February 10, 2022 at 1:51 pmarv2995Subscriber
I wish to know the boundary conditions for this physical problem to calculate the static deflection of the shaft in lateral direction at various locations .
I have to do the structural analysis and check the static deflection of a shaft. The following is the arrangement of the system. The shaft is supported with 2 bearings. It also has 2 rotors at its 2 ends. I wish to apply the boundary conditions in ANSYS Structural so that the solver does not gives errors.
If we consider each bearing it has 2 reaction forces and 2 moments as unknowns, each. The values of reaction force and moment are already known calculated through another type of analysis. Can we use these values as boundary conditions?
Kindly help me with this problem.February 10, 2022 at 5:35 pmTomPhemmySubscriberYou can do that but you should answer the following:
What type of analysis was performed for you to know the forces and moments of the bearings?
do you intend to do a linear analysis (material and geometry wise)?
How is the bearing connected to this rod? i.e. what DOFs are allowed or restrained from motion.
From your post i can only deduce that since you have 1 force and 1 moment reaction per bearing, you are saying the system you are modeling lies in the 2D plane? and the bearings cannot generate axial force in the attached rode? so small deflection analysis?
You might need to provide more details on how you obtained your bearing loads. Pictures of your model geometry will also be good.
February 11, 2022 at 9:21 amarv2995SubscriberThanks for the reply.
What type of analysis was performed for you to know the forces and moments of the bearings? - A CFD Analysis of the system gave the values of resultant forces and moments at the bearing.
do you intend to do a linear analysis (material and geometry wise)? - What is your suggestion? I think I want to include contacts so it might be a nonlinear in that sense. Main motive is what are the deflections when the shaft is suspended with its values on the 2 bearings and the 2 rotors at the ends.
How is the bearing connected to this rod? i.e. what DOFs are allowed or restrained from motion. - The following link will answer the question.
CHP5.5-5.6.pdf (utep.edu). please check this link. Single journal bearing is the one which is my case.
Assume the axis of shaft is Z direction.It isconstraining motion in X and Y direction. Hence has a corresponding Fx,Fy and Mx,My generated. The resultant moment and force are calculated with CFD analysis. Should I use these as bearing loads in ANSYS Structural settings for BCs.? The bearing is not an axial bearing it is a radial bearing.
February 11, 2022 at 1:12 pmpeteroznewmanSubscriberThe boundary conditions depend on how you model the shaft. If the shaft is modeled with beam elements (recommended), then one bearing would have a Simply Supported BC at the vertex, which means X, Y and Z are all Fixed. The other bearing has a Displacement constraint of X=0, Y=0 with Z Free (shaft is along the Z axis).
A Static Structural solution requires all 6 DOF to be constrained, which is why the first bearing needs a Z displacement set to Fixed. In reality, somewhere along the shaft, a thrust bearing is present. It may be on one of those bearings or it may be on one end of the shaft or the other (not both!). That adds up to 5 constraints, which allows the shaft to spin, which is fine in reality, but no good for the Static Structural solver, which requires the rotation of the shaft to be fixed somewhere so it can solve.
A single constraint is needed to prevent rotation about Z. You haven't mentioned the moment about the shaft axis, which is the whole point of the entire system. While this moment may not cause lateral deflection of the shaft, it creates stress in the shaft that must be included in the analysis of the shaft. Under steady state operation, the moment about Z from the turbine is equal and opposite to the moment about Z from the compressor. At one bearing only, apply a Fixed Rotation and set Rotation Z Fixed, leaving Rotation X and Rotation Y Free. Ask the CFD model to provide the moment about Z on the rotor and apply that to the vertex at other bearing (without the Fixed Rotation).
February 11, 2022 at 1:28 pmpeteroznewmanSubscriberThe CFD model solution provided a complete pressure map for the compressor rotor and a complete pressure map for the turbine rotor. CFD post processing was used to sum the pressure map to compute the forces and moments at each bearing. Having the forces and moments is sufficient to design the bearing and the support structure for the bearing. The forces and moments at the bearing are not the best input to compute the static deflection in the shaft. It will show the deflection of the shaft between the bearings, but does not show the correct deflection of the shaft that overhangs from the bearing to the rotor hub.
A better input for shaft deflection would be to sum the pressure map at the rotor hub. Then when you apply forces and moments at the rotor hub, the shaft bending will include the overhang of the rotor from the bearing.
If you can't get new output from the CFD model, you can use statics to calculate the Force and Moment at the rotor hub and apply those newly calculated values to the shaft vertex at each rotor hub. That will cause deflection in the overhangs.
Viewing 4 reply threads
Ansys Innovation Space
- 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.Trending discussions
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- 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
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Colors and Mesh Display
- User manual
- material damping and modal analysis
Top Rated Tags
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.