June 28, 2018 at 5:41 pmFernando TorresSubscriber
Hi , I have to determine the maximum height from which the glass should be thrown (under gravity only) so that it does not break.
I have 3d CAD model of glass. How to setup and perform this analysis. Accurate results are required as I'm going to check it practically.
How to setup material properties for glass and floor ?
How to set up model ( step time ,end time etc )
June 28, 2018 at 7:30 pmSandeep MedikondaAnsys Employee
I would recommend doing this as an Explicit analysis with either ANSYS LS-DYNA or Explicit Dynamics where you can set up some erosion criteria.
If you use this, you can start with a rigid ground and simple material properties with erosion criteria based on strain. You could also use the drop-test ACT extension available to do this.
Contact and damping might be important here. Time step is automatically accounted for to satisfy the CFL condition, for total time use around 0.1sec (so like a quasi-static analysis), don't forget to include dynamic relaxation while using gravity.
June 29, 2018 at 12:05 ampeteroznewmanSubscriber
Experimentally, how will you determine the probability of breakage as a function of drop height?
Let's say you have 100 samples to drop and you group them into 10 sets of 10.
There will be some height where all 10 survive and some height were all 10 break, then between those values, you will get some number of samples, b, breaking and 10 - b samples surviving. It won't be a monotonic change because each sample will have different flaws and edge cracks that will make it break early or late compared with another sample.
You could plot out the results from dropping 10 sets of 10 samples and it might looks something like this:
What is the drop height your experiment determined that you would compare with your simulation result?
June 29, 2018 at 2:47 amFernando TorresSubscriber
Hi Sir Peter !
Actually I am having a single glass CAD model. I'll change the drop heights in simulation i.e.
simulation1: drop height = 20 inches
simulation2: drop height = 40 inches and so on.
Lets say it breaks at 120 inches.
Then practially means, to verify the results, I'll drop some of those glasses from heights < 120 inches in order to be in safe domain while droping a glass.
June 29, 2018 at 5:02 ampeteroznewmanSubscriber
Forget about the simulation. You said, "I'm going to check it practically." That is what I am talking about.
Say the simulation predicts it breaks at 120 inches and doesn't break at 110 inches.
For your practical test, you physically drop a real part at 100 inches and it breaks. What do you do next?
Let's say you practically drop the next sample at 80 inches and it also breaks.
Let's say you practically drop the next sample at 60 inches and 40 inches and they also break.
Finally you get down to 20 inches and you get a glass that doesn't break.
Do you say that the glass breaks between 20 and 40 inches?
No, because you drop another sample at 40 inches and it doesn't break then you drop another sample at 20 inches and it does break.
What do you say is the height at which the glass will break in a practical test?
The point is that there is a range of heights with varying probabilities of breakage.
The plot I showed is one way to quantify the probability of breakage as a function of drop height in a practical test.
June 30, 2018 at 12:43 amBhargava SistaAnsys Employee
Check out Johnson-Holmquist model in explicit dynamics, it is a brittle material model for glass and similar materials. Getting the material properties for it might be tricky, I'd suggest searching the literature.
Regarding the physics of your problem, there are microscopic defects in the glass that are randomly distributed which contribute to the failure. But you're not accounting for them (unless you use a specific material model such as stochastic failure model) in your model so the simulation is idealized. So, the theoretical minimum height at which you see the glass cracking in your model will be an overestimate of what you may see in reality. As peteroznewman suggested, you'll need to approach this problem in a stochastic sense rather than deterministic sense. If you're a graduate level student who is brave enough to geek it out, look up uncertainty quantification.
In a practical sense, I'd recommend you to start with a simple linear elastic material model with a max. principal strain based element erosion criteria. This just gives you a brittle fracture simulation. To get physically reasonable results, you'll need realistic material properties and failure criteria. Search for "windshield failure analysis" and you'll come across many papers that are open to the public. You'll find some specific material models and may also find the relevant material properties.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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.
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- What is the difference between bonded contact region and fixed joint
- Massive amount of memory (RAM) required for solve
© 2022 Copyright ANSYS, Inc. All rights reserved.