August 27, 2023 at 6:32 amKiran KolluruSubscriber
Hi, I am trying to simulate a table with two trunnions and shafts at either end. Both the shafts are given revolute joints. Shafts are connected to table through fixed joints. Standard Earth Gravity applied in downward direction. Rigid Dynamics analysis was carried out for one full revolution - for 30 seconds with 2 rpm rotational velocity. Total force from joint probe for both the revolute joints are extracted. Only one revolute joint is taking full load. Other joint is showing 0 N. Can someone please explain how to correct this so that equal force reaction comes on both the joints? Thank you.
August 28, 2023 at 12:35 ampeteroznewmanSubscriber
A rigid body has only 6 degrees of freedom. A revolute joint with an angular velocity load applies 6 constraints. That means the second revolute joint is redundant and the correct answer for the loads through this joint is zero.
You need to use Static Structural and have flexible bodies to share loads between two pins.
August 28, 2023 at 5:51 amKiran KolluruSubscriber
Hi Peter, thank you for the reply.
Yes, static analysis gives reaction on both shafts correctly. But in static analysis, the platform is not moving 360 deg if rotational velocity is given (even with Large Deflection ON). So the variation of forces in one revolution of the platform cannot be obtained, which is possible in rigid dynamic analysis.
I have applied rotational velocity just to check force extraction procedure. End objective is to find the dynamic forces on the shafts due to acceleration and sudden stopping of platform. If rotational acceleration is applied in static analysis, it gives error - solution magnitude exceeded.
Can you please suggest a workaround for the above issues? Thank you.
August 28, 2023 at 6:19 am
August 28, 2023 at 2:27 pmKiran KolluruSubscriber
Hi Peter, referred to your comments in following two links which are useful in understanding Revolute Joint and Rotational Velocity "load" simulation in static structural.
I could successfully simulate the static analysis for 360 deg (in 30 seconds) by giving Joint Rotation for Revolute joint (it is not accepting rotational velocity showing a question mark). I have few questions.
1. Though the earth gravity is always acting downwards, the reaction force at the revolute joints is rotating with the platform. Technically it should always point upwards because weight acts downwards - in whichever orientation the platform stays. Why this difference?
2. Moment about Z axis (or torque) at the revolute joint is shown below. It's variation is not fully understandable or is the time step too coarse and hence the jumps observed in plot discreetly?
3. Why Joint-Moment input for Revolute joint is causing solution magnitude exceeded / non convergence error even for a small moment value? Ideally it should move to an angle corresponding to the torque. How can we input torque without getting this error?
August 29, 2023 at 10:03 ampeteroznewmanSubscriber
I will take a look at your model if you share the archive. In Workbench, use File, Archive to create a .wbpz file. Don't save results to keep the file size smaller. Put that .wbpz file (not the .wbpj file) up on a file sharing site such as Google Drive, OneDrive or Jumpshare and put the link to that file into your reply. If using Google Drive make a link that anyone can use to download the file. Say what version of Ansys you are using, year and R#.
August 29, 2023 at 5:56 pmKiran KolluruSubscriber
Hi Peter, thank you for the help. Please find the .wbpz file at the following link with mesh and results removed. Please let me know if you cannot access this file, it is on Google Drive. ANSYS version 2023 R1.
I tried rotational velocity and rotation for the joints in Rigid dynamics, it works well and gives same results for joint forces. However, as explained earlier, in Static Structural Rotational Velocity or Acceleration for the Joint Load gives error.
If there is some way to get both revolute joints same load in Rigid Dynamics it will be good as several velocity and acceleration changes can be studied quickly.
August 29, 2023 at 11:59 pm
August 30, 2023 at 6:41 amKiran KolluruSubscriber
Hi Peter, thank you very much for the inputs. I could reproduce the moment graph as shown by you by changing the substeps.
I also noticed that the direction of joint probe force is changing along with platform orientation because ANSYS is reporting the force in joint reference coordinate system (which is rotating) and not in global coordinate system.
And Joint Load - Rotational Velocity and Joint Load - Rotational Acceleration could be given only in Transient Structural and not in Static Structural.
Thank you once again.
- 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.