September 25, 2020 at 6:14 pmxiaoSubscriber
I tried modelling the cale strcture with Link180 elements. The cable is divided into 20 elements. I do the following steps to analyze the strcture
1. From other resources, find the shape of the cable. Extract the coordinate of the cable and put it in the txt file. Format the txt file so that it follows the format of the ANSYS DM.
2. In ANSYS DM, read the txt file and connect the line using the points. Assemble them as part.
3. In the model --> geometry, add APDL commands as in the figureSeptember 26, 2020 at 8:47 ampeteroznewmanSubscribernWhenever you put numbers in a Command object that require the units to be set a certain way, it is best to go to Analysis Settings and set the Solver Units to Manual and set the system correctly as I have done below. By default, the solver will use whatever the units system you left Mechanical set to. In my case, I opened your file and it was set to mm. Is the cross-sectional area property in your Command in square meters or square mm? Without making the setting I show below, you will get a different solution depending on the current units setting.nI see you are using ANSYS 19.2 and that is important to say in case someone spends time fixing your model in a later version and you won't be able to open that file.nSince this is basically a 2D problem in the XZ plane, you can help the solver out by setting all the bodies to have a Y=0 displacement boundary condition.nWhen I run the model, there is this warning.n *** WARNING *** CP = 0.531 TIME= 04:14:00n For element type = 1 (LINK180), KEYOPT(3) = 1 is an undocumented option. nWhy are you using this?nWhen ANSYS solves the Statics problem, it is searching for equilibrium of all the forces. If you have drawn a perfect catenary shape and used the correct initial strain, then the solution would make no deformation.nANSYS will not consider self-weight if you don't turn on the Gravity load.nI can get a solution with the Force in the center.nYou have one line body that you meshed with 43 beam elements, then converted those to link180 elements.nI don't know if the Command that converts Beam elements to Link elements has the same effect as setting the Model Type to Link in the Details.nThe problem is if you do that, you need 43 line bodies to be drawn in DesignModeler because you can only mesh one link element per line body.nBelow is the deformation with Gravity only, magnified 100 times. Maybe your initial catenary share has these errors in it, and ANSYS is providing the correct deformations. You could try drawing a straight line and then let ANSYS deflect it into a catenary shape and see what that looks like.nANSYS 19.2 archive attached.nSeptember 27, 2020 at 8:56 pmxiaoSubscriberHello Peter,nThanks so much for your reply. But I still have some questions.nThe unit system I use in MD and Model is mks. The cross-section of the cable is the circle2 is 3.1415e-04 m^2. I don't know why when you open my file, the unit system becomes mm. Maybe this is because when I check the results, I changed the unit into mm. nThe command line 'keyopt(3)=1' is of nonsense. But this command doesn't make any change to the solutions. I added it in to my APDL command is because I paste and copy this command from previous one and forget it delete it.nThe geometry of the catenary shape of the cable I got is from SAP2000 built-in catenary element. The coordinate of the nodes and the end force is shown in the figure below. nIf I understand your suggestion correctly, you suggested to change the initial strain to be the actual strain which can be calculated as F/E/A = 1.4686e-06. After I changed the strain to be that value, the displacement of the cable under gravity is still a positive value. But as you suggested, if the initial strain value is correct, the displacement of the cable under graivity should be zeros.nI ran the model in the attached file. The purpose is that I would like to see what is the displacement of the cable under -10 N or even higher vertical load. But when I increased the vertical value to -10N, the solution diverge.nDo you have more suggestions?.Sincerely,nXiaonnSeptember 27, 2020 at 10:24 pmSeptember 27, 2020 at 10:55 pmxiaoSubscriberHello Peter,nThanks for your quick reply.nYes, this model can run under -10N in the Z directin.From SAP2000, I calculated the catenary shape and I extracted the end force from the cable under gravity. Then I applied the initial strain under that end force (tension under self-weight). But, still, the displacement under gravity is still positive. I really confused about this point. nThe APDL command i appled is based from this post https://forum.ansys.com/discussion/5740/transmission-line-simulation. From this post, the APDL commands are used just to initiate the nonlinear lateral stiffness.nXiaoSeptember 28, 2020 at 12:29 ampeteroznewmanSubscriberUnder 10 N and gravity, the downward deformation was 10 mm, while under gravity only, the deformation upward was only 0.077 mm or 0.77% of the -10 N deformation. That is a small number. FEA solutions with less than 1% error are useful models.nSeptember 28, 2020 at 12:16 pmErik KostsonAnsys EmployeePeter is absolutely right here. We could not expect the deformation to be exactly zero under gravity, but as pointed out something quite small, and smaller than the deflections under applied forces.nnThank younnEriknViewing 6 reply threads
Ansys Innovation Space
- 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.Trending discussions
- 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
Top Rated Tags
© 2022 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.