Beam-to-Solid-Bar-Slip

[cqf_2232]

Dear STKO Team,
I recently watched your E-learning course “Links and Interactions between Nodes and Elements”. There are still some questions about the definition of the interface between the rebar and concrete.
As far as I know, the behavior of “MultiLinear Material” can be only defined as stress(N/mm^2)-strain or force(N)-displacement(mm). But in the example “03_beam_solid_bar_slip_2”, the bond-slip relationship was defined as stress-displacement (tau(N/mm^2)-slip(mm)) by using “MultiLinear Material”, while it was defined as force-displacement(tau*area(N)-slip(mm)) in the other FEA software such as Abaqus and Ansys. So, could you tell me how it works in SKTO?

[STKO Team]

As far as I know, the behavior of “MultiLinear Material” can be only defined as stress(N/mm^2)-strain or force(N)-displacement(mm)

This is not necessary true.
In OpenSees a uniaxial material is just a Y-X relationship, it's up to you to understand what is X and what is Y.
Few examples:

• stress-strain (Y = Pressure, X = none) in case of fibers
• force-displacement (N = Force, X = displacement) in case of concentrated springs
• force-deformation (N = Force, X = strain) in case of distributed shear in a section aggregator.

When you use the Bar-Slip automation in STKO, the uniaxial material should be a Stress-Displacement law, because it should represent the behaviour of a cohesive zone of a unit-area.
Internally, STKO takes the tributary area from the mesh and automatically computes an equivalent concentrated spring(Force-Displacement = Stress*TributaryArea - Displacement).

In order to do it for any kind of material, we do not change the input in the original material. Instead, we wrap it into a Parallel material which allow us to assign a scale factor to the original material such that:
parallel_material_stress = original_material_stress * scale_factor.
Setting the scale_factor = the tributary area, the parallel_material_stress is actually the concentrated force you need.

Have a look at how we do it in the analysis_step.tcl file:

slip.png (36.7 KiB) Viewed 1695 times

[cqf_2232]

Thank you for your detailed explanation. I have another question about modeling. In ABAQUS and ANSYS, reinforcement elements and concrete element nodes need to be overlapped to simulate bond-slip. Is this factor to be considered in STKO?

[STKO Team]

The Beam-to-solid-bar-slip automation assumes you create a hole in the solid volume. So it's a different kind of modeling. We are currently working on another automation that allows you to apply bar-slip into the ASDEmbeddedNodeElement to consider slip in embedded rebars as well

[cqf_2232]

Ok, I get it. Thank you very much!

[cqf_2232]

Dear STKO Team
There was a problem when I was running the model "03_beam_solid_bar_slip_2" in the E-learning course (Links and Interactions between Nodes and Elements) . What is the reason for this warning? Thank you again！

[STKO Team]

The model was set up for parallel analysis with OpenSeesMP, while you are using OpenSees.
You can tell it from the error:
OpenSees cannot find the ParallelRCM numberer which is only available in OpenSeesMP

[cqf_2232]

Hi, I used the same method to create two simple bond-slip models. The first cube model runs normally, but the second cylinder model shows a singular matrix. What is the cause of this error?

[STKO Team]

here's a working version of your model:

02 cylinder.zip

(450.23 KiB) Downloaded 39 times

the singularity was due to 2 errors:

• the GJ was 0 in the fiber section -> beam singular in the Rz DOF
• there was a circle (Edge) floating without any element assigned. Probably you forgot to remove it.

there was also another mistake:
since you applied an imposed displacement (which is a single point constraint) you should use a load control. the displacement control should be used when you have an imposed load and you expect softening.
But if you apply an imposed displacement, the softening behavior can be captured with the load control.

I also added two extra edges to the inner and outer vertical faces of your solid, so that the mesh on the faces is structured and the solution is more accurate due to a regular mesh

[cqf_2232]

Hi, I used ASDEmeddedNodeElement to add stirrups to the new bond-slip model. I tried many methods but failed to mesh successfully. Please help me to see where the model needs optimization, thank you!