tensile behaviour for plain concrete with cdp model

[Andi_Co]

Hi guys,
I need some help.
How can i model the tensile section in the concrete damage plasticiy model?
For example the tensile strength is 3 N/mm2 and the max crack wide should not exceed w0<0.12mm with a mesh-size of 2x2x2 cm (C3D8R-Elements).
Do I use strain, displacement or fracture energy-type? And how can i considered the mesh sensitity in the model?

Kinds regards
Andi

 

[FEA way]

To define concrete damaged plasticity model in Abaqus the following keywords have to be included:

*Concrete Damaged Plasticity
*Concrete Tension Stiffening
*Concrete Compression Hardening

You can also add *Concrete Tension Damage and/or *Concrete Compression Damage optional keywords.

Both *Concrete Damaged Plasticity and *Concrete Compression Hardening don't have any types to choose from and you just have to provide the values of specific parameters for them so I won't focus on the definition of these keywords. However the last mandatory keyword (*Concrete Tension Stiffening) can be defined in one of 3 ways (type = strain/displacement/GFI). The default one is strain. According to the documentation, when there's no reinforcement (like in your case), the use of this default strain type will cause mesh sensitivity. Thus it is recommended to use either displacement or GFI type in such case. Keep in mind that even then there's still a risk of some mesh sensitivity in the analysis due to the concept of characteristic length. To reduce it you should avoid elements with high aspect ratio. Another way would be to use VUCHARLENGTH subroutine (in Explicit).

 

[Andi_Co]

Thanks, but if i use stress-displacement approach for plane concrete with a beam (size 300x300x4000mm³, mesh 20x20x20mm³ C3D8R), how would the stress-cracking displacement look like?
e.g.
ft = [3; 0.03] N/mm²
ut = [0; 0.12] mm
Do the 0.12 mm belong to one element(size20x20x20mm³) or to what extent does the effective length play a role?

 

[FEA way]

In case of C3D8R element (reduced integration linear hexahedron) characteristic length is taken as typical length of a line across element. When you specify stress-displacement data pairs, Abaqus divides cracking displacements by characteristic length of specific element to determine strains.

I can recommend the following resources that explain the details of this topic and provide additional relationships between variables used in CDP model:

- Abaqus documentation chapters: "Concrete damaged plasticity", "Damaged plasticity model for concrete and other quasi-brittle materials", "A cracking model for concrete and other brittle materials" and "An inelastic constitutive model for concrete"
- "A note on the Abaqus Concrete Damaged Plasticity (CDP) model" W.S. Li et al.
- "Numerical modelling of the seismic behaviour of adobe buildings" S.N.T. Ruiz
- "The use of continuum models for analyzing adobe structures" N. Tarque et al.
- "Analysis of Crack Formation and Crack Growth in Concrete by Means of Fracture Mechanics and Finite Elements" A. Hillerborg et al.