October 28, 2023 at 9:46 pmKarol SołtykSubscriber
Hello Ansys community,
I am currently working on an analysis of a mechanical device (Solid 1 and Solid 3) where the primary goal is to accurately represent the physics of the device, and not to analyze the rope itself. For this purpose, I've created the rope (referred to as Body 2) as a single solid. I apply either displacement or force to one end of the rope, and due to the friction between the rope and the curved part of solid 1, it causes solid 1 to rotate and squeeze the rope between solid 1 and solid 3.
The rope is composed of multiple individual fibers and has low transverse stiffness; it is not a homogeneous block of isotropic material, and the individual fibers are not bonded together. My question is: what is the simplest and most effective way to represent the properties of this rope in Ansys?
Is the main challenge here to define the rope as an orthotropic material? I'm quite new to using Ansys, and I'm struggling to find the right approach to model such a rope accurately.
Any help or guidance on how to model this rope in Ansys would be greatly appreciated. Thank you in advance for your assistance. I'm an amateur in using the Ansys software, and I'm having difficulty finding the solution to this particular modeling problem.
October 30, 2023 at 1:58 pmDave LoomanAnsys Employee
It would be more practical to model the rope with the cable280 element. Use a small contact stiffness factor between the cable280 and the surfaces of the solid bodies to help convergence. With a 3D model of the rope it will be difficult to simulate the low bending stiffness, but more importantly, will be hard to solve for a large amount of motion.
October 30, 2023 at 9:20 pmmjmiddleAnsys Employee
Are you using workbench Mechanical or APDL GUI?
Use SpaceClaim or DesignModeler to define a beam with cross section. You may need to share topology on line and arc segments.
In Mechanical, in the Details of the beam under Geometry, set the "Model Type" to either "Link/Truss" or "Cable."
The Link/truss will make link180, which is a linear element (2 end nodes). The cable will make cable280, which is the quadratic version of the element (2 endnodes, and a mid node), if the Mesh setting is not set to linear.
1. Command object is necessary (inistate) in the environment setup (Static Structural) to put some initial stress (tension) on the link180 or cable280. This is necessary in static simulations since the cable is just a bunch of pinned link elements now. Imagine holding up a chain in space (no gravity) the links have no lateral stiffness w/o tension.
cmsel,s,cable ! place the geometry edges in a named selection first, name "cable" in this case
esel,r,enam,,180 ! Or use 280. may be necessary if there are contacts scoped to the line bodies, since overlain contact elements are created on the line bodies
inistate,define,,,,,100 ! to define an initial stress
!inistate,set,dtyp,epel ! or set an initial strain
2. Large deflections must be on
3. At least 2 load steps. In first load step, a constraint mush keep the cable from contracting due to inital stress (inistate). Deactivate this constraint in the second load step and apply other loads in second load step.
4. link180 has to be meshed very fine to prevent a faceting behavior as it still is just a bunch of links. Cable280 can use less elements.
5. Substep size should be limited to be small enough so that the contact between the link180/cable280 and the surface does not change status too quickly, otherwise you may see the cable penetrate the solid if displacements change too quickly, pinball (next bullet point) should be set sufficiently large to help prevent this as well.
6. Pinball region on contact should be made bigger than default. Make sure it is larger than the gap between the cable center represented by the beam and the 3D body faces. Specify the "Offset" for the "Interface treatment" or "Adjust to touch." If this is hard to converge and the cable is small diameter you can model the center of the cable (beam representation) to lay the 3D bodies in the CAD modeler, which will be easier to converge.
October 30, 2023 at 9:27 pm
- 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
- 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
- A solver pivot warning or error has been detected
© 2023 Copyright ANSYS, Inc. All rights reserved.