Bar Pull-out analysis in Ansys

  • Last Post 18 January 2018
  • Topic Is Solved
Osamashakil posted this 15 January 2018

I have done non-linear analysis by applying displacement of 4mm in 10 substeps. When I check the force needed for the displacement it keeps on increasing with time. But in actually force should first increase then decrease. I m using "frictional contact" between rebar and concrete can someone tell me possible reason for this issue? I think bar is yielding instead of pulling out.


Order By: Standard | Newest | Votes
peteroznewman posted this 15 January 2018

What is the geometry of the rebar?  Did you include plasticity in the steel material? Does the rebar have a smooth cylindrical shape? If so, what is the diameter of the bar compared with the hole? If they were equal, how were you generating a normal force to create friction? If you have a deliberate interference, it is possible the frictional force is greater than the yield strength of the steel.

What is the element count around each circle? What shaped elements are you using (tet or hex)? With a coarse mesh, it is possible to create contact angles between the faces that are not 90 degrees with the centerline.

You can using the Attach button to upload a Workbench Project Archive file (.wbpz) to you post if it is less than 120 MB.  In Mechanical, right click on Mesh to select Clear Generated Data, then save your model before using File, Archive in Workbench to create the smallest archive file size.

  • Liked by
  • Osamashakil
Osamashakil posted this 15 January 2018

Thanks for your response,

Rebar diameter is 10mm, (11.3mm including ribs). I have not included plasticity in steel material. Rebar has smooth cylindrical shape. Diameter of hole is exactly equal to diameter of rebar, that is why I was trying to use offsets in contact tool, but it is not working as well.

Meshing type is tex and count is 20 approx, changing mesh is not working as well.

I think there is an issue with contact or properties of material and as you mentioned with hole size issue.

I have attached the project with reply (dropbox link)

I will be very thankful if you give me an idea how to proceed.

peteroznewman posted this 15 January 2018

I watched the video below to see how a pull test for rebar in concrete fails.

I see the concrete fractures around the rebar.

An Explicit Dynamics model can remove an element from the model when it has exceeded its failure strength. I performed a few simulations that you can see in this post.

I downloaded the rar file you left in the dropbox. I have 7-zip software which has successfully opened other rar files, but it could not open the rar file.  You can try to use the directions in the previous post to create a .wbpz file and use the Attach button to upload it to your post. 

If your model is a Static Structural model, that does not remove an element that has failed like Explicit Dynamics can.  There is an ACT extension called EKILL that does, but I have not tried it.  So given that the concrete elements don't fail then get removed, I would expect the force in the simulation just keeps increasing and does not decrease like the experimental data does.


  • Liked by
  • Osamashakil
Osamashakil posted this 15 January 2018

Thanks for sharing it.

But can you tell me in my model where hole in concrete is exactly equal to concrete, what should I do for it?

Osamashakil posted this 15 January 2018

My prof. asked me last time to use static structural model.

I have emailed you the Ansys file.

its wpbj. 

please have a look.

peteroznewman posted this 15 January 2018

The wpbj file is not sufficient, there is a folder with the same name that is required.  In Workbench, use File, Archive... and that will combine the .wbpj file and the folder into a single file with a .wbpz file extension. That is just like a rar or zip archive. You can Attach that file type to these posts.  Below is the concrete with rebar compression failure model I have a video in this post.

Attached Files

Osamashakil posted this 15 January 2018

sorry, I understood it now. 

I have attached now.

Osamashakil posted this 16 January 2018

Please check this file and let me know abt any issue you find in it. Also please let me know possible the possible way of same opening size issue or if there is a material issue.

peteroznewman posted this 16 January 2018

What is the goal of your simulation? When I perform a simulation, it is usually to predict the load at which failure would occur, and compare that with the expected service load to calculate a factor of safety. With that goal, I don't need to simulate the behavior of the system beyond the point of failure. That is why a Static Structural model is sufficient to predict the factor of safety. You are not going to see the concrete fracture in the simulation, and the load on the rebar suddenly drop to zero like you see in the physical test because the model doesn't include the ability to simulate element failure, but that is acceptable if your goal is to predict if the design is safe and will be far from failing under the design loads.

