March 23, 2023 at 8:33 amLear NerSubscriber
Say I want to do a structural analysis (deformation/equivalent stress) on a compressor impeller for an overspeed run..
For the overspeed run the impeller bore will have a 0.0mm fit with the shaft. Axial bore face 'B' is pressed against a shaft shoulder. Face 'A' will be limited in axial movement by a plate which is bolted onto the balancing shaft.
Which boundary conditions should I apply in this example?
2nd question: Say the impeller bore has an interference/shrink fit with the shaft. Would a simple displacement BC suffice? Where the displacement value is set only to mimic the shrink fit, and leave the other 2 displacement coordinate components at 0 mm?
March 23, 2023 at 12:59 pmpeteroznewmanSubscriber
For the slip-fit impeller, I suggest scoping a Remote Displacement, Behavior = Deformable, to the two contact faces on the ID of the impeller and setting all six DOF to 0. This completely constrains the rigid body motion of the impeller and allows the solver to run. This allows the ID to expand with the rotational velocity and the distance between the A and B faces to contract due to Poisson’s ratio effects. Make sure that the Behavoir of the Remote Displacement is not set to Rigid because that would prevent the deformations I just described. There is no need to apply any boundary conditions to faces A and B.
An alternative is to model the shaft with a shoulder and the plate. Bond the ID of the plate to the shaft. Slice the face of the shaft at the plate to use Bolt Pretension on the face of the shaft between the plate and shoulder. That will sqeeze the impeller with the force that torquing down a nut on the plate would do. Then apply frictional contact between the A and B faces of the impeller and the shoulder and plate. This requires a two-step solution. Step 1 has a 0 rotational velocity and the bolt pretension builds up. Step 2 the bolt pretension is locked and the rotation velocity is applied.
Answering the second question, I suggest adding a section of the shaft in the hole and putting frictional contact between the shaft and ID of the hole in a 2 step analysis. Step 1 has a zero rotational velocity load, only the interference is resolved, then step 2 applies the non-zero rotational velocity. Make the cut in the shaft at approx. 2 diameters past the A and B faces so you can apply fixed supports to those faces without affecting the material in the interference fit part of the shaft. This type of analysis may benefit from increasing the Displacement tolerance under Analysis Settings, Nonlinear Convergence to a Tolerance of 0.01% instead of 0.5%. Turn on Large Deflection, which should be done for the slip-fit solution also. Assuming the interference is maintained at the overspeed rotational velocity, you won’t need any boundary conditions on faces A and B.
The above correctly apportions the interference between the shaft and impeller according to their respective stiffnesses. There would be a small error if you apply all the interference to the impeller alone.
- 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
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- User manual
- 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
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.