Topic: Switch from unbonded to bonded reinforcements

I would like to simulate (in ATENA 3D Engineering) the construction phases of a prestressed concrete element, by reproducing the following steps:

Step 1) I define a concrete macroelement;

Step 2) I define some reinforcement bars (called "primary reinforcements") and I apply to these elements a pre-stressing load, in this step the bars are unbonded so I would like to simulate this behaviour;

Step 3) The reinforcements become bonded, but i don't know how i can reproduce the change of behaviour from unbonded to bonded (i've tried to define a bond material with very low properties for the unbonded phase and to switch to a perfect bond for the second phase, but it seems that the software doesn't allow to change the bond law once it is defined for the previous construction phase);

Step 4) I define addictional bars (called "secondary reinforcements") and I try to repeat the same steps made for the primary reinforcements.

I've made several attempts to reproduce this behaviour but i still can't reproduce the switch from unbonded reinforcements to bonded. How can I do to solve this issue?

In addition, I would like to know if, in a construction phase, is it possible to remove elements (added previously) or if is it possible (always in a construction phase) to change the type of an element e.g. from external cable to reinforcement bar. I've tried to do both but somthing seems to don't work.

Thank you in advance for your help.

Re: Switch from unbonded to bonded reinforcements

Dear DLM,
I. I recommend to fist see ATENA Troubleshooting, 2.2.5 How to model bonded post-tensioning cables in ATENA?
You may be interested in the (relatively new) option "Internal Cable".

II. For an introduction in representing construction process in ATENA, please see Troubleshooting, 2.2.1 Is there an example how to change the structure during analysis to consider the construction process?

III. If you decide to work with ATENA Science, please see the description for the Condition "Elements activity" (section 5.2 Conditions) and "Show Material Activity" in Interval Data (see also ATENA-GiD User's Manual, Fig. 5-81 Interval Data window – Material activity), and the help bubbles in the corresponding dialogs.

For adding reinforcements later during the analysis, please see the option "Application from Interval", see also the ATENA-GiD User's manual, Fig. 5-64: 1D Reinforcement material properties – Element Geometry, and again the corresponding help bubbles.


Re: Switch from unbonded to bonded reinforcements

Dear dpryl,

Thank you for your answer.
I've already read the troubleshooting sections 2.2.1 and 2.2.5 but now I switched to ATENA Science + GiD.

Before simulating the test described in my previous post I decided to try to model a simpler one:

Basically, I would like to simulate the stress migration from a cable (that reaches the design prestressing force in two different steps (1 and 4) to the surronded concrete, casted (step 2) after the initial prestressing of the cable (step 1).
In particular, I have a first stage (step 1) in which I apply an amount of prestressing to the unbonded cable, in the second stage (step 2) I cast the concrete element around the cable, then in the third phase (step 3) I inject the duct (and the cable becomes bonded) finally, at the last stage (step 4), I apply additional prestressing to the cable to compress the concrete.

In these condition, having applied some force to the cable in stage 4, what I'm expecting is to have a re-distribution of this stress between cable and concrete.

I tried to obtain this result in several ways but no one seems to correctly work; in particular I made these tests:

1)I tried to switch the behaviour of the internal cable from not injected to injected (both with perfect bond and with a generic bond law) but it seems not possible to change the material law for a reinforcement bar from an interval to the following one;
2)I tried to introduce the concrete in the third stage by defining a fictitious soft material adopted for stages 1 and 2 and by changing the material with the actual one at the beginning of the stage 3;
3.1)I tried to simulate the injection by introducing two different volumes [the first one around the bar (in order to have a prism around the entire length of the cable), the second one around the prism] and then by connecting these 2 volumes with interfaces having a material (interface) that changes
from the stage 2 to stage 3 to simulate the injection of the duct;
3.2)I tried to reproduce the same test of point 3.1 by deleting the bar and by applying the force directly to the internal prism.

In all these tests i tried to apply the prestressing by means of several ways by using the following commands:
-"Prestressing for Reinf Line" or "Initial Stress for Reinf Line" for cases 1-2-3.1;
-"Load Force for Surface" for case 3.2.

I'm not able to reproduce properly the migration of the stress; further I have a lot of convergence issues, even if I am using only elastic materials except for the cable (but it is working in the elastic part of its strain-stress diagram, so basically all the elements are elastic).

Thank you in advance for your help, I am available to give you further details or, if you prefer, I can send you all these files.

