# Reinforced Concrete Beam - Problem with Degrees of Freedom

Joseph Lim
Member

in Structures

Dear community,

I was trying to using the finite element method to model the failure behaviour of the structural reinforced concrete beam element. From the literature review, I had found that the reinforced concrete was able to deform plastically and cracks in the direction of x, y, and z, by modelling the solid element with three degrees of freedom in each point. However, I was not able to find the degrees of freedom setting. May I know where can I find the setting (degrees of freedom)?

Thank you in advance.

## Comments

Lim,

The finite elements are made of the nodes and each node already has the degrees of freedom depending on the type of element. For instance, 3-D structural solid elements are made of nodes which have 3 degrees of freedom each (X, Y and Z translations). You need not turn them on using any setting, the solver is already calculating for them. You may want to check the literature to see if they refer to any particular type of elements, then search for them in the help document. You'll find all the relevant details in there.

TB,CONCR for use with only SOLID65: This is an old concrete model. It is only supported for SOLID65, an 8-node brick element. SOLID65 allows to model brittle behavior of concrete/rock. Basically, when the stress state hits the failure surface, we lose stiffness completely at the integration point. Hence, think of this as a failure/damage model (where damage=100%). This model separates "cracking" and "crushing" behavior - if an integration point 'cracks', it loses stiffness completely in that direction only in tension, but it can 'close' the crack as well. If the integration point undergoes crushing, it loses stiffness completely in all directions.

TB,MPLANE is the microplane model, supported by current-technology planar (plane strain and axisymmetry only) and solid elements. The failure surface for the microplane model is a bit different from the concrete model noted above - it also does not differentiate between 'crushing' and 'cracking'. Instead of instantly losing 100% stiffness, this is a gradual damage model, so it helps with convergence (TB,CONCR can be harder to converge since we lose 100% stiffness when failure surface is reached; with microplane model, the stiffness loss is a bit more gradual). TB,MPLANE can also be used to model rock and concrete (lower tensile stiffness than compressive).

Reinforcements - discrete or smeared - can be included with REINF26x elements.

TB,EDP is the Drucker-Prager model that can look at the inelastic behavior of soils or rocks. This is a plasticity model, so it doesn't model cracking/crushing or damage. Instead, it is used to model the inelastic volume change and shearing of soils/rocks. The Cap model is useful since it provides a yield surface for triaxial compression, too.

As you can see, we really have two ways of modeling rock/concrete - if you are looking at the brittle failure, you would look at TB,CONCR or TB,MPLANE. On the other hand, if you wanted to look at the inelastic response prior to brittle failure, you would use TB,EDP.

We also have a porous media model for looking at soil consolidation problems (CPT21x elements), although they currently do not support nonlinear inelastic material models.

How to define the smeared reinforcement in Solid65 in Ansys workbench? I found out from the search that one should define Real Constants for Solid65 in order to define fiber reinforcement in Solid65 using APDL commands.

I could not find any commands for Solid65 smeared reinforcement. If you could mention the commands here it would be of much help.

SOLID65 element is legacy element technology not under active development. Workbench already uses SOLID18x elements and the latest geomechanics material options for concrete are already exposed in Engineering Data. Could you use this together with discrete or smear reinforcement? Reinforcing sections (SECTYPE,,REINF) define the location and orientation of the reinforcing (SECDATA). The sections are referenced by REINF263, REINF264 and REINF265 elements, or MESH200 elements when used to temporarily define reinforcing locations. See also the EREINF command.