February 9, 2021 at 7:04 pmpaganelli9Subscriber
I want to evaluate the deformation only in the chassis frame, but with the force "passing" throught the suspension arms and making no deformation on then, just on the chassis. I basically want to set all the suspension system like "Rigid elements", but I don't know how to do that in Ansys Mechanical. Can someone help me? Thanks guys!
I will upload my project and some images for illustration.
Here is a image of the deformation in all chassis (with the suspension arms)February 10, 2021 at 5:14 pm1shanAnsys EmployeeHelloArray,nTry setting the A-arm material stiffness behavior to rigid. You can find that under Geometry. Also I would suggest you to define a cylindrical joints between A arm and chassis rather then a direct mesh connection and try doing a transient structural analysis. You could have a look at the third tutorial in -https://courses.ansys.com/index.php/courses/time-domain-dynamic-problems/lessons/homework-quizzes-simulation-examples-time-domain-dynamic-problems-lesson-6/nnRegards,Ishan.nFebruary 10, 2021 at 8:25 pmpaganelli9SubscriberHi ArraynThanks for repplying!nSo I changed the material to Rigid in Spaceclaim, because in the Model wasn't making any difference in the deformation, beside I can only change the behavior to Stiff Beam in the Geometry tab inside the Model. But when I make the suspesion A-arms rigid in Spaceclaim I get a very small deformation, a maximum value of 0,00047mm and that can't be correct. I will uppload a image of the situation.nnWhat can I do sir? Again, thanks for your help!nFebruary 11, 2021 at 3:51 am1shanAnsys EmployeenSince I do not know the kind of boundary conditions and forces you applied to your model I cant really justify the deformation. However you could try a methodology similar to https://www.longdom.org/open-access/analysis-of-torsional-stiffness-of-the-frame-of-a-formula-student-vehicle.pdf or someone else. Also, while calculating torsional stiffness the springs are modelled as solid rods (and not actual spring elements which I see in your first model). If you don't want to model the suspension flexure, delete those components from the geometry and just add remote displacements/forces to the pickup points.nnAll the best.nIshan.nFebruary 11, 2021 at 8:33 pmpaganelli9SubscriberHi Array nThanks again for repplying!nI will uppload a image with all my boundary conditions for more details. The image below is from a simulation without the rigid elements set in Spaceclaim.nFebruary 16, 2021 at 12:38 ampaganelli9SubscribernHi sir! Sorry to bother you again, but since you helped me with my project a few weeks ago I thought you would know how to solve this situation too.nThanks a lot for your collaboration sir!nFebruary 16, 2021 at 1:17 ampeteroznewmanSubscribernYou got a small displacement, but you didn't say what forces you were putting in to the model. If you want higher displacement, use higher force. In the end, it doesn't matter because stiffness = Force/Displacement.nDeleting all the A-arms and using a Remote Force (type = Deformable) scoped to all the points on the frame the A-arms attached, is the simplest solution.nFebruary 16, 2021 at 10:51 pmpaganelli9SubscriberArraynHi sir! So I put 2 Remote Forces with 1500N each in the A-arms. I understand what you said to do, but how I will calculate in the formula? Because if I set Remote Force in all the points of the chassis that connects with the A-arms the L in the formula will change.nWhere:nKt = Torsional Stiffness of the chassisnF = Force applied in the chassisnL = Distance from the center of the chassis to the point where the force was appliednBeside that, I will have to decompound the forces in the points? Ex: 375N in each point of a A-arm side.nThanks a lot for your help sir!nFebruary 17, 2021 at 12:45 ampeteroznewmanSubscriberOne Remote Force with a +Y component of F is on the left, at the coordinates of the center of the left wheel. The Remote Force is scoped to all the mount points on the left side of the frame that supports the left wheel, making a spider of rigid elements.nAnother Remote Force is on the right, at the coordinates of the center of the right wheel, with a -Y component of F, scoped to all the points on the right side of the frame that support the right wheel.nPromote each Remote Force to a Remote Point. That will make obtaining the directional deformation of each remote points in the Y direction easy to get deltaY1 and deltaY2.nnFebruary 18, 2021 at 11:29 pmpaganelli9SubscriberArraynHi sir! Thanks for your repllying!nSo I see that you explain my simulation and I understood about the Remote Points for measure the deformation in each side, but if I do that, I'm counting the deformation in the A-arms too, don't it? And if I'm doing that, I'm not calculating only the chassis stiffness, that's my point. Or you are saying that the way that the simulation is set the suspension system is acting like rigid elements? Because in the simulation they are having deformation too. I know how to get the deltasY, but I have to be sure that I'm calculating only the deformations in the chassis. nThanks again for your collaboration, Peter!nFebruary 18, 2021 at 11:40 pmpeteroznewmanSubscriberArraynThe chassis is fixed at one end. You have a rigid handle to torque on the chassis at the other end. You have a force F that is applied to the ends of the rigid handle. You measure the displacements at the ends of the rigid handle. You have a formula that includes the length of the handle, L, which is used to compute torsional stiffness.nDo the calculation once, then make the remote points at twice the distance from the center line. The deltaYs will increase, but so will L and those will cancel each other out and give you the same torsional stiffness.nFebruary 19, 2021 at 8:53 pmpaganelli9SubscribernThanks for your answer sir!nI understood it your explanation and how I will do it. I just have one more question: I have to eliminate the spring system? Because the simulation is set with them. I have to eliminate them or I can make the calculus of the chassis stiffness with them in the simulation?nThanks again and have a nice day!nFebruary 19, 2021 at 10:12 pmpeteroznewmanSubscribernI expect the springs will have an insignificant effect on the result. I expect you would leave them out to measure just the frame.nMarch 3, 2021 at 9:39 ampaganelli9SubscribernHi sir! Thanks for your answer!nSo I leave the spring system out of the calculation, runned the simulation and evaluate this results.nBut then, when I put half of the force that I put before (750N), the results that I obtained aren't linear. Do you know why? And if there are an error?nI will upload my project if you wanna take a look.nThanks again for your help!nMarch 3, 2021 at 9:39 ampaganelli9SubscribernHi sir! Thanks for your answer!nSo I leave the spring system out of the calculation, runned the simulation and evaluate this results.nBut then, when I put half of the force that I put before (750N), the results that I obtained aren't linear. Do you know why? And if there are an error?nI will upload my project if you wanna take a look.nThanks again for your help!nnnMarch 3, 2021 at 9:39 ampaganelli9SubscribernHi sir! Thanks for your answer!nSo I leave the spring system out of the calculation, runned the simulation and evaluate this results.nBut then, when I put half of the force that I put before (750N), the results that I obtained aren't linear. Do you know why? And if there are an error?nI will upload my project if you wanna take a look.nThanks again for your help!nnnMarch 3, 2021 at 9:39 ampaganelli9SubscribernHi sir! Thanks for your answer!nSo I leave the spring system out of the calculation, runned the simulation and evaluate this results.nBut then, when I put half of the force that I put before (750N), the results that I obtained aren't linear. Do you know why? And if there are an error?nI will upload my project if you wanna take a look.nThanks again for your help!nnnViewing 16 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
- 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
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.
Please Login to Report Topic
Please Login to Share Feed