March 12, 2018 at 5:34 pmJosé MantovaniSubscriber
Hello ladies and gentlemens!
I need a little help. I need make a structural analysis of a wheel (see in the image below). I want to know which simulations to submit to do a good structural analysis (how a static strutural, modal, etc.) and possibly improve geometry. Other question is, the material of this wheel is Polyamide 6 (Nylon 6), and I havent found it in engineering data in ansys workbench. If I create the material by introducing the Young Modulus and Poisson's ratio what kind of elasticity should I use? Linear, ortho or ansio ... I already have the wheel CAD model.
I found the Young Modulus for this material:
Min. 2300 MPa and Max. 2500 MPa
The Poisson's Ratio is 0.39.
A image of the real wheel.
Thanks a lot!
March 12, 2018 at 6:23 pmpeteroznewmanSubscriber
Hello my friend José,
What does the wheel roll on? If the wheel rolls on a smooth steel surface then that is simple. If the wheel rolls on the floor and has to roll over bumps, gaps, thresholds, then that is complicated.
What happens at the center of the wheel? Is there a rolling element bearing or does the wheel slip on a smooth fixed shaft?
What is the maximum speed of the wheel? If the wheel rolls very fast and slips on a fixed shaft, then the plastic can heat up and cause problems.
What is the maximum static weight the wheel must support? Is the weight fixed or variable. If the weight is variable, does it spend most of its time unloaded? If the weight is fixed, then you could do a creep analysis.
What temperature does the wheel operate at? If it spends a long time at an elevated temperature under load and requires a long service life, then you must do a creep analysis.
What is the service life expected of the wheel? How many kilometers must it roll before it can be replaced? You could do a wear analysis on the tread and the bearing surface.
Will the wheel be underwater? Nylon is known to absorb moisture and swell up. A tight fit between the shaft and bearing hole could cause a problem when if the wheel has to work under water.
You might have the wheel in CAD, but you have to add a rolling surface and a shaft or bearing to the CAD model. The highest stress will occur when the ground is adjacent to a hole rather than between holes, so place the ground adjacent to a hole.
You should start with a Static Structural system and use an Isotropic Elasticity material for your first model using the properties you found. What you learn there and the answers to the questions above will help to determine which other analyses are worthwhile.
March 12, 2018 at 6:52 pmJosé MantovaniSubscriber
Hello my friend Peter!
So... In this case, that wheel is of a model aerodesign on her, but in the airplane have 3 wheels. The wheels roll in the asphalt without roll over bumps, gaps or thresholds, like a ideal asphalt floor. The wheel slips on a fixed shaft. This airplane model has variable weight, but around 13 to 15 kg. The airplane has a flying speed of approximately 13 m / s, I believe that when touching the ground this speed tends to decrease obviously. Then maximum 13-15 m / s. About the maximum static weight the wheel must support, I believe around 13-15 kg as I said. The wheel is attached to a nylon bushing and secured by a bolt, but it rolls with the bearing. The operating temperature I believe is that of asphalt on a hot day, around 40-60 ° C. I create a new material and setup the Young Modulus and Poissons ratio, I set linear elasticity as You said. But I have a doubt. How I setup the stiffness behavior in the geometry sets? (Flexible, rigid or gasket). And I defined the load as in the picture, for an initial analysis should I do this?
March 12, 2018 at 8:20 pmpeteroznewmanSubscriber
Great detail! The question about what do the wheels roll on should have asked if the wheels ever leave the ground! Impact loads from landing can be significant. Either landing or rolling into a threshold would result in impact loads that can be analyzed in a Transient Structural analysis, but that would come later once the initial Static Structural analyses have been done.
The bodies in the Static Structural analysis are generally Flexible (the default), and are only changed to rigid or gasket for special cases.
What I meant by adding a ground in CAD is something like this:
The piece of ground has a joint to ground, and a joint load applies the force that the wheel should support. Then center of the wheel takes a compression only support. Below is the von Mises stress result.
March 12, 2018 at 8:44 pmJosé MantovaniSubscriber
Oh yes Peter, very good! So, I need join the ground in the CAD Model. How could I carry out this simulation of impact analysis? From the way I set up the loads I got what's in the image above and I got the following message. Now, Peter, how could I improve my geometry? Making one with 6 holes for example and comparing the results? Or lessening the thickness I used? Or even doing other types of holes? I would need to lower the weight of this wheel without lose resistance, in my opinion it is oversized. I get a crazy result! hahahaha. I get this mensage, I do not know if it's because of the wrong way of defining the loads or the size of the geometry. The diameter of the wheel is 80mm, the holes have 17.4mm of diameter and the middle hole 16.3mm of diameter. And I need respect the diameter of wheel and diameter of middle hole. How can I make an wear analysis on the tread and the bearing surface?
Thanks so much, my friend!
March 12, 2018 at 8:56 pmpeteroznewmanSubscriber
That's a funny looking deformation. I attached my model above in an ANSYS 17.2 archive if you want to open that.
There are two approaches to Shape Optimization José.
