June 28, 2023 at 10:20 amCarles DomenechSubscriber
Hello, first post here, hope I'm not breaking any rule.
I've tried to use the new geometry-based adaptivity feature, but it seems i does nothing.
I'm running a Static Structural analysis with a simple solid part, one force, and a fixed support.
I haven't specified any mesh settings (thus it's quite coarse).
After running the simulation, the mesh doesn't change, it's still coarse and quite bad. The simulation time is not split into substeps (with different meshes).
What am I doing wrong? Also, what's the energy coefficient?
June 29, 2023 at 3:46 pmmjmiddleAnsys Employee
The adaptvivity doesn't do anything when:
- The time occurence criteria is not met, such as determined by the equally spaced points value.
- The adpativity criterion is not met, such as the energy coefficient you have specified
Check the solution information. If there is no section where it checks the energy criterion, reporting the model's value and the user-specified value, then if wasn't triggered by the time occurence criterion. If it did meet the time occurence, but your model has criterion above the threshold set, then it won't do anything. It seems that you think the adpative region should determine the time of substeps by your sentence: "The simulation time is not split into substeps (with different meshes)." But it does not do this. Your model looks linear, and the documentation for it states the large deflection must be off. So if you have not specified multiple substeps, or an time steps less that the end time in the Analysis Settings, it's going to do only one substep and this will be at the endtime (probably at 1 sec). So the geometry based adaptivity will only check once at the end of the analysis.
The nonlinear adaptive region is similar, so you'll probably want to look at that documentation also:
Here as my writeup of the time checking:
Values for "Check At":
1. "Equally Spaced Points"
Divides time range by the "Value"
"Time Range" is either:
1. "Entire Load Step"
It takes the time range of the entire load step and divides by the "Value" for the "Check At" and checks at time increments of this time. Example:
Load step is 0-1sec
"Value" is 5
1/5=0.2sec, so it checks every 0.2 sec: 0.2, 0.4, 0.6, 0.8, 1.0sec.
Specifies the time range in which to divide the number of "Value."
So for a load step 0-1sec, you set range 0.75-1sec, and with Value of 5, it does:
0.25/5=0.05sec, so it checks every 0.05sec after 0.75sec: 0.75, 0.8, 0.85, 0.9, 0.95, 1.0sec
2. "Specified Recurrence Rate"
Checks every time the number of substeps done increases by the "Value"
"Time Range" is either:
1. "Entire Load Step"
Checks wihin the entire load step, every n substeps, where n="Value"
Checks withing the specified time range every n substeps, where n="Value".
I usually use the mesh criterion for a nonlinear adaptive region, but the geometry based adaptivity doesn't allow that criterion (onlt energy and box). For understanding the energy criterion, the documentation page has some links to the APDL documentation for the section on nonlinear mesh adaptivity as well as the command NLADAPTIVE,,,ENERGY:
2.5.1. Energy-Based Criterion
This criterion is defined for current-technology structural 2D and 3D solid elements. It is based on the magnitude of strain energy of the element compared to the mean strain energy of components to which the element belongs. During the substep at which nonlinear mesh adaptivity criteria are checked, if the element’s strain energy is greater than or equal to the mean strain energy of its components times the user-defined
VAL1(NLADAPTIVE,,ADD), the element is either refined via general remeshing or it is split (NLMESH,REFA,SPLIT), depending on the element types.
This criterion is used to refine the mesh to achieve high-accuracy simulation in regions where a high concentration of stress exists and elements are too large. It can also be used to refine the mesh at certain intervals of substeps if a very small value or 0 is input for
June 30, 2023 at 9:17 amCarles DomenechSubscriber
I've split the simulation into 4 substeps and now it seems to work as expected. I did believe the Geometry Based Adaptivity object would do the split for me.
- 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.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- User manual
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- Defining rigid body and contact
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.