I may need nonlinear properties like plasticity in a model, because failure may be defined as collapse, while a test may permanently bend the structure but a small deformation is permitted since it is not a collapse. For this goal, Static Structural is a good tool. Rarely do I want to predict the behavior after failure, but when I do, Explicit Dynamics may be required to simulate element failure and removal from the model during the post failure simulation of the collapse, or in your case, fracture of the concrete.

If your goal is to predict the load at which failure would occur, then I would expect you would plot the Maximum Principal Stress in the concrete, but you have no result for that. Since concrete is a brittle material you would check when the Maximum Principal Stress exceeds the Tensile Ultimate Strength and the Minimum Principle Stress magnitude exceeds the Compressive Ultimate Strength.

I perform a mesh refinement study manually. I solve the model, get a result, make the elements smaller, solve the model, get a result and repeat this until the result doesn't change very much. The result I am tracking is usually stress. Here is one post on the topicHere is another example.  I see you have added Adaptive Mesh Refinement to your solution, which can be an automated way to accomplish a mesh refinement study. I haven't used that before, so I was glad to see it in your model. However, you selected maximum displacement to converge on, and that always occurs on the face of the rebar where you put the displacement load. That defeats the purpose of the Adaptive Mesh Refinement. You want Maximum Principal Stress to be the quantity to converge on.

In your model, you are requesting stress in the same face of the rebar that you are applying the displacement. That is never a good idea. Important results in the model should not be occurring near an applied boundary condition. If you request the stress in the body of the rebar, you will find it is much higher elsewhere, like where it is in contact with the concrete. You are only requesting Normal stress in the rebar. If you want the average stress, you know the diameter and area and have the Force Reaction, so you can calculate the average normal stress by dividing the force by the area.

In your geometry, you have three solids in one component for the concrete, and Topology is set to Share. That means the nodes on the shared face will be common and that is like there is just one big block with deep holes and rebar cast around the center portion. Is that the physical sample, or is the physical sample three pieces of concrete?  If it is really one big block, you probably don't need such a large block since the failure will occur in a very small volume near the center.

Another observation is that the rebar is axisymmetric and so is your load and support. That means you could build this as an axisymmetric model and save a lot of time solving.

Osamashakil posted this 16 January 2018

Thank you for checking my model. My main aim is to draw force-slip curve. The stress you mentioned at tip of rebar, I m not actually using it. Actually I m checking reaction of the fixed support. That reaction is equal to the force experienced by rebar. I m giving displacement to rebar, according to literature when displacement is given to rebar , the concrete-steel bond experience change. Force required to produce a particular displacement 1st increases, but when bar slip occurs, force will decrease. I just want to plot force vs time first. But what I have seen, the force keeps on increasing (probably bond is not breaking, otherwise force would increase first and then decrease). Meahing is an issue as well, but still I think there is something other wrong, which causing this problem. In geometry, 3 parts are bcz I sliced it and then connected it. I did it bcz I wanted fine meshing in bond area, which is 20mm (so physically it is one big concrete block) So if I able to get Force-time curve, I will convert that force to bond-stras and plot it with slip (displacement of rebar-concrete) ,it will be curve. But initially I m getting linear relationship between force and time, which must be different, first increase then decrease, usually after 1.5mm of displacement force starts decreasing, according to literature.

peteroznewman posted this 16 January 2018

I found a relevant article. It has an informative introduction that I copy below...

Adherence is usually subdivided in three parts: adhesion, friction and mechanical. This subdivision is based on the bond stress-slip relationship, as shown in Figure 1. In this figure, s1, s2 and su represent the slip relative to the bond stress due to adhesion (τ1), to friction (τ2), and to mechanical anchorage (τu), respectively.

Adhesion bonding, also called chemical adhesion, corresponds to the initial part (rather inclined) of the curve and consists of the resistance to the shear stress between the concrete and steel particles. It occurs due to the physic-chemical connections between the bar and the cement paste formed during the bonding. In comparison with the other parts of the bonding, adhesion is rather small, being destructed as soon as the first slip between steel and concrete occurs.

Friction bonding occurs when a material tends to slip in relation to another one. However, it depends on the friction coefficient of the steel-concrete interface and on the surface roughness of the steel bar. The mechanical bonding is represented by the last upward sloping part of the curve shown in Figure 1. This part is due to the existence of irregularities at the bar's surface that function as support points. This means that the more irregular the bar's surface structure, the higher the mechanical bonding, since a so-called 'wedging effect' will take place. The part related to mechanical bonding is the main reason for the anchoring of ribbed steel bars in concrete, providing a certain post-peak resistance, and varying in function of the inclination, height and the distance between the ribs.