One is you have a small number of parameters, such as the number of holes, hole diameter and wheel thickness. You set up DesignModeler to have Parameters that can be used in Mechanical to study those parameters.
The other approach is to have no holes and let Topology Optimization take away material that is not needed to support the load. You will end up with organic shapes that are easy to print in a 3D printer, but not easy to turn on a lathe and drill press.
I recommend you try the first approach first. What is the range of hole diameters you want to try? What is the range for hole count you want? You might have to limit the hole diameter range when the hole count gets high or you will end up with no spokes.
March 12, 2018 at 9:06 pmJosé MantovaniSubscriber
Yeah Peter, hahaha it's funny. I will open the archive... think in the 3D printer it is complicated to I make the geometry. In reality I just have to respect the wheel diameter and the diameter of the middle hole (where it fits on the shaft). From the rest everything can be changed, including not necessarily be holes. It could be like a star-shaped wheel, You can understand?.. And I still have trouble reading the diagrams. I have more facility with CFD. For example, what conclusions can I draw from this current geometry. Is it good to "hold" that load, or for example, does not this load "tickle" it?
According to the conditions I told you, is this a good geometry? I think I'll try to reduce 1/3 the thickness of the wheel and see the answers. Or increase the number of holes from 5 to 6. What I need is to decrease the weight. Each wheel weighs 24g.
March 13, 2018 at 2:08 ampeteroznewmanSubscriber
I made a parametric version of the wheel, which has 3 design parameters.
Numholes is the number of additional holes after the first. So Numholes = 5 has 6 holes.
Investigating the tradeoff of Stress with number of holes or HoleDiam is now in a table.
The first model was of the full wheel, but all the stress is in the lower half.
The number of nodes and elements is less than the Student limit, but I cut the model in half to increase the mesh density. Note that the Maximum Stress increased due to the smaller elements. This refinement should be continued to ensure the true maximum stress is captured by the model.
This could be cut in half again through the thickness if there is no need for a side load.
March 13, 2018 at 7:16 pmJosé MantovaniSubscriber
Really, very thanks my friend! I will try to improve my geometry and have a good weight. Today I didnt have time, but I'll open the files you sent me and work on. I forgot to tell you the actual thickness of the wheel, 4.5 mm, then I correct. Again thank you very much Peter!
March 13, 2018 at 8:47 pmpglAnsys Employee
Really nice work and discussion. Thanks for sharing. This is valuable for other Student Community users.
March 14, 2018 at 12:58 pmJosé MantovaniSubscriber
Really nice, sir PGL! It's a real application for the software and can be a ANSYS learning module!
March 14, 2018 at 1:25 pmJosé MantovaniSubscriber
Peter, you stay here my friend?
I opened the files and I'm working on it. It really is very good! But I would like to know the following, I want to submit to 3 types of uploads and also an impact test, which I do not know how to do.. How do I do that (about the impact test)? Can I accomplish the 3 together, or should I duplicate the project and do it separately? A imagem below of the loads types.
Thanks a (very very very very) lot!
March 15, 2018 at 10:02 pmRaef.KobeissiSubscriber
Just reading this thread made my day! Peter and Jose this should be the thread of the year!! Excellent work I truly learned a lot just from reading here.
March 16, 2018 at 1:28 pmpeteroznewmanSubscriber
You always ask great questions.
I created a three model project. The first model has the wheel making contact with the ground, where the axle hole is compression only. The second model changes the axle hole to a fixed support to simulate the brake is on, while the ground pushes inward to represent the weight and the ground pushes sideways to represent the force on the rim from having a brake on to decelerate the vehicle. The last model is the transient solution to the impact of the wheel with the ground.
March 16, 2018 at 6:54 pmJosé MantovaniSubscriber
Oh my God Peter, That is very nice, better than the "girl from ipanema" hahahahahaha!
Take a look at the email I sent you. I'll have to hit the geometry again and leave it as close to the real as possible. Yesterday, as I told you (in the email), when talking to a teacher a guy who works at Embraer arrived and entered the conversation. He told me that he can get some aluminum alloy 2000 and 7000. If this happens I will be able to not only touch the geometry but also the material. I'll let you know.
I do not know how to thank you. Come to Brazil to have a few liters of beer! hahahahaha
March 16, 2018 at 6:56 pmJosé MantovaniSubscriber
Very thanks Raef!
I'm looking to learn more about structural analysis. And for that I have looked for a real case, which will be useful to me, since time is a severe and scarce factor. I decided not only to chat with Peter via email, but also here, because it can be useful for everyone!
Hugs and Have a nice friday!
June 6, 2019 at 6:57 pmsuddtuSubscriber
I read this very useful thread, could you also tell about how to include wear model and most importantly calculating specific wear rate between wheel and road contact considering frictional contact with coeff = 0.3.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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.
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- whether have the difference between using contact and target bodies
- Colors and Mesh Display
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Massive amount of memory (RAM) required for solve
- What is the difference between bonded contact region and fixed joint
© 2022 Copyright ANSYS, Inc. All rights reserved.