November 28, 2018 at 5:11 amENV159Subscriber
I am doing a modal analysis (free vibration) for a rotating shaft. Are fixed supports in place of the bearings the correct boundary conditions? Do my results make sense in regards to the frequency (Hz) value? The first mode frequency when converted to RPM is 314400 RPM. Does this value seem too high?
November 28, 2018 at 4:05 pmpeteroznewmanSubscriber
Using Fixed Supports is wrong as it eliminates the correct torsional mode. Does the shaft have gears or other large masses fastened to it? The model should include a disk with the same mass moments of inertia as the actual part fastened to the shaft to get correct vibration modes of the shaft assembly. The vibration of the shaft without the added parts is not that useful.
Which coordinate direction is the axis of the shaft? I will assume it is the Z axis for the description below.
Create a Remote Displacement on one face. Set X, Y and Z displacement to zero, leaving the rotations free.
Create a second Remote Displacement on the other face, set X and Y displacement to zero, leaving the others free.
In the modal results, the first mode will have a zero (or very small) frequency. That is the rigid body rotation of the shaft. Just ignore Mode 1. All the other modes will have a non-zero frequency, including a torsional mode and various bending modes.
Instead of two Remote Displacements, you could use two Bearing Constraints, one on each of the two faces. You have to also constrain the axial motion with a remote displacement and have only Z=0 leaving all others free. That would add the flexibility of the bearings (and housing depending on how you define K) to the modal analysis and the vibration modes will include radial displacement of the bearing faces on the shaft.
November 28, 2018 at 4:36 pmENV159Subscriber
Thank you, this is what I was looking for. And the shaft is just simply bearings.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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.
- How to calculate the residual stress on a coating by Vickers indentation?
- Errors – Reinforced Concrete Beam
- Solver Pivot Warning in Beam Element Model
- An Unknown error occurred during solution. Check the Solver Output…..
- 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
- Massive amount of memory (RAM) required for solve
- Cannot apply load on node
- Large deflection
- Colors and Mesh Display