July 10, 2019 at 9:59 amSportyDawbsSubscriber
A CATRA test is a standard set for assessing the sharpness of knives and spikes. It involves penetrating a silicone sample with a knife/spike by 3mm at 0.1mm/s and recording the force required to do this.
I'm trying to simulate a coned spike penetrating a silicone cube sample in the same way as this standard. The issue I am having is that the CATRA test takes 30s, which for the explicit dynamics solver seems to be impossible, giving estimated computation times of '****s'.
I have tried reducing comp time using 2D geometry, simple mesh, increasing energy errors and time step safety factors but cant seem to get anywhere near running the simulation to capture 30s of data.
Does anybody please have any advice on how to run long duration transient simulations that could help me with this project?
July 10, 2019 at 12:31 pmpeteroznewmanSubscriber
I imagine you need some small elements to capture a spike penetrating silicone. That forces the Explicit Dynamics solver to use smaller time steps. If you double the element size, you double the time step. Read this post (and the included link).
Moving at 0.1 mm/s is a quasi-static speed. You could switch to a Static Structural analysis that uses an implicit solution that does not scale with element size.
What material model do you have for silicone?
What failure mechanism do you have for silicone?
July 10, 2019 at 3:34 pmSportyDawbsSubscriber
Thank you for replying so fast!
Using very small elements! That makes sense. Looking at that link you have sent, could comp time be improved by scaling up the geometry and therefore, the mesh with it (I've done element sizes based on number of divisions)?
I have tried a static structural simulation but get zero deformation in the Silicone as shown in the attached image. For this reason I didn't think it could do a penetration and had to use transient?
Currently I am using explicit rubber 2 material from engineering data with Emod = 0.3mpa and Poisson's = 0.499 because I do not yet have silicone sample to measure.
No failure mechanism set, i'm interested in the peak force at 3mm penetration.
July 10, 2019 at 3:35 pm
July 10, 2019 at 6:29 pmpeteroznewmanSubscriber
The simpler method to speed up the simulation is to increase density, which has the same effect as increasing the geometric scale, but is easier to implement.
Explicit Dynamics has the benefit of automatically eroding elements that have exceeded a strain threshold of 1.5 but that may not be appropriate for silicone which might well support strains > 3. Static Structural can also remove elements that have failed using ekill command but it is far less automated. See this tutorial.
July 11, 2019 at 9:37 amSportyDawbsSubscriber
Would increasing the density not hugely affect the reaction force results?
July 11, 2019 at 12:05 pmpeteroznewmanSubscriber
Yes, as would increasing the size of the geometry.
Here is the text that I linked to in the first sentence above.
There is an equation Explicit Dynamics uses to calculate the maximum stable time step. It is a function of length and the speed of sound in the material. The speed of sound is a function of density. When you want to reduce the waiting time for the Explicit Dynamics solver to show something, it is much easier to increase the density by 100 or 1000 times than change the geometry. To answer your question, the larger geometry will take less time to solve, but read my last paragraph.
I highlight the word something, because when you do this, you are not solving the original problem anymore, you have changed the physics by making the material so dense.
Sometimes I want a "cartoon" animation to show roughly what the end result might look like. I am happy to have a fast solve time so I can check that I have things properly built in the model. Sometimes that cartoon animation is sufficient to show someone the motions, even though they might deviate from the true solution, and I don't need to wait for the true solution.
If I need to calculate engineering quantities from the solution, then I have to return the density to its original value and wait the required time.
Note that you can minimize your wait time and have accurate physics by carefully meshing the part to avoid a few small elements. There is a mesh metric called Characteristic Length that will highlight the few smallest elements that are dictating the maximum time step. Edit the geometry or the mesh controls in double the size of the smallest element and you will have cut the wait time in half.
July 11, 2019 at 1:05 pmSportyDawbsSubscriber
It makes a lot more sense now, a lot of things there that I never knew about explicit dynamics! Thanks for your help with this, I will try the density change and see what differences it makes to my results.
- You must be logged in to reply to this topic.
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.
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- 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.
- Colors and Mesh Display
- User manual
- material damping and modal analysis
© 2023 Copyright ANSYS, Inc. All rights reserved.