MARS - A Software Dedicated to Advanced Concrete Modeling

question for shell elements with a given thickness:
is it possible to define if the actual 2D shell element lies in the center or is aligned with either the top or the bottom outer surfaces?

Assume for example a case where you want to bond a steel sheet to a concrete body, using e.g. master slave.
How can we model the connection and in parallel ensure the correct location of the resulting force in the sheet?

The nodes of shell elements are defined on the mid-surface, the thickness is used to account for transverse effect in force computations, such as bending, and post process (plot as 3D slab instead of flat 2D surface). The alignment is up to the user, but the forces are always on the nodes, which are on the mid-surface.

In a master slave situation, the slave and entity are kinematically constrained. In TrngFaceNodeBondList - SlidingWithFriction, the slave nodes, if not already on, are moved onto the master surface.

In a contact situation, there must be a initial gap between the shell mid-surface and the other surface for the penalty force to engage, i.e. the nodes of shell (on mid-surface) should not be exactly on the surface of the other party.

It depends on what you want to achieve to choose whether a master slave or a contact formulation, then the shell elements are placed at slightly different location.

I understand that nodes of standard shell elements are in the center plane and what the purpose of the thickness is.

What I refer to is the ability to define the nodes on the surface of the shell in order to use master slave. Then the software needs to properly account for the introduced load eccentricity.
This feature is available in other FE software where you have a switch TOP,CENTER,BOTTOM to decide where the nodes of shell are assumed.

see e.g. https://www.sharcnet.ca/Software/Ansys/ ... fsets.html

In the force calculations of the shell elements and the other party (in a contact or constraint formulation), the offset effect (e.g. moment) between them is accounted for. It is a matter of where you place the shell elements to achieve the alignment or eccentric effect.

Can you please provide an example?
Which constraint can account for the eccentricity ? Does this work for / is allowed for all the constraints?

Assuming we are using node-face constraint formulation (TrngFaceNodeBondList) to model the interaction between the steel sheet and concrete.

To clarify: my previous comment (slave nodes moved to master surface) applies when the user specifies SlavesOnSurface when defines TrngFaceNodeBondList.

With keyword MasterSlaveWithRotations, the formulation allows a certain gap between slave nodes and master surface. This is the one we suggest to use in the following example.

In reality, let's image a concrete slab sits in XY plane, a steel sheet (thickness of T) sits on top of it, we apply an evenly distributed force on the top surface of steel sheet along XY plane in shear.

In MARS model, if the steel sheet is modeled as shell elements, the mid-surface is T/2 away from the concrete. When we directly apply forces on the shell elements, these forces are applied on the nodes which are on the mid-plane of the elements. As a result, this gives the correct resultant force, however, to account for the eccentricity effect (and resulting moments), we need to create another load list to apply moments on the shell elements. Keyword NodalLoadList can be used to apply force or moment. It's recommended to make the steel sheet as master surface, and concrete nodes as the slave nodes.