how to make the concrete smash or fall apart from the body

  • Last Post 17 January 2018
  • Topic Is Solved
zhizhuo posted this 20 December 2017

I mean when you finish your model and put it in workbench,and then set up material  boundaries and so on, what I need is to simulate the destruction of concrete. It should be smashed with time goes on. But the  result is  amazing。I can not explain why and don't  know how to handle it. I do set up erosion,while it doesn't make any work.


the left picture is what I want,whlie my simulation is like the right

you can know it from the video

By the way ,is anyboby know about how to use LS-DYNA in workbench

Thanks in advance!

Whatever  advice is appreciated.



Order By: Standard | Newest | Votes
peteroznewman posted this 20 December 2017

I used Explicit Dynamics to simulate an aluminum plate with a hole in it being pulled by a steel pin. I wanted to see erosion (element failure) as the element exceeded a principal strain limit. See the video in this post. I made the velocity of the pin be a function of time so that the load could build up gradually. The first attempt had an initial and constant velocity on the pin, but the shock from that caused the whole body to disintegrate. Perhaps a velocity ramp would help you.

In your other discussion, you ask about how to reduce the time an Explicit Dynamics model will take to run. The maximum time step is calculated from the minimum element size and the material speed of sound. See slide 7 on this presentation.  The best thing is to have large uniform element size. If some small elements are unavoidable, you can use mass scaling, where AUTODYN will automatically identify the small elements and increase their density to change the speed of sound and give larger time steps. Mass scaling is automatically switched on when the Quasi Static or Low Velocity analysis types are chosen. You get to choose your own maximum stable time step and it will calculate the required density, but you don't want ridiculously dense elements, so you can set a limit on how large of a change in density is allowed.



zhizhuo posted this 21 December 2017

You are really a nice person! Thanks a lot for all your attention.The velocity should be constant,and it will abey my assumption if  a velocity ramp is set up to the model.I use  Explicit Dynamics to simulate concrete in quasi-statistic situation.I do want to see erosion (element failure) as the element exceeded a principal strain limit. So I set up erosion option in AUTODYN. It does't work well.

So i guess the best way is to choose SPH solver .But there is a a hard nut to crack -how to put the stl format file into AUTODYN.I have tried may ways.It is difficult to convert the stl to any format which can be accessbile to AUTODYN,such as .gon .Ok,maybe I should turn to a ICEM.

About the mass scaling,I know it is helpful to reduce the computation time.While I can't find the option in AUTODYN.My Operation interface like this

I guess that mass scaling cannot be used in 2D palar



peteroznewman posted this 22 December 2017

 You can show your appreciation by clicking "Like" on the posts that are helpful.

The geometric strain you show for erosion is 1.5 or 150%.
Did you mean to have failure at 1.5% strain? If so you have to type 0.015 in the field for strain.

Mass scaling can be used in a 2D axisymmetric model, so I assume it should also in 2D planar.
Here is a message from the solver when I requested too large of a time step...

Initializing.....Please wait
Mass scaling limit exceeded for Part SurfaceBody, fraction of added mass = 1.0899E+01
Mass scaling limit exceeded
Finished model setup with errors... 

However, when I tried to use mass scaling in a that 2D model, I didn't see an increase in the time inc over a run without mass scaling.

I see you are using the AUTODYN interface, while I am using the Workbench Explicit Dynamics interface to the AUTODYN solver.

This is the input form that enables mass scaling

If you use the Workbench Explicit Dynamics interface to the AUTODYN solver, getting the geometry is very easy.
I described how to do that in this post.

I am interested to know more about your model. What is the true length of the lattice? Which concrete is the lattice made of? Please tell me more about how the structure is loaded. Does one end have an applied velocity and the opposite end a fixed support?

peteroznewman posted this 24 December 2017

Erosion is working well in this 2D model.

zhizhuo posted this 25 December 2017

Merry Christmas!

Thanks for all.I have got same resoult just as the video you unload,which I thick there is something wrong.I hope it does not annoy you if you are so kind to take down the video from the youtube.I think it is not corrcet or It is not what  i want.So I don't want to mislead others.

There are always too many problems.and hope more ways out .



peteroznewman posted this 25 December 2017

I took down the YouTube video as requested, and replaced it with an image of the last frame instead. You said in the first post that erosion wasn't working, and I wanted to show you that it was working, especially when velocity ramps up instead of being applied as a constant. I don't understand how the video might mislead others.

Failure along a plane 45 degrees from the direction of compressive load is what I would expect from a solid brittle material. Why do you think that it is not correct?

