Concrete Rod Contact Simulation

  • 302 Views
  • Last Post 4 weeks 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,

https://drive.google.com/open?id=18NyzKDZLjOOm5ttptzMdz2knMo3O6bPY

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.

https://drive.google.com/open?id=1MkjnqaNOnklaWuLHcsjWPhuUgYjfMMkM

(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.

Regards,

Peter

  • Liked by
  • jacks3215
jacks3215 posted this 14 August 2018

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.

Model is here

 

jacks3215 posted this 21 August 2018

I am having the convergence issue in my model (attached here). I tried changing the mesh size and steps but did not work. Any suggestions to solve the issue?

SandeepMedikonda posted this 21 August 2018

Hi Jack,

  I am unable to look into your model but can you provide some more details on how you are setting up your model (boundary conditions, contact etc.), snapshots will be helpful? Also, what is the exact error message you are seeing and how does your force convergence plot look?

  I haven't used CZM recently, but I did use it in explicit a while back. Hopefully, I can help.

P.S: In the future please post as a new discussion and link it to your old post if needed. This way your post is likely to get more attention, long threads often tend to get less attention.

Regards,
Sandeep

peteroznewman posted this 21 August 2018

Hi Jack,

Disclaimer: I have never used CZM before.

I downloaded your model and made a few tweaks to get it to converge on some early substeps.

First, I changed the scope of your displacement from edge to face. For solid models, it is always best to apply BCs to a face, not an edge or vertex.  I also cut the displacement by half to 0.4 mm.

Second, I added the command snippet neqit,50 to make sure more iterations were tried than the default 26.

Third, I changed the Auto Time Stepping to have 200 initial and minimum substeps.

Fourth, I requested 3 Newton-Raphson Residuals under Solution Information. Those plots are helpful so see where the convergence is failing.

Here is the Force Convergence Plot for the first 100 iterations

I will report on the point at which it stopped converging in the next post.

Regards,
Peter

 

  • Liked by
  • jackhero
peteroznewman posted this 21 August 2018

Here is where it stopped.

Here is the Netwon-Raphson Residual Plot.  It told me that the Maximum occurred on the Rod, so I am only displaying that below.

The corrective action to make the solution progress further is to use smaller elements on the Rod.

Regards,

Peter

 

  • Liked by
  • jackhero
  • SandeepMedikonda
jackhero posted this 22 August 2018

 @Sandeep

Thank you for your reply.

The convergence issue seems like has been solved by @Peter in his reply. However, your experience in CZM could help me in the modelling of interface behavior. Please note that the following description (loads, boundary conditions etc) are for the model before the modification/correction by Peter

I am trying to model pullout behavior (load displacement curve) of rod with concrete. Initially the rod is bonded with the concrete (embedded 1mm) and after some displacement (if the load doesn't exceeds rod strength limit) the bond is broken and then the frictional behavior starts which leads to either slip-hardening or rod rupture (if frictional stresses exceeds the load bearing limit of the rod) or slip-softening behavior. The boundary conditions are shown in the attached image (bottom of the concrete is fixed while displacement is applied on the free end of the rod).

The bonded contact I have modeled is shown in here,

The issues with CZM I have mentioned in my previous post are shown in the following images. My model is able to accept the CZM fracture and CZM separation but not the CZM Bilinear and CZM Exponential. Could you provide any suggestion regarding this issue?

CZM Error

jackhero posted this 22 August 2018

@Peter,

Thank you for your reply.

I will follow your guidelines to make changes in my model and get back to you if there is any problem.


Since you have mentioned that you have cut the displacement by half to 0.4mm. Would it effect the convergence, in your opinion, if I change the displacement to any other value between 0.4 and 1.0mm? Since the rod is embedded upto 1mm in the concrete therefore the displacement might need to be changed to see the effects later on the interface.

peteroznewman posted this 22 August 2018

Jack,

You can add Step 2, to add more displacement without affecting the convergence of Step 1.

I also recommend reducing the size of the block by half (or more) to reduce simulation time.

