Dear Fcil,
1. we recommend to make the "wrap" smaller (ar the mesh in it coarser) such that there is just a single element where the bar end is anchored (as you are not interested in calculating bond slip in the wrap...).

2. I don't get why you prefer to show Principal Stress for 1D elements, which only have a single stress component (SigmaXX)?

3. Are you displaying the bar stress in [Global] Nodes or Element Nodes?
Usually, Element Nodes give the more interesting/useful picture (this prevents averaging the values between neighbouring elements).

4. I am not sure what you mean by "monitor point of strength of the bar"? For the multilinear plastic law, there is nothing like the current Tensile Strength for the Cem2 material model family...

Regards.

Dear Fcil,
it is still not 100% clear what you are comparing to what? I assume "main" is a typo, meaning "mean" (or average).

Simply said, if you wish to compare the calculated results to an experimental measurement which gives you some average bond stress, you should calculate the average bond stress from the analysis results the same way as when evaluating the experiment.

Do I understand that to make a check, you are summing the bond stresses along the bar to verify you get the total Reaction? And that you choose a step when the stresses are almost constant along the bonded length of the bar, such that the calculation becomes very simple?

You need to pay special attention to the part near the end of the bonded segment, where the bar continues "through the air" - as the unbonded segment is quite long compared to the segments in each element, a small difference in the bond stress can make a relatively large difference in the sum (resulting force). Yes, the bond stress has to be 0 in the air, but when you display results in [global] nodes, the neighbouring values get averaged (that is why Element Nodes display probably makes more sense in this case).

Regards.

Dear Fcil, if you still can not identify the source of the difference, you can send us your latest model along with information at which load step you do the check, and your hand/spreadsheet calculation.

Regards.

Dear Fcil,
1. for quicker checking, the "Bond Force" output data item may also be of your interest.

2. Thank you very much for careful checking and reporting the problem. It looks like the problem is really related to the long "through the air" segment, where the bond stress gets interpolated from the 2 ends. We at least need to better explain this in our documentation (Troubleshooting, 2.2.12.3.2 Unrealistic bond stresses along unbonded segments)!

As the solution suggested there can not be directly applied in ATENA Egr 2D, I only see the following way:

I. Add a small elastic cube or triangle around the bar, just underneath the end of the bonded segment.

II. End the bar inside that triangle.

III. Create another bar, with perfect bond, from the endpoint of the above bar, till the original bar end in the "wrap".

The problem is that if you make the distance from the surface too short, the extremely short bar segment brings extreme stiffness differences in the model, resulting in numerical problems. Something like 1/2 of the element size in the concrete should work.
Fixing a node of the triangle in horizontal direction helps to avoid unrealistic horizontal displacements.

I am sending my model through email such that you can look at it and make further modifications.

Regards.