January 23, 2018 at 7:33 pmOsamashakilSubscriber
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.
January 23, 2018 at 9:59 pmpeteroznewmanSubscriber
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.
January 23, 2018 at 10:42 pmOsamashakilSubscriber
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".
January 23, 2018 at 11:38 pmpeteroznewmanSubscriber
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.
January 24, 2018 at 10:27 pmOsamashakilSubscriber
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?
January 24, 2018 at 11:12 pmpeteroznewmanSubscriber
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.
January 25, 2018 at 12:05 am
January 25, 2018 at 1:28 ampeteroznewmanSubscriber
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.
January 25, 2018 at 1:47 am
January 25, 2018 at 1:54 amOsamashakilSubscriber
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?
January 25, 2018 at 2:09 ampeteroznewmanSubscriber
Right, Menetrey-Willam was added in 18.2. I don't know how you can use that in 18.1.
March 26, 2018 at 9:20 pmOsamashakilSubscriber
Hi Mr. peter,
Please tell me your full name and designation.
I want to add your name in acknowledgment of my project work.
March 26, 2018 at 9:36 pmpeteroznewmanSubscriber
Thank you, I learned a lot on your project.
ANSYS Student Community Moderator
- The topic ‘Bar Pull-out analysis in Ansys Explicit Dynamics results issue’ is closed to new replies.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- Maximum Time Step
- Error 20211 (STR+211) while 2D impact analysis
- ls dyna has no solver
- LS-Dyna Prestressed
- Whereabouts of the LS-DYNA program manager
- License error : NO SUITABLE FEATURE FOUND
- Total Contact Force and Contact Pressure
- Contact not working in Ls-Dyna and Ls-Dyna ACT (WB)
- Element direction..
- TIED_CONTACT for Shell Elements – Gap between Shell-Shell and Shell-Solid
© 2023 Copyright ANSYS, Inc. All rights reserved.