Bar Pull-out analysis in Ansys Explicit Dynamics results issue

  • Last Post 26 March 2018
  • Topic Is Solved
Osamashakil posted this 23 January 2018

Hi Mr.  peteroznewman,


I have done Explicit dynamic Analysis as guided by you :

But result (Force vs time) curve I m getting is very strange (picture attached).

A professor told me to use another concrete matrial model, but I m not sure if the issue is with material only or with other things. 

I will be very thankful if you take a look at the attached model.

Attached Files

Order By: Standard | Newest | Votes
peteroznewman posted this 23 January 2018

I can say without looking at your model that this is typical for an Explicit Dynamics model.  Look at the time scale, there are 5 oscillations in 1 ms. That's a frequency of 5 kHz.  Do you know what is the speed of sound in steel?  It's about 6,000 m/s.  How long is your steel bar?  If it is 0.6 m long, then it takes about 0.0001 seconds for a pressure wave to travel from one end of the steel bar to the other, where it gets reflected and travels back. Round trip time, 0.0002 seconds, or a frequency of 5 kHz.

You have to take way longer than 1 ms to pull the bar 4 mm in order to let the 5 kHz oscillations die out. Unfortunately, if you take 1 second to pull the bar 4 mm, the simulation time will be 1000 times longer. That is just the way it is in an Explicit Dynamics model.

Osamashakil posted this 23 January 2018


my bar is 0.25 m long and I need displacement of 4 mm ( or maybe 3 mm) is there any way to calculate END TIME will be suitable for Analysis? However, in actual bar pull-out experiment displacement of 0.01 mm per sec is applied.

Moreover, there is "initial, min, max" time, which is programmed control, can I adjust it by myself to make substeps smaller? because every time I change it the error appears "time step too small".

peteroznewman posted this 23 January 2018

So if you did a "real time" simulation, you would take 400 seconds to move 4 mm. You can probably speed that up 400 times to 1 second.

The Explicit Dynamics solver calculates what the minimum time step must be for a stable solution. It's best to leave time steps Program Controlled.

Remember my 2D example?  There were about 5 elements along the side of the rib on the rebar.

You're going to need at least 5 elements along the side of rib on the rebar to have a fine enough detail to see the gradual failure of the concrete. Your current mesh has 1 element along the side of the rib on the rebar.

Unfortunately, in Explicit Dynamics, the minimum stable time step is a function of element size. The smaller the element, the smaller the time step, so multiply by at least a factor of 5 the time to solve for the reduced element size, not to mention all the extra elements that will be created. The simulation could take days to solve to a 1 second end time.  That's the way Explicit Dynamics works.

Osamashakil posted this 24 January 2018

I have reduced time to 0.01 and result is getting better. Thank you, and for meshing, actually there is one element outside, but if you cut the section and see inside, the meshing is much finer.

Now I have one more question, I m using "Non-Linear concrete" in it as you told me. But my prof. asked me to use "Menetrey-William-Model" instead of drucker-prager , if I look at Engineering data of Explicit Dynamics, I cannot find this concrete material model. Can you guide me that how can I use this model material parameters in ansys?

peteroznewman posted this 24 January 2018

Do you mean you have increased the end time from 0.001 to 0.01 seconds?

Here is a section through the "much finer" mesh on the small solid around the rebar that I found in the attachment to your first post.
There is only 1 element of concrete along the side of the ridge on the rebar.

So when you make the elements 5 times smaller, you will have to wait 10 times longer for the solution to reach 0.01 seconds. A factor of 5 for the smaller elements and a factor of 2 for the increase in the number of elements (it's good you are not on the Student license).

ANSYS supports the Menetrey-Willam model.  Type Material Reference into the ANSYS Help Viewer.
It's easy to get data for rows 11 and 12.  Not so easy to get data for rows 13 and 14. Ask your Prof.


Osamashakil posted this 25 January 2018

Thank you for detailed answer regarding meshing.

For material model, I got attached coding in help menu, but I m sorry as i m not expert in Ansys, do I need to copy the commands in workbench Engineering

data? and can u tell me where to copy?

peteroznewman posted this 25 January 2018

Open Engineering Data, and create a new material. Add a Density from Physical Properties, add Isotropic Elasticity from Linear Elastic, and add Menetrey-Willam from Geomechanical.

Fill out the required values.

The code example has a Young's modulus of 20E6 Pa, but Concrete NL has 30E6 Pa. Which value will you use?

Here is that form with the values from the code sample filled out.

The code example includes linear hardening and softening, which is optional.
I don't know how to add that to the material model using Engineering Data.

Osamashakil posted this 25 January 2018

I have the values, so I do not need to use to code values,

but the issues is that GEOMECHANICAL on left side, does not contain Menetrey-Willam


Osamashakil posted this 25 January 2018

I think its because of the reason that I m using Ansys 18.1, so is there no way to include Menetrey-Willam in 18.1?

peteroznewman posted this 25 January 2018

Right, Menetrey-Willam was added in 18.2.  I don't know how you can use that in 18.1.

Osamashakil posted this 26 March 2018

Hi Mr. peter,

Please tell me your full name and designation.

I want to add your name in acknowledgment of my project work.

peteroznewman posted this 26 March 2018

Hi Osama,

Thank you, I learned a lot on your project.

Peter Newman

ANSYS Student Community Moderator