how to model Soil Structure Interaction on Etabs,Sap2000 8

[Captains210]

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

 

[stressed]

You could define a "linear" type link which allows you to apply springs (K) and dashpots (C) in any or all 6 DOF. The link property form allows you to define factors if you want to assign to an area or line/frame instead of at a joint. Alternatively, there is a frequency-dependent link which enables you to define spring and dashpot values which vary as a function of frequency. Frequency-dependent soil properties are often provided by the geotech engineers for design of foundations supporting vibrating machinery. If you have frequency-dependent properties in a spreadsheet, you can use the Interactive database tables with Excel to paste them into SAP.

You didn't give much information on what type of structure you're modeling. Basemat foundations can be modeled with shell or solid elements.

 

[Captains210]

Thank you...
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...

 

[stressed]

You still don't give much information about your modeling and what you are trying to accomplish. For example, why are you using a nonlinear link property instead of the linear link which offers springs and dampers? Is it important to consider nonlinear PY TZ values? For pile analysis I could see that being a concern, but for building foundation analysis it's probably unnecessary in most designs. What are trying to accomplish by choosing the nonlinear link option?

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

 

[Captains210]

I am using a nonlinear link to capture the nonlinearity of soil, because I will study the Seismic Behavior of Building Frames Using Nonlinear Static Analysis (Push Over).
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

 

[Captains210]

i will send u the sap file to see it:

https://dl-web.dropbox.com/get/2D F...AANXM1V8r38gHFeVQ70GdvYvsuD4MBqMZdkAZQoFzH5rQ

 

[stressed]

Captains210, I don't have a dropbox account. Could you upload the .sdb file using Eng-tips standard upload by clicking "upload your file to Engineering.com" instead of using a 3rd party?

 

[Captains210]

Ok ...

 

[stressed]

Ok, I took a quick look. Contrary to what you posted earlier, you did not define a nonlinear link.., the link is linear and I saw no hinges assigned to the frames for nonlinear pushover analysis. You assigned a linear link with spring and dashpot properties to the area. Spring stiffness vertically (global Z direction) is 986 Kips per square meter (493 tons force per m2) with another spring value in the local 2 (global Y I believe?) direction and 0 stiffness in the other horizontal direction. Not defining stiffness in the link local 3 (global X) direction may create some problems, particularly because you have the X degree of freedom active with Y DOF turned off. Turning off degrees of freedom for analysis in such a small model can get you into trouble unless you're very careful. I am not 100% sure how the local link axes gets translated when it's assigned to an area, so I may have my global X and Y directions backwards.

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.

 

[Captains210]

Yes… I didn't define nonlinear link and hinges yet cause first i want to model the link area and plate or shell in correct approach then study the push over analysis.
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...

 

[stressed]

If you assign a body constraint to each footing area (1 body joint constraint for each footing) as I suggested earlier, results match almost exactly.

 

[Captains210]

Thank you…
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

 

[malekenp]

Hello Captains,stressed,
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_1924.pdf

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

 

[stressed]

Go to SAP2000 Define menu>Section properties>Link properties>Add new properties. There you will find by default a "Linear" link which enables you to define springs (K) and dashpots (C) in the same link. Dashpots account for energy dissipation into the soil for dynamic analysis. Alternatively, you can model soil stiffness with nonlinear multilinear plastic link instead of linear springs, which can be used with nonlinear P-Y T-Z soil data.

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.

 

[malekenp]

Thank you, stressed

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

 

[stressed]

Malek, do I understand you correctly that ATC and FEMA offer guidelines for calculating soil properties? I wasn't aware of that. Do you have a citation?

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.

 

[malekenp]

Mr stresssed you can see ATC 40 section 10.4.1.2 or Fema 356 chapter 4 for soil propreities
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-JEE_SEISMIC SSI. BENEFICIAL OR DETRIMENTAL.pdf

Regards

 

[stressed]

Thanks for the citation and the link Malek. Useful information.

 

[yazan1990]

Hello Captains,stressed,
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

 

[Captains210]

HI yazan1990
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.