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,
Manish

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, 2.2.10.1 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.

Regards.

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, 5.3.5.1 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

geometry?

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

condition.

6. Also, according to ATENA-GiD User's manual, 5.3.5.1, 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.

Regards,
Manish

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.

Regards.