May 3, 2018 at 6:40 pmThelibanSubscriber
While solving the Spur Gear (The Dimensions and loads are quoted from a research article), I didn't get the same value as the author got for his analysis. In that paper, the boundary conditions didn't mention clearly. So, by using some engineering assumptions and referring youtube videos I tried to solve that gear, but the error is consistently occurring.
I used full Gear model for analysis, but due to academic element limit, I am unable to solve the full model. I made a 90 deg cut in the gear and used it for analysis. Even though I am getting the error message as shown in figure 1.
Figure: Error Message
To find out the contact stress, I assumed Frictionless contact model for solving the problem. With this discussion, I attached the details of the RESEARCH ARTICLE, ANSYS FILE, the picture of Boundary Condition and Error.
Figure: Assumed Boundary Condition
Figure: Gear Details provided in the Research Article.
Figure: Results compared- the Research Article
Thanks in advance
May 3, 2018 at 10:21 pmpeteroznewmanSubscriber
The reason for the error is that the initial contact status is Near Open. You find this out by right clicking on Connections and Insert a Contact Tool, then on the tool, Generate Initial Contact Results. This is the table you will see.
There is a 3 thousandths of an inch gap. The corrective action is to either rotate the gear to make the teeth tangent, or to edit the contact and under Geometric Modifications, Interface Treatment, set it to Adjust to Touch.
Under Analysis Settings, I usually set Auto Time Stepping to On and Initial Substeps to 10 and set Large Deflection to On. While there, scroll down to Output Controls and say Yes to Contact Misc and all the outputs.
While the Frictionless Support 2 and Displacement will work, it really slows down the solution time. Much better to delete those and insert a Revolute Joint. You can also delete the moment and put in a Joint Load. The joint load applies a force through the hub of the gear which is much closer to the load path through the part than the moment that was applied to the flat side of the gear.
I made all those changes your model, then it wouldn't converge. I put a minus sign on the moment and it easily converged. The reason is that the contact was touching on the minus torque side of the tooth, so a positive torque opened the contact and went nowhere, while a negative torque pushed the contact pair together.
Attached is an ANSYS 19.0 archive.
I have more to say but I will put that in another post.
May 4, 2018 at 1:36 ampeteroznewmanSubscriber
May 4, 2018 at 1:45 ampeteroznewmanSubscriber
May 4, 2018 at 1:45 ampeteroznewmanSubscriber
See the blank post above, it contained a long and detailed explanation of how I improved the model, but when I hit Post, all I got was this blank post. I'm not going to retype it all, I will just add a few figures that are saved separately. You can look at the attached archive and figure it out for yourself.
The gist of the post was that you don't have real tooth geometry, you have a poor CAD facsimile of the real tooth profile and that is not good enough to do FEA on. You don't even have a fillet at the root of the tooth, which is arguably the most important feature after the face, which should be an involute, but probably isn't.
May 4, 2018 at 1:57 amThelibanSubscriber
Thanks for your explanation,
1) Why are we doing initial gap calculations? From that What we will infer?
2) In BC, we are fixing one gear and give the moment to another one, but in the real case, both the gears will rotate right? What is the assumption behind that fixed support? (I thought, while giving fixed support, we are analyzing for worst case condition).
3) Here, I didn't use symmetry BC, but I analyzed a part of the gear. Whether this thing rise to an error (magnitude) in solution?
4) The result which we got from Contact Tool
> Pressure, is equivalent to the Hertzian Stress? Can we validate the Ansys result using the Hertzian Stress Equation?
May 4, 2018 at 2:04 amThelibanSubscriber
Ya, I will try to understand what changes you made to get those results.
I generated these gears from Solid Works toolbox, to have a better gear geometry, What should I have to do?
Really Thanking you for your effort to clearing my doubts.
May 4, 2018 at 2:29 amThelibanSubscriber
The point, I understood from your modifications,
1) Sliced out the unwanted portions from the gear.
2) Made the contact at one pair of a tooth at a time.
3) I didn't get the reason behind the symmetry about plane 7.
4) Reduced the element size at the contact region using Sphere of Influence Method.
May 4, 2018 at 2:30 ampeteroznewmanSubscriber
1) You do initial contact status to check that frictional contacts are initially closed. If they are not closed, you should take some corrective action. For example, in the second model, I rotated one of the gears until it was visually a tangent (after I increased facet quality to 10). The reason is the contact algorithm needs a closed contact to start the simulation.
2) Yes both gears are really rotating, but the contact force dominates and this can be analyzed as a statics problem. Fix one side and apply the torque to the other. Do you have a good idea about the line of contact between the gears. This webpage has an excellent animation that you must watch. The worst case for stress may not be when the contact is at the pitch circle.
3) By using symmetry through the center of the thickness of the gears I was able to use twice as many elements on the tooth while staying under the Student limit.
4) Pressure is on the surface and is valuable for selecting lubricants. Hertzian stress includes the stress below the surface. The peak equivalent stress is actually below the surface.
Bonus question: to get better gear geometry, don't use the SOLIDWORKS toolbox. That is not real gear geometry, it is just a spaceholder in the assembly and the geometry is far from accurate for FEA input. Most importantly, it does not have a root fillet!!! To get accurate gear tooth geometry, you have to construct all the detailed curves in the profile of the gear. There are more details besides the root fillet. Talk with a gear design specialist or read a lot more about gear design, and not the basic information, but references that talk about the manufacturing details.
You can show your appreciation by clicking Like below the posts that are helpful.
May 4, 2018 at 1:55 pmThelibanSubscriber
By using the Hertzian Contact Stress equation from Mechanical Design by Shigley, I validated the result and got the similar result.
In many research article, they have validated the bending stress induced in the tooth also, for bending stress they checked the equivalent stress value. In my case, the equivalent stress is too high when compared with the AGMA equation from the same book.
Thanking you for your continuous support!
May 9, 2018 at 2:04 pmThelibanSubscriber
By creating the involute profile for the gear by myself, The equivalent stress value reduced drastically and I'm getting value with deviation about just 20% with the value of base reference paper.
May 9, 2018 at 10:29 pmpeteroznewmanSubscriber
That is encouraging news Theliban. Good luck.
- 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.