that I have uploaded.
RE: how to model Soil Structure Interaction on Etabs,Sap2000
RE: how to model Soil Structure Interaction on Etabs,Sap2000
Where can assign these links to area springs or to the base of coloumn
RE: how to model Soil Structure Interaction on Etabs,Sap2000
RE: how to model Soil Structure Interaction on Etabs,Sap2000
RE: how to model Soil Structure Interaction on Etabs,Sap2000
Thank you..
RE: how to model Soil Structure Interaction on Etabs,Sap2000
P-Y data can be modeled as NL link elements. See Define > Section Properties > Link/Supports.
Changing the link type to 'Multilinear Elastic' will allow you to define the curves. Note that the U1, U2, U3 are in the link local axis such that U1 will always be axial. You need the non-linear box to be checked in order to enter the P-Y data.
I recommend drawing these links as 2- joint links with one end connected to the frame element and the other to a support.
If you define non-symmetric links, you have to be careful which orientation the links are drawn on.
Lastly, the defined P-Y links require all relevant load cases to be run non-linear.
These links can also be assigned as area springs (eg: for bearing)
RE: how to model Soil Structure Interaction on Etabs,Sap2000
I think there is no one way in modelling soil stiffness as links or area Springs. Most handbooks I have read about soil structure interactions with raft foundations always uses area Springs. Let me share my method even though I have not concluded it's the best way.
I modeled the raft in ETABS as shell thick. Then I manually meshed the raft slab say 1x1m. Then I assign area Springs to these meshed Slabs. I define modulus of subgrade reaction in the 3 direction. There is an option to choose whether it's linear, compression or tension. I choose linear. I also restrain the springs in the X and Y direction. Does using 4DOF.What also define nonlinear load cases to my linear load cases. What do u make of my method.
RE: how to model Soil Structure Interaction on Etabs,Sap2000
So i have created a rcc structure modedl whose natural frequency i have obtained. I am varying the soil layer thickness and setting the system in resonance by adjusting the shear wave velocity (by using SHAKE or PROSHAKE) and finally conducting a time history analysis to study the response.
My problem is for modelling the soil I had no clue how to assign transmitting boundaries for which i have brief idea now after reading the dialogue here. I am considering the bottom to be bed rock so the bottom will be fixed. The sides however have to be truncated and a viscous transmitting boundary has to assigned. I have read various journals which give similar views to the conversation here. But can someone help me by telling me how to go about with the modelling as to which elements to use for the meshing and how to calculate stiffness and damping values based on the mesh used. Im sorry for asking so much. I really dont have a knowledge level as intense as you people here. Thanks in advance..hope somebody helps.
RE: how to model Soil Structure Interaction on Etabs,Sap2000
my method is replacing the (soil and foundation) with a Springs to represent the dynamic stiffness and damping by using link element
maybe you didn't consider the dynamic effects and soil properties in your method..