September 26, 2020 at 1:41 pmValiullinDamirSubscriber
Hello, dear colleagues!
Your help is needed: i cannot solve my problem with contact in shell model.
I have a quite big assembly with bolt pretensions. At the first step, pretension loads are applied, and at the second step they are locked and the external loads are arise. All the contacts are frictional and all the details work together because of the bolt pretensions. The whole assembly consists of shells created by Midsurface option in SpaceClaim (i have solid model created in Solidworks). All the bolts are beams and they are connected to shells like @peteroznewman did it in this video:","embedType":"youtube","name":"Shell Mesh Joint with Bolt Pretension","frameSrc":"https://www.youtube.com/embed/tQykfXMuQp4?feature=oembed&autoplay=1"}">September 26, 2020 at 2:43 pmpeteroznewmanSubscriberI suggest you use Bonded Contact on one side of that detail piece to bond it to one flange. The other side of that detail piece can retain Frictional Contact with the other flange.nSeptember 27, 2020 at 6:50 amSeptember 27, 2020 at 11:22 ampeteroznewmanSubscriberInsert a Contact Tool under the Connections folder and Evaluate Initial Contact Status. You can remove the Linear (Bonded) Contacts and only look at the Nonlinear (Frictional) Contacts. They should all be Closed assuming you have no deliberately open gaps.nIf that is the case, then under Analysis Settings, turn on Automatic Time Stepping and set the Initial Substeps to 100. That may fix this problem. If it does not, try 1000.nSeptember 27, 2020 at 4:41 pmValiullinDamirSubscriberI have checked Contact status in Connections folder - and all the Contacts are closed. Now i started the Solution with 100 Initial Substeps - it will take quite a long time, but Total Deformation plot tracker shows, that we have penetration at this zone:nSo, it is a really strange thing - when i chose Bonded type for manually created Contacts - everything is fine (there are no penetration and flying details), but when i chose Frictional type for them - such a thing occurs. nSeptember 27, 2020 at 7:25 pmpeteroznewmanSubscriberIt's not strange at all, it is expected. nBonded contact is linear, which means it is easy for the solver to find equilibrium.nFrictional contact is nonlinear, which means it is difficult for the solver to find equilibrium.nIn complicated models, extraordinary steps are sometimes required to get nonlinear contacts working.nBut first, check that you actually have large penetration or is it in fact just an exaggerated displacement display scale? When you click on the Results tab, there is a displacement display scale area on the ribbon. The display scale defaults to an automatic value, which might be thousands of times larger than reality. Change that setting to 1.0 (True Scale). Did the parts return to their normal positions?nIf you were already showing True Scale plots, then make sure you have selected the correct side of the shell to make contact with. Maybe Bottom is wrong and it should be Top or vice versa.nSeptember 28, 2020 at 3:14 pmValiullinDamirSubscriberthank you for help!nIn my case, it was penetration, not big displacement. The last picture i have attached was made with True Scale size. nChoosen shells sides were correct too. nThe problem was with small pinball radius. I increased it to the value that 0.1 mm bigger, than distance between midsurfaces - now solution goes right. nSeptember 28, 2020 at 7:22 pmpeteroznewmanSubscriberAre you saying a Contact Tool evaluated this contact as Closed before you increased the pinball radius? nOr did you just miss that this contact was Open and increasing the pinball radius made it Closed?nSeptember 29, 2020 at 6:23 amValiullinDamirSubscriberAs i remember, all the Contacts before were closed.nThen i increased pinball radius, and now i have such a situation:nManually detected contacts are orange. They have small ammount of penetration, but i think, that this approximation can be done. nAnd as i understand now, the whole problem was with manually detected contacts - there are really small gaps at these zones, and because of these gaps contacts were not created automatically. nViewing 8 reply threads
- 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
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- 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.