Regards,

Peter

  • Liked by
  • jackhero
SandeepMedikonda posted this 22 August 2018

Jack, 

  In case, you haven't seen this video, please check it out.

  Also, see VM248 and VM255 for contact debonding.

Now, as far as setting up a bi-linear contact softening in Mechanical.

  • Change the formulation to either Augmented Lagrange or Pure penalty (only penalty based methods support the CZM) once you have inserted a Bonded contact.
  • If you wish to use bilinear CZM law, change the Update Stiffness to Never so that the contact stiffness remains the same during the simulation

Hope this helps.

Regards,

Sandeep

  • Liked by
  • jackhero
peteroznewman posted this 23 August 2018

Jack,

Have you considered running an axisymmetric 2D model of the pullout with the CZM?  That would be able to solve in a short time with a high density mesh.

Regards,

Peter

  • Liked by
  • jackhero
jackhero posted this 18 September 2018

Peter,

Thank you for your suggestion of using 2D model for the simulation. I have reduced the geometry size in 3D but still using the 2D simulation would be useful to reduce the computing cost. I have the model in 3D (archive here and geometry only here) is it possible to reduce it to 2D model without starting to make the 2D geometry in the design modeler from zero? I searched for the possibilities and tried using the Surface from sketches but it did not work in my case as I have two different sketches (one for rod and another for block). I must be missing something to convert to the 2D model.

peteroznewman posted this 18 September 2018

Jack,

Looking at your 3D geometry, the rod is along the global Z axis, which is inconsistent with the needs for an axisymmetric model, where you must put the rod centerline along the Y axis and draw only the +X radial slice. Since it is fairly simple geometry, you should just start from zero.

For complex 3D geometry, I have done the following in a CAD system: 1) Slice the solids about two planes to get a quarter model. 2) Extract faces on one of the slice planes. 3) Transform those faces to the XY plane putting the centerline along the Y axis.

Regards,
Peter

jackhero posted this 5 weeks ago

Peter,

I tried the 2D geometry for the said simulation (attached here). Processing time much quicker than the 3D. Thank you for your suggestion on using 2D.

I had convergence problems i tried solving it by reducing the time step to 0.0001 seconds (attached Solution information.txt). I tried following your method of locating convergence issues as mentioned in your post here. The residual newton raphson force, (images attached) showed the maximum near the contact point of the rod and concrete. I tried modifying the contact mesh (image attached below) with more reduced time step (0.00001 sec) but still had the same convergence problem (attached Solution information 2.txt).

Could you please suggest on solving the issue? Shall i try it with more reduced time step or my model have other problems.

 

 

 

peteroznewman posted this 5 weeks ago

 Jack,

You have not created the Axisymmetric model you want. It should be a radial slice that is revolved around the Y-axis to create the solid body.

What you have drawn is this:

When I rotate that around the Y axis, this is the model that you are simulating in ANSYS.

I said that the axis of the rod goes on the Y-axis. You haven't done that.

You have applied the displacement to the entire rod body when you picked the face of the rod. That does not allow the rod to stretch. You need to apply the displacement to the top edge of the rod. Also, put in a much smaller displacement.

I recommend you make the elements on the rod the same size as the elements on the concrete.

Regards,

Peter

  • Liked by
  • jackhero
jackhero posted this 5 weeks ago

Peter,

I suppose by axisymmetry you mean to draw like the image shown below. Could you please confirm this is what you meant?

 

If I put the axis of the rod on y-axis I ended up like shown in the image. I drew the half of the design on the axis and other half was done by revolving  .

 

peteroznewman posted this 5 weeks ago

Yes Jack, that is kind of how you draw the geometry for an Axisymmetric structural model. But you show the concrete radial slice as a rectangle. You want a rectangle with a cutout in it as shown below to create a hole for the rod.  The rod is just a rectangle that you Add Frozen to have as a separate body.

