Stress - displacement based material input(Tension) for Concrete Damaged Plasticity

[aurum]

I'm implementing stress displacement-based damage model for tension using Concrete Damaged Plasticity. So, it turns out when I select displacement-based input instead for cracking strain, ABAQUS will issue an error message if the calculated plastic strain values are negative and/or decreasing with increasing cracking strain, the tensile damage curves are incorrect. This error does not arise for when I opt for cracking strain as input.

I independently verified if my plastic strains are decreasing/negative using the formulations provided by ABAQUS and they seem very good but it turns out to be not working in the software.

ABAQUS manual says, "The implementation of this stress-displacement concept in a finite element model requires the definition of a characteristic length associated with an integration point." I do not understand where do we define the characteristic length in the software. Any assistance is appreciated.

 

[FEA way]

Abaqus/Explicit calculates this characteristic length automatically. For first order solid elements it’s typical length of a line across an element while for second order solid elements it’s half of that. Beams, trusses, membranes and shells use different definitions. However you don’t have to specify this in Abaqus. But if you want to define it manually you can use VUCHARLENGTH user subroutine.

 

[aurum]

FEA way

That's what I have read on the manual but how do you think I can implement stress-displacement based damage model in Concrete Damage Plasticity since it is showing the above mentioned error? Thanks for your time.

 

[FEA way]

Can you share your .inp file or part of it where material is defined ? Keep in mind that in the *Concrete Tension Stiffening, Type=Displacement keyword first value of cracking displacement must be 0 while for the *Concrete Tension Damage, Type=Displacement keyword first pair of tensile damage variable and cracking displacement must be zero as well.

There are some examples with these keywords in the documentation (like the one called „Seismic analysis of a concrete gravity dam”, „Notched unreinforced concrete beam under 3-point bending” and those in Verification Guide).

 

[aurum]

Hi FEA Way,

I tried reproducing the Notched unreinforced concrete beam under 3-pointing bending problem using their input file. My load-displacement output curves do not seem to be in agreement with those in the manual. Which load and displacement are used to plot the load-displacement curves. Aren't we supposed to use the RF2 and U2 at the output nodes?

 

[FEA way]

Yes, they used U2 and RF2 but they summed reaction forces for constrained nodes. That’s probably the reason why your curves are different.