Hi! Anyone can advice how to model the connection between mat foundation and soil? My idea is to use gap element plus spring element to simulate the non-linear behavior and use non-linear static analysis to analyze our mat foundation.
The procedure to follow will depend if you are meshing both the contacting bodies: material foundation and soil. If yes, then the use of CGAP elements between both materials is the the target, because meshing the soil you are capturing its stiffness explicitly.
The other alternative is to mesh only the foundation and use nastran CELAS2 spring elements to consider the stiffness of the soil: you will have to define different spring properties in function of the covered area under the spring.
With CGAP you can define a compression-only element, simply input a value in the field "Compression-Stiffness" and you are done, it should be a big value, say 1e6 N/mm, this value will be used when the GAP element is closed, it means that the CGAP element when closed will run as a rigid element, transmitting all the received compression force. The element will work only in compression, allowing freely separation between the two bodies. But take care with singularities, the FE model should be properly constrained, if not you will have the error "stiffness matrix is singular". To avoid rigid body movements in the lateral directions the trick is to define symmetries, then only movement in the direction of the CGAP element is allowed.
Take care when meshing the CGAP elements, you need to define the orientation of the CGAP element properly: the trick is to select any GLOBAL axis normal to the element local X-axis.
Also, when defining the linear static study make sure to activate the option "GAPS AS CONTACT", if not your CGAP element will behave as an spring:
But if contact separation is not your problem (ALL the element will work always at compression!!) and the meshing of SOIL material is neglected, then you can use an spring CELAS2 element (or a simply CROD element playing with K=AE/L, is the same!!). Here you can define different properties for the spring element in function of the influence area of every spring. Take a look to my web site where I explain step-by-step how to solve a spring problem:
And in the case where you need to define a nonlinear relation between force vs. length (ie, nonlinear stiffness) then you can use a CBUSH element and solve the problem as nonlinear:
In summary, as you can see you have many options, always use the simplest one !!.