You are not simulating the adhesion bond between the concrete and steel in your model. You are only simulating the friction and mechanical wedging action of the ribs in the rebar on the matching faces of the concrete, which gets you to the peak of the curve in Figure 1. The decreasing side of the curve is when the concrete fractures as it reaches its Ultimate Tensile Strength.  A Static Structural model is not going to show you the concrete fracturing, so yes, you will see an ever increasing graph of Force-Displacement.  If you plot Maximum Principle Stress vs Force, you will then know the force at which failure will occur.

Please followup with other questions. I am creating a 2D Axisymmetric model size to show you and will post that later.

peteroznewman posted this 16 January 2018

Concrete in your model has a UTS of 4 MPa.  I applied 10,000 N to a 2D Axisymmetric model and found that at 6,400 N, the Concrete Maximum Principal Stress reached 4 MPa, so that is where the peak of the curve in Figure 1 is estimated to be.

I didn't do a mesh refinement study, and this is a somewhat coarse mesh. Unfortunately, if you were to run a mesh refinement study, the stress would keep increasing at the 6,400 N load because there is a sharp interior corner and that represents a stress singularity in the model. You have to add a small radius to the geometry to get rid of the singularity.

I have attached the archive to this post.

Attached Files

Osamashakil posted this 16 January 2018

Thank you so much for detailed answer and clearing my concepts as well. 2 short question now I have:

1) If I want to move on with static analysis, should I use non-linear material (steel & concrete). As I have seen when I use concrete NL, it doesn't give any input for compressive strength, so I dont know which strength it is using.

2) In my case diameter of the opening is same as diameter of rebar. Is there any issue with that? or what should I do for that?

peteroznewman posted this 17 January 2018

1) In a Static Structural model, Concrete and Concrete NL are identical materials. They are both linear materials that only have a Young's modulus and Poisson's ratio. The entry for Tensile Ultimate Strength doesn't change the solution result, so the solver is not "using" that value. It is only there in post processing of the results to divide by the maximum stress to calculate a Safety Factor in the Stress Tool. I don't use that myself. I prefer to plot the Stress rather than the Safety Factor.

If you create an Explicit Dynamics model, then the Concrete NL has a Tensile Pressure Failure criterion that allows elements to fail during the simulation. Now the solver is using the failure criteria by taking out elements that have exceeded the value of Maximum Tensile Pressure shown in the materials data.

2) The diameter of the concrete should be the same as the diameter of the rebar because the concrete was cast around the rebar and formed a bond with it. The bond is not represented in the model, but the mechanical wedging action of the contact of the ribs is in the model and supports a high pullout force.

Shivani posted this 17 January 2018


I have been recently given a pull out test simulation but I have to perform using different material.I am trying to get the result for the value of force at which the the cube or the bolt fails but haven't been successful.It would be a great help if you let me know how are you applying the boundary conditions to your geometry and what kind of results are you plotting after the simulation.

Thank you.

Osamashakil posted this 17 January 2018

Thank you so much peteroznewman for such a great help!! You have cleared my concepts and my ambiguities as well.

Osamashakil posted this 17 January 2018

Hi Shivani, I have applied fixed support at top face of concrete block. Then i m plotting reaction force on fixed support with respect to time.

peteroznewman posted this 17 January 2018

I ran the Axisymmetric model of rebar being pulled in Explicit Dynamics with three materials, two with different failure criterion, one with no failure criterion.

CONC-35MPA from the Explicit materials library,


Concrete NL from the General Non-linear library


Structural Steel - No failure criterion in material model

  • Liked by
  • pgl
  • Osamashakil
Shivani posted this 18 January 2018

Thank you for your help.

And also could you please tell me if you used explicit analysis or static structural analysis for the problem?

Shivani posted this 18 January 2018

Thank you peteroznewman for your help.

I had been trying to simulate it static structural but now that you told me explicit simulation would be more useful,I am trying to learn how to do that.Are thereif there are any videos or materials,in your knowledge, that would help me to understand using explicit dynamics.

Osamashakil posted this 18 January 2018


I have done static structural analysis.

Osamashakil posted this 18 January 2018


Thanks, videos are helpful to make a picture in mind.