Best regards,

Re: Switch from unbonded to bonded reinforcements

Dear Dario,
I. I suggest to first try the simplest approach, i.e., a bar with perfect bond + applying the prestressing as Initial Strain for Reinforcement. The casting sequence seems quite similar to the traditional wire prestressing where the wires are cut at form removal, which is usually well represented this way. Moreover, as you mention prestressing the cable before casting the concrete, I guess the cable channel is straight (not curved nor bent at some points), which means the frictional losses are not likely to be of interest.

That means steps 1-3 can be covered in a single Interval, Step 4 = additional prestressing can be applied in Int 2, again as (additional) Initial Strain.

II. If the above shows not good enough, please look at the example model demonstrating injected cables which is installed with ATENA: %Public%\Documents\ATENA Examples\Science\GiD\Tutorial.Static3D\BondCabel_Injected.gid

III. If you still have problems and need help with your particular model, you can follow Troubleshooting, 2.1.1 to send us your mdoel etc.


Re: Switch from unbonded to bonded reinforcements

Hi Dario,

It seems that your first approach was correct but you used wrong tool.

DLM wrote:

1)I tried to switch the behaviour of the internal cable from not injected to injected (both with perfect bond and with a generic bond law) but it seems not possible to change the material law for a reinforcement bar from an interval to the following one;

Probably you tried to change material in dialog "Interval data" while it is not applicable to rebars. I recommend you to check demo model which Dobromil mentioned and read Tutorial for construction process.

If you use Reinforcement Inactivity for Line condition it has to work. See this picture as example: … cpM9lqYSFG

Re: Switch from unbonded to bonded reinforcements


thank you for your help. I have followed your advices to develop a simplified version of my model and it seems to work properly.

Now I am trying to analyze the complete model (basically very similar to the simpified one but larger).

However I'm having troubles with the convergence of the analysis in the cracks developing phase.
Considering that when I was working with the simplified model I didn't have this kind of problems, I think that there are some solution parameters to be set.

I have done a lot of tests in order to find the problem but no one seems to work.

Could I send you my model in order to have a general check?

Thank you in advance for your help.

Re: Switch from unbonded to bonded reinforcements

Hi Dario,

Of course you would better share your model, otherwise it is difficult to identify your problem. You can upload the model to any filesharing service.

Re: Switch from unbonded to bonded reinforcements

Thank you,

here you can download the file created with GiD

I am available for any further information.

9 (edited by pavlo 2019-11-01 07:42:00)

Re: Switch from unbonded to bonded reinforcements


I have noticed some mistakes which should be corrected before running analysis.

1. Boundary conditions are defined in all intervals rather that defining them in first and use in subsequent intervals. Moreover, boundary conditions differ in each interval which makes no sense to me. See clause 6 for details.

2. In order to understand your model I need description of each interval: what do you expect from each one. I recommend always describing your models in Utilities - Tools - Notes. It will create a simple txt file in model folder. You will be able to read your notes even after 5 years and understand your model easily.

3. I understood your intervals like this:
Int 1 - application of 2.45 MPa tension to beam end
Int 2 - prestressing of cables Cavo 4 with initial strain defined as a bilinear function... I would better define exact prestressing value in Conditions rather than multiplying unit strain in Interval data.
Int 3 - application of displacement to the beam end (1 mm) with bilinear function and activation of other cables. It is strange to me why you firstly applied load at Interval 1, and then displacement... Also it seems that you unintentionally defined a function instead of linear application of displacement. Cables Cavo 12 and 16 seems not prestressed...
Int 4 - Same as Int 3 but 0.5 mm. Also you added some restraints at beam edges... You don't need to assign displacement twice, you can use Add Additional Load Cases in Interval Data or even easier: Define Load History in Interval Data. So Interval 4 can be omitted and fully replaced by interval 3.
Int 5 - Application of 160 mm displacement!!! Is there any mistake? Anyway, you can combine this interval with 3 and 4 as well.

4. I haven't found any self weight...

5. I havent found any switch from unbonded to bonded which you intended to apply...

6. It seems that your problem is something like this:
I. beam manufacturing
II. tendon prestressing
III. grouting of tendons
IV. loading up to failure

If so, I recommend you to arrange your intervals like this:
I. self weight and boundary conditions. Delete BC Data after calculation in Interval Data should be UNCHECKED in order to use boundary cond in subsequent intervals.
II. reinforcement activity for tendons (they appear and are prestressed with initial stress). Add Additional load cases should be CHECKED and in tab Additional Load Cases you define Load Case id=1, Multiplier = 0 (in order not to copy self weight but only boundary conditions). Hence, you don't need to copy bound cond in each interval!
III. tendons change material to bonded with the use of reinforcement activity. Don't forget about Additional Load cases.
IV. loading with uniform or non uniform steps up to failure. Don't forget about Additional Load cases.

