March 2, 2022 at 11:06 pmfrancescocurzioSubscriber
Hi everyone! Im simulating a battery cell and i have modelled the inner part of the battery as an homogeneous mean. The simulation seems to go smooth, but i have only a problem. Near the end of the simulation the jellyroll (green) penetrates the shellcasing (red). Furthermore, the elements are characaterized by an huge distortion as you can see in the picture. How can i resolve these issues and what can be the error? I have modelled the contact between the parts using the CONTACT_AUTOMATIC_SURFACE_TO_SURFACE with the option SOFT=2 because the jellyroll is modelled with a soft material model (mat model 63 with ADD_EROSION). Adding the erosion also to the shellcasing made in steel can improve the simulation and resolve the problem? Another question is related the CONTACT_AUTOMATIC_SURFACE_TO_SURFACE: in the model i have to relate with this keyword only the parts actually in contact (e.g. shellcasing's surface and outer surface of jellyroll in the picture) or i have to relate all parts of the model (e.g. shell casing related with outer surface of jellyroll, with inner surface of jellyroll and with the outer surface of the grey part in the pic)?March 17, 2022 at 4:34 pmtslavikAnsys EmployeePlease tell us which release of LS-DYNA is used (e.g., R10.1.0, R11.2.2, R12.1.0, etc.) and whether it's SMP or MPP.
It appears the model comprises three parts, which use *SECTION_SOLID for the green foam part, and *SECTION_SHELL for the ground plane and red casing. Correct? Or, perhaps the ground is represented with a rigidwall? The thickness of the shell parts should be taken into consideration when building the mesh; it is important for good contact behavior, although it's possible to work around this. For example, the nodes of the red shell should be positioned away from the outermost nodes of the green part by one-half the shell thickness. Similarly, a gap should exist between the red case and ground plane shells - the gap dimension would be equal to the sum of the half-thicknesses of those shell parts.
Please let us know if the initial geometry of the parts take into consideration the shell thicknesses, as described above.
The response of the green foam part seems strange. What ELFORM is used in *SECTION_SOLID? Is there a "hole" in its center, or do the elements extend to the axis?
Let's focus on developing a robust baseline for the *MAT_063 definition. For simplicity, use MODEL=0. The stress-strain curve, LCID, should look similar to Figure M63-1 in the manual and assure the first point is (0,0). Set the elastic modulus, E, equal to the slope of the last segment in LCID. Set PR=0.3. Set TSC to a positive value similar in magnitude to the peak expected compressive stress.
Eliminate erosion for the time being; it can be added later. Do not use *MAT_ADD_EROSION and assure ERODE=0 in *CONTROL_TIMESTEP. Special contact treatment is required (*CONTACT_ERODING ) when solid elements erode.
How many *CONTACT definitions are used. Describe them, please. SOFT=2 is recommended in the *CONTACT definitions. Use SBOPT=3 and DEPTH=35.
Let us know the results of this test run.
March 18, 2022 at 6:55 pmfrancescocurzioSubscriberHi sir. thank you for the reply! The model in the picture luckily worked well and i was able to find the issue! However ill explain you what is in the model: there three parts, all modelled with solid elements:
CenterPin in grey (width 0.16 mm) using simplified JC mat model
JellyRoll using foam material model
ShellCasing in red (width 0.26 mm) using simplified JC mat model
Then there are a ground (modelled with shell elements) and an indenter (modelled with solid elements), both use rigidi material model.
However the issue was the formulation of the contact: i used a penalty formulation instead of a pinball segment based contact (SOFT = 2)! Then all went smooth; however this model was built up only on my purpose, in order to get familiar with LS-DYNA (this is the first time i use this software). The goal of my research is the detailed model of a battery cell, so it needs to contain all the components such as separators, electrodes ecc.
Thank you for your exhaustive answer, i appreciate it a lot
Viewing 2 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
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.Trending discussions
- ANSYS Workbench Measuring within Design
- how to improve the inflation quality at sharp corners?
- check element type
- The mesh file exporter could not resolve cyclic dependencies in overlapping contact regions error
- How to resolve Mesh Failure
- Meshing Error
- Error in meshing
- Conformal vs Non-Conformal Mesh
- execution error inside the mesher. The process suffered an unhandled exception or ran out of memory
- inflation created stairstep mesh at some location
Top Rated Tags
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.