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)


Due to restriction by Gmail, I have shared a folder (titled "FilesFromManishRoy") with all the files using google drive (shared with


Dear Dobromil,

I have developed the pullout model and ran it (GiD 11.0.8/ATENA 5.6.i1). To save on computational cost I modeled only a part of the specimen. I am not modeling the support bar. I am going to send you all the files through emails. My peak pullout load is much lower than the peak experimental load. My concrete (UHPC) has fibers as smeared reinforcement and I am trying to run the simulation with fibers aligned in the load direction (the attached input file has the complete fiber stress-strain values, which I provide by editing the input file). I understand that the fiber alignment in the experiment might not be an ideal scenario and hence, my simulation results may not exactly match the experimental results. However, it would be great if you could have a look at the model and advise if I need to modify anything.

Thanks and regards,


Dear Manish,
ad 1.: make sure there is only a single element generated for the bar (would behave like chain if meshed finer in GiD - see also Trpubleshooting, 2.1.21 When I model the reinforcement, do the bars and stirrups have to be in geometric connection (with common intersection points) or they can be modeled according to their axis so that they do not touch one the other in geometric sense?).

Ad 2.: For a finer mesh, if you suspect/find out that the fact of "squeezing" the bar cross section into a smaller volume has too large adverse effect on the results, you can represent the bar with multiple 1-d bar elements (see also Troubleshooting, Bending).

Ad 3.: The perimeter is used for bond. And the artificial cut of the bar at the symmetry plane is not expected to add to the bond surface?

Ad 4.: Check the line using the List command - will see there the point numbers of the Start and End.

Ad 5.: Please send a sketch (or 2). Just guessing: You assign the symmetry condition to a Surface, and therefore no Lines are touched by this = no need to hide them while assigning.

Ad 6.: Yes - any slip through the symmetry plane would actually mean breaking the symmetry assumptions.



Dear Dobromil,

Thanks for your response. I have a few follow-up questions mentioned below:

1. Since there is no need to assign a symmetry condition directly to an embedded bar, I

should not worry about the portion of the pullout bar that is in the air (in between the

concrete prism and the end elastic cube). Is my understanding correct? (I know 1D bar has

only axial stiffness; however, I would like to get the concept clear.)

2. Ref.: Troubleshooting, 2.1.21 - If my reinforcement bar diameter is 12.5 mm, does it

mean that the finite element size of the surrounding concrete material should be at least

12.5 mm or larger?

3. Yes, for a bar in one symmetry plane (in my pullout example) I set the number of

profiles under the "Basic" tab of 1D Reinforcement material card as 0.5 in order for the

program to calculate the bar area correctly. However, should not the "Bar Perimeter"

under the "Bar With Bond" tab be (1/2*pi*bar dia + bar dia)? The program calculates only

(1/2*pi*bar dia) as the perimeter.

4. I understand from ATENA-GiD User's manual, that the end of the pullout bar

inside the elastic cube should be fixed (no slip). However, what end does the program

consider as "Start"? Is it the starting point (co-ordinate) while I create the line


5. Also, I need to model a tensile test of a UHPC prism specimen with embedded rebar. I

am trying to model the portion of the specimen between the gauges. Hence, I can use 1/8

symmetry. My question is when I apply the symmetry condition or the load (in terms of

prescribed displacement) condition, should I turn the rebar layer off so that the

symmetry and load conditions are applied to the concrete surfaces only? Or it does not

matter? The same question applies to the pullout model, as well, for the symmetry


6. Also, according to ATENA-GiD User's manual,, the bar end at the symmetry plane

of the tensile specimen should be Fixed (bond slip blocked). Is my understanding correct?

Thank you again for your time and help.



Dear Manish Roy,
ad 1.+2.: There is no need to assign a symmetry condition directly to an embedded bar, see also Troubleshooting, 2.1.21 When I model the reinforcement, do the bars and stirrups have to be in geometric connection (with common intersection points) or they can be modeled according to their axis so that they do not touch one the other in geometric sense?

However, for a bar in the symmetry plane, one should set the Number of Bars to 0.5, as only 1/2 of its cross section lies inside the part being modelled.




I am trying to model the pullout behavior of a reinforcement bar (as 1-D discrete bar) embedded in UHPC using GiD 11.0.8 as the pre-processor and ATENA 5.6.1i as the FE program. Because of the geometry and load conditions in the experiment, I would like to employ symmetry boundary condition in the simulation. I am going to send the sketch of the specimen as well as the picture of the test set-up to soon after posting this message.

After reading the clause "2.2.12 How can I model a pull-out experiment?" in the ATENA Troubleshooting manual I have the following questions:
1. If the symmetry line runs through the middle longitudinal bars, will it be a problem to assign symmetry boundary condition to the discrete bars (lines)?
2. Since I need to apply symmetry boundary condition to the concrete surface as well, will this condition conflict with the line symmetry condition on the discrete bars?

I have tried to run the model (created according to the clause 2.2.12 in the ATENA Troubleshooting manua) using the above conditions but the execution is aborting right after the first step. Hence, I would like to eliminate the problems causing the early termination of the analysis.

Thank you,
Manish Roy