You say the failure shown in my model is not what you want to see, please describe the type of failure you want to see. Are you going to change the shape of the lattice? In your first post, you show failure of steel reinforced concrete as the desired outcome.  I used your lattice geometry and plain concrete with no reinforcement. Are you planning to add reinforcement?

zhizhuo posted this 26 December 2017

Thank you  for your attention.I didn't notice the failure along a plane 45 degrees from the direction of compressive load.So you choose a velocity depent on time.Isn't it?You have a better skill of ANSYS and provide me a new direction for me .Thanks again.

Whill what I want  to see  is the model smashes  into part,like real concrete.I saw someone do it 

Maybe my idea is wrong.Is it convenient to leave your email .I think it will more  efficient .to discuss with you



zhizhuo posted this 26 December 2017

OK.I want to ask more about your analysis setting.I see you set low velocity as analysis setting type .while I set custom instead.

These days ,I came across the  problem which drive me crazy.

and a message say : A general failure occurred during the solution process.

Have you ever met it before ,and how do you concer it


peteroznewman posted this 26 December 2017

All the Low Velocity setting in Mechanical does is to enable many other fields for editing, such as: Automatic Mass Scaling, Minimum CFL Time Step, Maximum Element Scaling and Maximum Part Scaling.

I applied a velocity on the right edge to have an X component of -1000*time and I simulated 0.1 seconds so that edge reached a displacement of 10 mm, but started with zero velocity. It needed a million time steps to get to 0.1 seconds and took about 27 hours and ran on only 1 core since it was a 2D model.

A useful Analysis Setting to change is the Maximum Energy Error. I set it to 100 to get this simulation to run.

 The attached file is an ANSYS 18.2 archive of the Explicit Dynamics model that I took the image above from. Since I didn't know the true size of your model, I scaled it to be 100 times larger than it imported from the STL to reduce the solution time (larger elements = larger time increment).


Attached Files

zhizhuo posted this 27 December 2017

Have you ever met this problem: a general failure during the solution process.

I guess  the model is OK,and the material and boundaries are correct. while when I click solve ,the error pups up. It make me screwed up




peteroznewman posted this 27 December 2017

Yes, I have seen this error message. Unfortunately, AUTODYN does not provide very good diagnostics when the model does not run. I have only built a few Explicit Dynamics models myself and am still learning how to diagnose problems. If you clear the mesh and attach the ANSYS archive to your previous post, I will take a look at it.



zhizhuo posted this 27 December 2017

Thanks again. I solved it in an inappropriate way --------just restart  your computer.  OK,  It sounds stupid.Anyway it works.In my piont ,it  is a bug with ANSYS.and   the problem happened in ANSYS workbench, when I  built a Explicit Dynamics model and run.



peteroznewman posted this 27 December 2017

There are bugs in ANSYS, but there are also bugs in Windows. One student had a computer with 6 GB of RAM and was working on a small model that failed to run, but he had been opening and closing many different programs and documents for a week. The memory got fragmented and ANSYS could not find a big enough block to run the model. A simple restart fixed the problem, which was caused by Windows not managing memory very well.

Just for fun, I am running a model of your 2D concrete lattice, fixed at both ends and a steel cylinder that impacts the side of the lattice at 1 m/s. It has 16 hours left to go to get to 0.1 seconds or 100 mm of penetration. Let me know if you want to see that and I can put it on YouTube for you to watch.



zhizhuo posted this 28 December 2017

I wonder if you simulate the uniaxial  compression test . What significant process do you get? Does the concrete fall aprt .The particle should be smashed and peel off from the part.I think it sholud be alaways joined together all the time or for the almost time. That is what I emphasize .So how about your result.?

There are more tough things I should solve not only for the software but also for the windows




peteroznewman posted this 28 December 2017

peteroznewman posted this 01 January 2018

You asked how to speed up an Explicit Dynamics simulation. I said bigger elements result in a larger time increment. I created a 15 m long, 7.2 m diameter cylinder with a slight waist to cause concrete failure at the center. Each element is 150 mm. That made the stable time increment large enough that I could create the video below in about 6 hours. Next I am going to add some steel rebar to the center.

peteroznewman posted this 02 January 2018

Explicit Dynamics simulation of concrete under a compression load caused by a velocity BC on the right face and a fixed BC on the left face. There is a circular pattern of 7 steel reinforcement bars in the concrete.

Attached Files

peteroznewman posted this 17 January 2018

Those interested in concrete failure should read this discussion.