You are not logged in. Please login or register.

Forum updated

We have recently updated our forums system, and we have cleared all spam topics and users. In case we accidentally deleted your account, please register again. If you miss a topic you have posted before, please let us know.

Post new reply

Post new reply

Compose and post your new reply

You may use: BBCode Smilies

All fields with bold label must be completed before the form is submitted.

Required information for guests

Required information

Topic review (newest first)


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, 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.



Dear dpryl,

here is the folder sharing link: … sp=sharing

In the link, there is the latest model, a photo of step 19 (to easily calculate the mean of the bond stress because you can see the reaction and the bond stress (almost constant) on the embedded bar).

Furthermore, there is my excel file that I use to have a graph of the bond slip - bond stress curve of:

- Test CL0-S1 curve (the curve of the real experiment);

- Modelling results (the curve carried out reading the displacement from the first node of the embedded bar, node 523, and the
                             stress from the farthest node of the embedded bar, node 513);

- Mean value of bond strength (the curve carried out reading the displacement from the first node of the embedded bar, node
                                               523, and the mean stress carried out using the formula τ=F/Dl*Pi*lbond with the reaction as F)

So I'm checking at the "Step 19" and the bar diameter is 12 mm and the embedded bar is 100 mm.

Thank you for your support,

best 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.



Dear dprly,

yes was a typo, the right word is "mean", I'm sorry.
So I have (as in the real experiment) to calculate the mean of the bond stress with:


where F is the reaction that I take from the monitoring point, at the step when the stresses are almost constant along the bonded length of the bar.

The mean of the bond stress as to be similar to the bond stress (almost constant along the bonded length of the bar) that I read on the embedded bar in the same step.

At that step, the result that I read on the embedded bar is as I expected and modelled (1.90 MPa), but when I calculate the mean using the formula above written, it doesn't match at all. It's almost double.

Can you help me to understand why?

Thank you for your help,

best 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).



Dear dpryl,

first of all, thank you for your answer.

For the points 1 and 2, thank you, I will follow your suggestion to see if I can have different results.

About 3 and 4 (it was stress, not strength, I made a mistake). I'm sorry if I wasn't clear, I'll explain it better.

What I'm trying to do, is to have as an output the main of bond stress. Because I'm studying a real experiment so I can't read the value from the point in the program, instead, I have to use the main of the stress in the bar (that should be the same) through;


where τ is the bond strength in [MPa], F is the applied force in [N], Dl is the nominal diameter of the longitudinal rebar in [mm], lbond is the bond length in [mm] and Pi (3.14).

But when I use the reaction at the wrap (so the applied force) coming from my monitoring point, the results don't match with the Bond stress that I read in the bar when is constant in all the embedded bar (this one right in the value expected).

So I tried to use the Principal stress to see if the force was right, but still, I don't get why if I use the reaction the main value don't is the same of the value read in the embedded bar.

Best regards,



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...



Dear all,

I modelled a pull-out experiment, following the ATENA's manual. To model the unbonded segments I chose to make a (rectangular) hole in the concrete, as suggested in the "ATENA-Troubleshooting".

The model works good, but doing this, there is a problem in the way the program read the principal stress at the beginning of the embedded bar. There is a big jump of value for an unreasonable value to a more expected one. I was able to improve the precision of the value whit the incrementation of the mesh near the point.

I would like to know if there is a way to prevent this without implementing the meshing or this situation is normal. Furthermore, there is a way to put a monitor point of strength of the bar?

If you prefer, please have a view of my ATENA file and the output graphics (with and without refined mesh): … sp=sharing

Best regards,