7. If it is an experiment which was perfomed in reality, you would better share the experiment details. I could help you modify the model.

8. there is no end anchors for rebars which might lead to stress concentrations at tendon ends and convergency problems.

9. tensile load is applied to the concrete surface directly. How do you expect it in reality?

Best regards.


Re: Switch from unbonded to bonded reinforcements

Good morning pavlo,

Thank you for your help. Below I will try to explain my choices.

-    Reply to Point 1:
I define the BC in each interval because it is more comfortable for me, since I don't understand how to assign an ID to a condition (boundary, load or anything else), then currently I am not able to use te tab "Additional Load Cases". If this can affect the results of the analysis, could you explain me how can I assign an ID to a condition? In general, I need of a guide about the management of the Additional Load Case tab.
I am learning to use ATENA Science + GiD, but I did not find any reference in the related manual or in the troubleshooting manual about this issue.
-    Reply to Point 2:
I will send you the model with the description of I want to do in each interval and further details in order to help you in the understanding of my problem.
-    Reply to Point 3:
About your comment in Int 2: In general, I apply the loads (prestressing, displacements etc...) as unitary loads and then I apply the multiplier in the interval data because I don't know hot to display in GiD the magnitude of the applied loads then, in this way I know that they are applied to the model as unitary loads and then I read the multiplier in the Interval data (clearly it works if I have just 1 load per ecah interval, as in this case). If there is a way to display the magnitude of the load in GiD, could you explain to me how to do it?
About the application of the loads in terms of force or displacements: I apply force in Interval 1 and displacements in Int 3,4,5 because I think that it is better (in Intervals 4 and 5) to execute the test in displacement control in order to avoid convergency issues due to the nonlinear behaviour developed in these intervals.
About the further horizontal constraints applied in Interval 4, I have added them because in the simplified model (that I have modeled before to run this test) I have found that for high axial displacements (in tension), the model showed a non-symmetrical cracks pattern (probably due to numerical rounding) which led to non-symmetrcial displacements f the structure (even if the loads, the geometry and the mesh are symmetrical). Then I have decided to apply these constraints, checking that their presence did not affect significatively the stress distribution in the model.
About your comments in Int 3 and Int 4: I divided the displacement application in two intervals because with the displacement applied in Int 3, the structure has still a linear behaviour while, with the additional displacement applied in Int 4, concrete reaches the tensile strength and then I subdivided this interval in more steps in order to avoid convergency issues.
About your comment in Int 5: The magnitude of the displacement is correct, since I want to evaluate the behaviour up to the failure in tension of the reinforcements. In particular, I have assigned an ultimate strain to the reinforcements equal to 2.5%, having the bars a length of 7.6m (ecxluding the parts in correspondence of the steel plates) they have an ultimate elongation of about 0.025x7600mm=190mm, very close to the sum of the displacemens applied in Int 3,4,5=175mm.
-    Reply to Point 4:
Self weight it is not applied because I am not interested about its effect.

-    Reply to Point 5:
There is not any switch from unbonded to bonded because I had some troubles in the definition of this switch then, in order to simplify the analysis, I have found a way to bypass the grouting of the tendons by redefining the loading phases and by translating the consitutive laws of the materials used for the tendons (You will find more details in the notes that I will send you privately after this reply).
-    Reply to Point 6:
In general the phases of my model are the ones identified by you. About your recommendations, I can follow them but, as I have already said in the Reply to Point 1, currently I am not able to use the additional load case tab then, at this time I do not know how to manage additional load cases in an interval.
-    Reply to Point 7:
This model is referred to an actual structure, but I prefer to give you further information privately. You will find them in the notes of the GiD model that I will send you after this reply.
-    Reply to Point 8:
Up to now this condition does not seem to affect the convergency, since I see concentration of stresses near the interface between elastic concrete and the actual concrete, while at the end of the reinforcements this concentration seems to be less conditioning, also because I have modelled two steel plates at the beginning and at the end of the model in order to spread the stresses. In any case, if you think that they can affect the results, could you help me to model the anchors for the reinforcements?
-    Reply to Point 9:
This is what I expect in reality, even if I know that this could lead to convergency issues specially for the concrete elements far from tendons or reinforcements.

I want to ask you if I can send you my model privately this time, since it contains confidential information. Could you igive me an e-mail address?
Thank you for your support, I am available for any further details.

Best regards,

Re: Switch from unbonded to bonded reinforcements

The problem has been solved: Newton Raphson had to be used instead of Arc Length.