September 12, 2019 at 9:35 pmyanivVKSubscriber
I am working on a modular robotic manipulator arm to be used for fruit harvesting. I have designed the modular parts - the connector segment, the base plate and the stopper. I have modeled them in SolidWorks and combined the connector, base plate and stopper to form one body using the 'combine' tool in SWs so that the number of contact regions are reduced in ANSYS. I am trying out the static analysis at the maximum deflection position of 20 deg with three modules. It solves with my set up of fixed support (purple colored base ring), standard gravity in -Y direction and an applied force of 30 lbf (shown by the red arrow). The deflection and stress values seem reasonable. The material used is Al-6061. I have added springs in between the modules to represent the behavior of spring bellows/actuators that we would need in the robotic arm.
My issue is that since ANSYS provides an option for a virtual spring and it only has a longitudinal behavior, it is not resisting the deflection due to bending. As a result my end point deflection values are over 2.5 inches which is not desirable. I want to know if there is a way to add a bending behavior to these springs so that these could behave like an idealized spring actuator/bellow. That would give me a better result related to the total deformation value and would be much closer to how the system would behave in real life.
Other relevant info:
-ANSYS version -2019 - research licence
-I have used spherical joint and contacts for the ball and socket joint
-Spring K=30 lbf/in ; preloaded with free length
- I have tried changing the behavior of the 'reference' and 'mobile' part of the spring to 'deformable' and 'beam', but there is no change in the results.
If anyone has any ideas as to how to do it, kindly let me know. Do I have to physically model the spring bellows/actuators in SWs to actually do the analysis?
September 17, 2019 at 1:12 ampeteroznewmanSubscriber
Add three beams in parallel with the springs to represent the bending stiffness of the bellows on each base.
The beams would be fixed to each base and have a 3D line contact of beam inside beam contact definition to beams on the next base.
It would be ideal to have a single point on the CONTA177 side of the contact pair but that might not be allowed. There is a CONTA175 that is a single node, but I don't know if it can operate inside a beam.
September 20, 2019 at 6:01 pmyanivVKSubscriber
I apologize for replying late.
Thank you for the reply. I have a few questions. How do I insert hollow beams in workbench? I tried using the 'beams' option from insert and it has options for circular beam between reference and mobile surfaces. Do i have to model the hollow beams in SpaceClaim ? And how to decide the size of the inner beams?
Also, I was wondering if there is a way to add cables/wires in ANSYS like we add beams and springs?
September 20, 2019 at 11:05 pmpeteroznewmanSubscriber
Beams are either hollow or solid as an assigned property that has nothing to do with geometry, just like the radius of the cross-section is an assigned property. Geometrically, they are both just line bodies. These properties are assigned using APDL code objects under each line body in the Geometry branch in the outline in Mechanical. Here is an example, but you don't want LINK180 elements, you want BEAM188 elements.
Note that when you mesh, you must set the element order to Linear if you use BEAM188 elements and set the element order to Quadratic if you use BEAM189 elements. The mesh element order has to match the order of the element in the APDL command or you will get an error.
The radius of the cross-section of the beams depend on the bending stiffness you want to achieve. Small radius beams generate low forces, larger radius beams higher forces for the same lateral deformation.
Cables and wires are modeled using line bodies and usually use Links instead of Beams. Links have rotational freedom at the end of each element. There are some discussions on this site you can read about.
- 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.
- Saving & sharing of Working project files in .wbpz format
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- 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.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.