July 30, 2019 at 10:44 amVanderbeziSubscriber
i am running a transient Analysis of a rotating part (crankshaft) from 0° to 2160° with torque loads on the crackpins (Joint) and a rotation joint on one End to be uniformly rotated. The problem is that the Stresses I have been getting are too high to be realistic. (around 9000MPa) and keeps increasing.
Can you help me with any ideas about what might be causing this stresses?
I have tested the part's Mesh through a convergence Analysis in static and it does not seem as that part contains singularities and the maximal Stress calculated in static was around(1MPa).
July 30, 2019 at 11:16 ampeteroznewmanSubscriber
Please attach the .wbpz archive file after you post your reply stating what version of ANSYS you are using.
July 30, 2019 at 7:22 pmVanderbeziSubscriber
thank you for your response. I am using the 19.2 version.
I have attached the .wbpz file to this URL: https://filebin.net/lu1g6j0ogdmtzf98
I could not share the exact same Model but I have created a smaller one in which the same stress effect occures.
July 31, 2019 at 3:30 ampeteroznewmanSubscriber
This model has too many constraint elements.
You have one revolute to the two ends. Given the third revolute, this should just be on the left end.
and you have a revolute joint to the center to apply a moment on as a load.
Then you have a revolute joint on the end face, which is the one you decided to apply the rotation displacement load on.
If you are trying to simulate the stress in a crank shaft, you want the forces pushing radially on the correct side of the bearing. Using a Moment on the entire surface does not create forces that just push radially on the surface, it also creates forces that shear on the surface and pull on the surface, which does not represent how forces are actually applied to the crankshaft which is by pure radial compressive force.
July 31, 2019 at 12:53 pmVanderbeziSubscriber
thank you for you answer. I am using Flexible rotation probes to calculate the rotation in some surfaces of the Body. Does applying the Load as you described have an effect on the values of these rotations?
July 31, 2019 at 1:58 pmpeteroznewmanSubscriber
July 31, 2019 at 2:04 pmVanderbeziSubscriber
would the stresses on the pin be right if I created rigid rings around the pins with a revolute joint and a frictionless contact with a small tolerance and then assigned the torques to the rings? If not what can i do to create such radial compressive forces for the whole cycle?
July 31, 2019 at 10:51 pmpeteroznewmanSubscriber
Some people have modeled the connecting rod and piston. The connecting rod has a frictionless contact to the crankshaft pin and a revolute joint to the piston. The piston can be on a translational joint to ground to avoid modeling the cylinder. A tabular force vs time load on the piston is in the model and is tied to the crankshaft rotation.
This is a more realistic model of the loads on the crankshaft because it can include the inertia of the connecting rod, which can put sideways forces on the crankshaft pin that a pure torque on axis cannot.
- 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
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver 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.