 

  • Liked by
  • jackhero
jackhero posted this 4 weeks ago

@ Peter

Still having some probelms in running the simulation (attached here). I can't solve the convergence problem and all of the convergence failure occured at the contact point. I tried modifying the mesh near the edges but it didn't work out. Also tried using smaller mesh size (0.01) but it took long time to solve and sometimes had the memory issue for my pc with this mesh element size.



If I apply the fixed support at the bottom edge I get the distorted elements and convergence error (shown in image below). In experimental work I fixed the bottom side. I also tried fixing the body instead of the bottom edge which resulted in convergence error (as shown in the residual image above).


I tried increasing the load steps to 200 but it took long time to process with the mesh size of 0.01 and load on the pc was too high. Surely I am missing something, would be helpful if you may guide me.

jackhero posted this 4 weeks ago

I tried some suggested ways for solving the convergence problems and I am sharing the results here.

In ansys help i read Artificial damping may help to solve or reduce the converegence problem. Initially I tried with artificial damping = 0 s and I got the force convergence as follows,

 

I modified the artificial damping value from 0 to 6e-6. The force-convergence progress little further than the previous result. But later again had problem for convergence.

 

I modified the contact stiffness from default value (=1) of normal contact stiffness to 0.5.

 

Re-modifying the contact stiffness to even lower value resulted as follows,

Most of the residual errors were at or near the contact region. I modified the mesh size increased the body mesh density 1e-2. This took long time to process and at the end I had the following result.

At the end again had the convergence problem but the solution information (attached) also said about the pc memory issue. I have ran out of options here to solve this problem. I tried different possible ways which I found in the community but still cant figure out how to solve it completely.  It would be helpful if you may guide me on the mistakes or if have time you make take a look at the model.

 

Attached Files

peteroznewman posted this 4 weeks ago

Jack,

MEMORY
Your computer has only 4 GB of RAM and the solver can't reserve a large enough block of free memory to solve this model entirely within RAM. When this happens (and with a smaller mesh it will not happen), the solver switches to a different branch of code that uses the HDD to hold some of the solution while it works on solving. Since a HDD (or even a SSD) is orders of magnitude slower to access data than RAM, the total waiting time for the job to run is longer. In the example output file above, it took 7955 seconds, when it might have taken closer to 3062 seconds if you had more RAM.

It's likely the motherboard on your computer is able to address more RAM, you have to check the specifications. If so, purchasing 8 GB of RAM and replacing the 4 GB of RAM will get this model to solve in less time. Note that memory cards come in many different types and you have to get the exact right type when you purchase 8 GB. Again, check the specifications.

CONVERGENCE
Your model has a displacement of 0.2 mm.  I'll bet there is nothing special about that number, it was just pulled out of the air (or somewhere else ) and you probably have no idea when interesting results will show up. What if all the interesting results show up after a displacement of 0.05 mm has occurred? Well that would be Time value of 0.25 s.  You have results going past that point, yet you haven't shown us any results. Why do you need the model to converge all the way to 1 s and have the rod end reach the 0.2 mm value?  It was an arbitrary number to begin with.

I set the Minimum Substeps to 200 to prevent the solver taking big steps. Also, I cut the displacement down to 0.05 mm so the solution will converge to 1 s.  It is nicer when it finishes that way, so you don't have to deal with that last unconverged increment in the results. I made those two changes to the model I downloaded from your link above and it converged all the way to 1 s in 860 increments. That took 3.5 hours on a 12 core computer with plenty of RAM.  It will also take 860 increments on your computer, it will just take a lot longer.

The early stages of debonding are shown in these results shown at True Scale, but the debonding is not complete.

Make sure you set your Retain Files After Full Solve to Yes under Analysis Settings in the Restart Controls section.

That way, when the solution finishes with 0.05 mm of displacement and you want to take the solution to 0.1 mm, you don't have to wait 3.5 hours to wait for solving up the the half way point. It can just restart from where you finished, but only if you made the above setting before you hit Solve.

Hope this helps.

Kind regards,

Peter

  • Liked by
  • SandeepMedikonda
  • jackhero
Close