Hello

you can model steel reinforcement as a truss element which is embedded in concrete (constrain), in this way, I think you will solve the problem of convergence

once you have interaction between steel and concrete (embedded) no need to think about node connectivity

Dear all,

The problem of non convergence for RC structures can have multiple origin.

Bad implementation of model or bad model

Instabilities that can be physic but that the numerical scheme cannot asses.

Anyway since concrete is subjected to softening, you must be careful of using a regularization method such as non local, gradient, or Hillerborg.

My  advice.

1) Use truss model for R bars as adviced by Mohammad  (be carefull if you are in 2D, the section area of Rbars must be computed in terms of thickness of you beam. depending on the FE code you use, the thickness can be assumed to be unity in 2D.

2) Use a improved model for concrete (Mazar's model is very simple and is quite robust)

3) Use a regularization limiter such as Hillerborg, if you don't your results will depend on  mesh size.

4) Usually there are some convergency problems at the peek, if it is the case, reduce the time step or use an arc length method.

regards

Christian

You can change the viscosity parameter.  First run the model without concrete damage in tension and compression  and apply these parameters later. You can use  the fracture energy instead of stress-strain relations in tension. 

One models for a particular objective - not just to avoid divergence. If your objective is to examine a structural behaviour in a global sense, you could use either a smeared or a truss element (or embedded reinforcement in ABAQUS) with perfect bond.  I suspect neither should have difficulty with convergence (relative to an unreinforced concrete model).  If you are examining closely 9at material level) for bond-slip (for example), you will need discrete elements with interface characteristics defined between steel and concrete.  Such problems are complex and may have many convergence issues.

You may used solid elements for to mesh the reinforcement bars, which led to extremely small elements with enormous number, and which require such origins in the adjacent concrete elements......That is why it is not converging.

Regardless of the used finite element program, reinforcing bars in reinforced concrete members are generally modeled as link or truss elements because they are subjected to axial forces only ( i.e. no shearing forces and bending moments)