June 7, 2018 at 3:27 pmmarius_aachenSubscriber
Dear ANSYS community,
I did a modal analysis for a stator-housing combination of a motor using ANSYS Mechanical.
In order to avoid fluid dynamic simulations I modeled oil as a solid using the following material parameters:
- density: 822 kg m^-3
- linear elastic behavior with
- bulk modulus: 1.476E+09
- Poisson's ratio: 0.499
The density and bulk modulus are taken from a datasheet. Since liquids can be assumed to be incompressible I set the Poisson's ratio to 0.499.
In the results of the modal analysis there are hundreds of eigenshapes which only show a deformation of the surrogate solid. These deformations look strange and do not lead to noticeable deformations of the outer housing (not displayed in attached screenshot). Furthermore, the eigenfrequencies of these eigenshapes lie close together. A picture of the deformations of the surrogate solid which should represent the oil is attached.
Do you have any ideas why the deformations look like this? Do I have to choose other material parameters to substitute the oil with a solid? I am glad for each hint you can provide.
June 8, 2018 at 1:16 pmpeteroznewmanSubscriber
The nodes in the oil have a low shear modulus which gives them the flexibility that allows multiple mode shapes to be created. You could just ignore the modes in the oil and focus only on the modes where the stator-housing has a large component.
Did you bond the oil to the stator and rotor or was it frictionless contact? Bonding may help. If you did bond, maybe the modes are coming from nodes internal to the oil. The problem with bonding is that you now pick up the shear stiffness of the elastic solid, which is not present in the oil. You could go with an orthotropic material, but then you have to create a cylindrical coordinate system to keep the radial and tangential directions in each element properly aligned to that axis.
If you make the oil have only one element through the thickness, then there would not be any internal nodes that are only connected to oil. All the nodes would be bonded to the rotor or the stator. ANSYS might warn you that there is only one element through the thickness, but that may not apply if both sides are bonded to something else.
You have two cylindrical surfaces between which is the oil that you want the spring rate included in the model, is it possible to define that as a gasket material? I don't know if that is permitted in a Modal analysis. A gasket must have only 1 element through the thickness, and the nodes on each side are bonded to the coincident faces. That way, there are no nodes that are free to oscillate, yet you have a spring rate between the rotor and the stator. Furthermore, unlike an elastic solid, gaskets only apply a normal force, so the shear force is effectively zero, like a fluid.
Another approach is to define a bushing joint between the stator and rotor to replace the oil. There would be no oil solid, just a bushing joint between the two cylindrical surfaces. I know bushings are permitted in modal analysis (though not in nonlinear statics!). You get to define the bushing spring rate.
In your model, is the rotation of the rotor fixed to ground or is it free?
- 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.