November 8, 2018 at 11:46 am
November 8, 2018 at 1:05 pmpeteroznewmanSubscriber
Step 1 Create the geometry.
Read the ANSYS Help on Import Shaft Geometry for DesignModeler. That will create the shaft geometry from a simple text file.
Are you going to add a fillet radius (blend) at the interior corner of each step in the shaft (more difficult) or are you going to leave them sharp (easy)? If you don't add a fillet radius, then your model will have a stress singularity in the solution. That means the maximum stress in the model depends on the element size. The smaller the element, the larger the stress, without limit. That means the fatigue life depends on the element size. Once you add a fillet radius, you eliminate the singularity from the model and there is an exact maximum stress for the model and as the elements get smaller, the solution will converge on that exact value.
Are you going to include the keyway slots (more difficult) or are you going to ignore them (easy)? Since the torque load on this shaft doesn't reverse, the keyway doesn't see the load go from one side to the other. It only sees the change in stress from the rotation of the shaft. In that case, the maximum cyclic stress is probably not going to be at the keyway because it is on a large radius section of the shaft and one of the small radius sections will have the maximum stress. That is a good justification for excluding the keyway from the analysis.
Step 2 Define the material
Are you going to use the ANSYS Structural Steel, which has Fatigue data included?
Step 3 Create Static Structural Model
A bearing support can hold each bearing face, but that is only 4 Degrees of Freedom (DOF) for the shaft. On one end of the shaft, use a Remote Displacement and set the axial direction to zero, leaving all the others Free. You now have supported 5 DOF. On the left gear bearing face, create a remote point on the pitch circle for that gear. Set the displacement to zero for the tangential direction. You have now supported all 6 DOF for the shaft. Apply the radial force to that remote point. On the other gear bearing face, create a remote point on the pitch circle for that gear in line with the first remote point. Apply the radial force to that remote point.
The tangential force on each gear requires some thought because the tangential displacement was just set to zero on the left gear to support the shaft. Nothing happens if you put a force on a point that you just fixed the displacement on.
The figure shows the left gear has a tangential force of 2400 N while the right gear has -10800 N which is a 4.5 ratio. For the shaft to be in equilibrium, that is for the torques to cancel each other out (neglecting bearing friction), the radius at which each tangential force is applied must also have a 4.5 ratio. The pitch circle diameters for the two gears have not been provided, but a 4.5 ratio must be present for the forces to balance. That means you can apply a tangential force to just the right gear remote point and you will get the correct torque in the shaft.
November 8, 2018 at 4:16 pmBruno1995Subscriber
Thank you peteroznewman.
- 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.