August 7, 2023 at 7:27 amPaolo LangellaSubscriber
Good morning everyone,
I'm trying to perform a static simulation to evaluate the stress in the wires that actuate a snake robot made of rolling joints.
At the moment I am focusing on a model which is composed of a base, a link and 4 wires.
Since I am having convergence issues, I'd like to have some feedback about it.
The settings of the analysis are the following:
- Base and link bodies are rigid, while the wires are flexible.
- Frictionless contact between the wires and the link and the wires and the base. Stabilization damping factor of 0,05 and time step control predict for impact;
- Frictional contact between the base and the link with friction coefficient of 0.2;
- Fixed joints on the right between the edges of the link and the wires;
- Ground to base fixed joint to the surface of the base on the left;
- Analysis settings
- Two wires are pulled while the other two have a fixed support constraint;
- Remote force on the edge of the link;
Thanks in advance to anyone that can help me.
August 7, 2023 at 7:45 amAkshay ManiyarAnsys Employee
Convergence issues can be tricky. Can you share the error message you are getting? Also, it looks like you ran the model with a Large deflection aet to OFF. We generally recommend running the model with a large deflection option set to ON. Also, check for Newton-Raphson residuals. The Newton-Raphson Residual data (if requested) will show graphically which areas had the highest force residuals. These areas usually correlate with the phenomena that are preventing the achievement of force equilibrium (convergence).
August 7, 2023 at 7:59 amPaolo LangellaSubscriber
Thanks for your reply. I thought I selected large deflection on in both steps, but actually I noticed I didn't select it for the second step. Maybe this is the reason why I didn't get any error but after five days It still didn't converge. I'll try to run again the simulation.
If you have any other feedback it would be much appreciated.
Thank you for your time.
August 7, 2023 at 2:31 pmpeteroznewmanSubscriber
For the surfaces that are rolling on each other, I suggest changing the contact from Frictionless to Rough.
I suggest adding a blend radius on the edge of the hole in each rigid link. Add a sizing mesh control to that blend so there are several elements around the blend radius. Make sure the element size on the cable is small enough to put several elements in the size of the blend radius.
There are two cables, one on the top and one on the bottom. One cable should be attached to a spring to ground with a pretension on it. The other cable should have a displacement boundary condition to shorten or lengthen the cable to bend the snake up or down.
These three changes will make the model converge more easily.
August 9, 2023 at 6:41 amPaolo LangellaSubscriber
Thank you for your reply. I'm still having some issues with convergence but my doubt is why do I have a lot of substeps that converge but the solution doesn't? And also there is no error message.
Then, I was wondering if I could get a feedback about my model because my goal is to move to a more complex one with six links and the wires attached to the last link. I want to evaluate the force which is necessary to keep the robot straight in an orizontal position.
August 9, 2023 at 10:17 ampeteroznewmanSubscriber
The solution control logic has many convergence criteria besides the one you are plotting. For example, you can plot Displacement Convergence, or Moment Convergence (for some elements).
In Workbench, use File Archive to create a .wbpz file, and do not include results. Put that file (not the .wbpj file!) on a file share such as a Jumpshare, OneDrive or Google Drive (allow anyone with the link to download it). Put the link in your reply and I will download it and take a look. In your reply, say what version (Year and R#) of Ansys you are using.
August 9, 2023 at 2:58 pmPaolo LangellaSubscriber
Thank you for your time, this is the link of my project and the analysis of interest is "Tendon solution - complex". Ansys 2022 R2.
Please let me know if mine is a good way to proceede since, as I wrote in my last reply, in the future we want to make the model more complex adding links, wanting to evaluate the stress in the wires and contact interactions during motion.
August 13, 2023 at 1:31 ampeteroznewmanSubscriber
Cable operated joints are not easy models to get working. I modified your model significantly. In particular, I reduced the cable material Young's Modulus to make it stretch a lot and act like a spring. In a 3-step analysis, step 1 stretches the cables to the left by 10 mm to tension the system, then in step 2 and 3, the top cable returns to 4 mm left while the bottom cable continues on to 16 mm to the left, causing the joint to rotate down. The joint uses Rough contact so that the surfaces can only roll and cannot slide.
Here is the link to the Ansys 2022 R2 archive.
August 14, 2023 at 3:21 pmPaolo LangellaSubscriber
Thank you for your help.
- 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.