Concrete Rod Contact Simulation

  • Last Post 2 days ago
jacks3215 posted this 23 April 2018

I intend to carry out simulation of rod pull-out from cement block. The rod embedded 1mm in the concrete block. I followed two threads related to pullout at these links bar pullout analysis; and bar pullout explicit

I have experimental results which I would like to verify from simulation. Although the theory is explained in the above mentioned threads but for confirmation I am writing here as well. The concrete block is fixed and displacement (say 0.5mm/min) is applied at the free end of the rod. We get resultant of force (y-axis in N or cN) and displacement (x-axis in mm) curve. The results although all are for rod pullout but of the following different types;

(1). Initial increase in load until debonding occurs. At the debonding the load drops and from there starts the frictional bond which leads to either (i) rod pulled out completely or (ii) rod being broken at the pullout stage because the rod strength is reached before being pulled out completely.

(2). Rod breaks/ruptures before debonding because the rod ultimate tensile strength is reached.

I would like to perform separate simulations for all of the above mentioned cases. I could enter different values for ultimate tensile strength (apparent strength) of rod (from experimental results) for each of the above mentioned case which I think would help in determining the rupture point for the rod.

I tried running the simulation in static structural but the results are none. I am not getting any force reaction value, must be something I have missed. The explicit dynamics took much long time on my pc so I could not test the results. I will try it again once I could get idea that where am I doing wrong. I am looking forward for guidance. 

The archive is attached here,

Thank you

Order By: Standard | Newest | Votes
peteroznewman posted this 24 April 2018

You say "displacement is applied at the free end of the rod", but in both your models, you have applied a displacement on the entire cylindrical surface of the rod, not the free end. This makes the rod behave like a rigid body instead of an elastic member and prevents the rod from failing. You should instead apply the displacement to the flat end of the rod where it leaves the clamp.

Both models also apply a Fixed Support to the entire top face of the concrete block, and prevent that face from failing. How is the experimental block prevented from moving up?  I expect some portion of the top face of the concrete block makes contact with a couple of plates that prevent upward motion. You need to model the plates, or at least split the top face of the concrete block where the plate prevents upward motion.

jacks3215 posted this 24 April 2018

Thank you for your reply.

In experimental setup the bottom part of the concrete was glued on to the specimen holder. That specimen holder was clamped by the grip of the testing machine, so no external force was acting on the concrete body. The glue prevented the concrete from moving upwards. In this case, shall I apply fixed support at the bottom face of the concrete instead of the top face?

In addition, please provide guidance on how shall I get the load-displacement curve in the solution? Is the applied reaction force on the top face is fine to get the load?

peteroznewman posted this 24 April 2018

In this case, shall I apply fixed support at the bottom face of the concrete instead of the top face?

Yes!  Why would you even think to put it on the top face? A simulation should replicate a physical setup as much as possible.


how shall I get the load-displacement curve in the solution?

If you apply a displacement (or velocity in a dynamics solver) to a face, you can request the reaction force in the results.
This doesn't seem to work in Explicit Dynamics so I need to figure out how to get that data out.

jacks3215 posted this 26 April 2018

If you apply a displacement (or velocity in a dynamics solver) to a face, you can request the reaction force in the results.
This doesn't seem to work in Explicit Dynamics so I need to figure out how to get that data out.


I hope to have your guidance on getting the resultant data soon

jacks3215 posted this 29 April 2018

Some of the references used cohesive zone modeling, I tired it in my model but still cant figure out the getting the required resultant data..


Apart from this, how can I model interfacial transition zone (linear elastic, third phase, having thickness in um) between concrete and the rod in Ansys?

peteroznewman posted this 29 April 2018

Here is how to get Force Reactions from Explicit Dynamics Support Boundary Conditions in 18.2

1) In Workbench, goto Tools-->Options -->Appearance and check on "Beta Options"

2) In Mechanical, Clear the results

3) Right-click on "Solution Information" --> Insert   (this is the list of Result Tracker items)

4) Choose "Force Reaction"

5) In the Force Reaction, choose which boundary condition.  Then solve.


I will have to do some research on your interfacial zone question and make another post when I have an answer.

  • Liked by
  • jacks3215
jacks3215 posted this 03 May 2018

I would like to ask some questions, a bit confused after checking some more references.

(1). In some references, researchers have applied load instead of displacement while some have applied displacement instead of load. So the possibilities are these two methods. When I apply displacement (or velocity), the same value as that of experiments, the reaction force is too less. I have tried in both static and explicit but still, the results are not as per expectation. What could be the possible reason? I have attached the model, you may kindly help me check it.The explicit results are a bit strange to me, although I have checked the previous thread on the explicit result of bar analysis but still can not figure out the problem.

(2). Some references have mentioned the applied load in sub-steps. Also, some have used cohesive zone modeling (CZM), traction-separation based modeling. But I can’t find such options available in explicit dynamics. Are these options specific to static structural only?

(3). If the answer to the last question is yes, then why do we carry out the simulation in explicit dynamics? Isn’t there the possibility of getting required results in static structural?

(4). From the experimental results, I had the values of chemical bond (J/m^2), frictional bond (MPa), fiber apparent strength, shouldn't I be entering these values in simulation for the interface?

(5). Regarding my question on ITZ (interfacial transition zone), I think this reference (Link here) might be useful for discussion on the design of ITZ.


peteroznewman posted this 03 May 2018

I have some quick answers that I can provide without looking at your model or doing any research:

(1) In Explicit Dynamics, the solver is using mass and acceleration. Some of the reaction force at a support that is in a static analysis is used to accelerate the mass, which is why it can be less than expected. You say you have tried static, and got less reaction force than expected. I don't understand that. If you have a system that is fixed at one end and you apply a tensioni force F at the other end, then the reaction force must be F in a static analysis.  When inducing damage, I prefer to apply a displacement since the model will continue to solve past the point when the force vs. displacement curve reaches a peak and the slope goes negative.  An applied force can't go past that peak. 

(2) Yes, you should use sub-steps to help the Static Structural solver converge. I don't know if CZM is available in Explicit.

(3) Yes, you could build a model in Static Sturctural, maybe in several pieces. One model for the CZM portion, another model for after the bond between steel and concrete has failed and there is just the mechanical shape of the ribs on the steel holding the rebar in the concrete. This second portion is when you need element death in order to allow cracks to develop in the concrete to make space for the ribs on the rebar to escape their confinement. Explicit Dynamics has element death built in and on by default, so that part of the model is easy to do.  Getting useful force reactions out is the difficult part in Explicit Dynamics, while that is the easy part in Static Structural.  The difficult part in Static Structural is element death, but there is a way. See the ekill script example in my tutorial for consideration of another approach to your model.

(4) I've never done a CZM model, so I don't know.

(5) I've never done a ITZ model, so I hope the reference is useful.



  • Liked by
  • jacks3215
jacks3215 posted this 2 days ago

I tried using the Cohesive Zone Model (CZM) for pullout. But I can not assign CZM Bilinear and CZM Exponential to my model. However, the CZM Separation and CZM Fracture can be assigned to the contact debonding.

I read some other people work and they have used CZM for modeling pullout with zero thick interface, as also suggested by @bsista here. But within their model, they have used either CZM Bilinear or CZM Exponential, both of which I am unable to assign to my model. In addition, the Inter205 has been used mostly for the interface debonding.

Please someone who has experience on CZM guide me on my mistakes. I intend to verify the experimental results which are somewhat like this image.

Model is here