November 22, 2020 at 2:29 amMinggie27Subscriber
Hi, I was doing a landing drop test for my landing gear for ANSYS 2020 R2 free student software.
My computer is running with Intel i7 and GTX 1050.
Here's the screenshot of my entire model and the "solver initialization error".November 22, 2020 at 6:43 pmpeteroznewmanSubscriberArraynIt looks like the material you selected for the landing gear is not supported for ANP tetrahedra.nWhat is the purpose of the analysis?nI recommend you try to run the solution in Transient Structural.nWhat is the material you selected?nWhat is the drop test height? I see a big gap between the bottom of the landing gear and the rectangular block, which I assume is ground. Arranging the geometry at the drop height distance above the ground is not an efficient way to perform a drop test. The efficient way to do that is to arrange the geometry of the landing gear just touching the ground and assign an initial velocity to the landing gear equal the the impact velocity you can compute from the drop height.nWhat is the total mass that the landing gear has to support?nI expect there is more than one landing gear mechanism to support the total mass of the aircraft.nNovember 23, 2020 at 8:15 amMinggie27SubscriberThe purpose of the analysis is to see the von mises stress and the total deformation of the landing gear upon impact.nMaterial I have selected are Carbon Fiber (230 GPa) and Aluminum Alloy 6061-T6 from the material list in ANSYS itself. I did not edit or add any other values inside those material properties.nMy Drop test height is 0.2m. And the landing gear (4 of such legs) has to support 30 kg.nAnd yes, There are 4 of such legs. In this analysis, I only used one.nnBased on your feedback, I will place the block near the landing gear itself, change the material back to the original structural steel. I will also try it in transient structural. Thank you so much for your feedback.nNovember 24, 2020 at 3:35 ampeteroznewmanSubscriberArraynDon't place the block near the landing gear, place it so it is just touching the landing gear. No gap, no penetration, just touching.nDoes your model include 1/4 of the mass that it has to support? If not, you need to add a point mass to represent that.nIf there are 4 legs, but you are only modeling one, then you need to include a Translational Joint or enough Displacement BC to keep the base of the leg level the way it would if there were four legs attached to a frame. Without that, the leg will just fall over in a way it would not if there were four legs on a frame hitting the ground.nNovember 25, 2020 at 2:58 pmMinggie27Subscriber@peteroznewmannMay I ask how do I make the joint work? I tried adding translational, cylindrical and revolute joint on my hinge and the top part is still not moving as much as I thought. It is just bending as if I never add any joint. Sometimes the whole motion just glitches and skip the moving part, and went straight to showing the stress. For my Joint, I select the cylinder surface of the hinge (Green part) as the reference and two of the landing gear structure vertical surfaces as mobile.nAnd how do you use displacement to keep the leg level. Because I do have the problem of the leg sliding off.nnNovember 25, 2020 at 3:18 pmpeteroznewmanSubscribernAdd a Frame body to the model. If you are using Transient Structural and not Explicit Dynamics, you can change the behavior to Rigid.nAdd a Translational Joint to Ground on the Frame Body. This is what keeps the Frame level as one of the four legs makes impact.nAdd a Rotational Joint between the top link in the leg and the Frame Body. This allows that link to rotate relative to the Frame. You might want to add a Rotational Spring into the Joint Definition as there are usually springs in landing gear.nWhat do you have between the two links of the leg? That might also be a revolute joint with a spring.nNovember 30, 2020 at 4:11 pmMinggie27SubscriberThank you for your help! nNovember 22, 2022 at 3:35 amViewing 7 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Earth Rescue – An Ansys Online Series
Ansys BlogTrending discussions
- Explicit dynamics ERRORS
- turning simulation
- explicit dynamics
- getting zero maximum and minimum stress value in explicit analysis
- How to figure out impact force in Explicit Dynamic Analysis
- How do get Full values instead of just minimum and maximum ?
- Monte Carlo Simulation
- Running an explicit dynamics simulation on a composite plate
- Euler Domain Restricting Simulation
- Error inside ANSYS LS Dyna: “An error occurred inside the SOLVER module: general error.”
Top Rated Tags
© 2023 Copyright ANSYS, Inc. All rights reserved.