June 2, 2020 at 5:58 pmVijay332Subscriber
I am trying to simulate an analysis where i have a composite part form ACP and a rigid body form mechanical going into static structural. But I am having issues of adding any contacts between the two bodies.
Can i combine composite part form ACP and a rigid body form Mechanical??
June 4, 2020 at 7:11 amAniketAnsys Employee
should be doable.
assemble the model as follows:
So when you define contact between rigid body and system C, it will prompt for a remesh there. Remesh it there and you should be good to go.
Please note rigid body must be in the target.
for more info:
How to access Ansys Online Help Document
How to show full resolution image
Guidelines on the Student Community
How to use Google to search within Ansys Student Community
March 30, 2021 at 1:16 pmrahmanmahfuz11SubscriberHello Aniket and Vijay,I have run into a similar problem. When I open the assembly model having both the composite and rigid body it prompts an error Rigid bodies scoped to contacts will require remeshing to solve successfully, but cannot be meshed because meshing is blocked. and when I press the meshing update or generate button this info pops The model cannot be remeshed. The imported mesh for this model has been resumed.. How can I overcome this problem?nThank younMahfuzn
March 30, 2021 at 11:23 pmBenjaminStarlingSubscribernWhen assembling models the mesh, along with most other objects, is set to read only. This is what is preventing remeshing, but there are other consequences that need to be considered. I have not attempted this myself, so I can not give a definitive answer, but one of the following should work.nIn the assembled system, set the mesh -> read only property to NO, then try scoping the contact. My concern is that this will then try to mesh or alter the Composite bodies.nPlace a dummy body in the sub assembly system where the rigid bodies are. If it is easy enough, use the same geometry that forms your composite part. In this system apply the contact as you would like it to exist in the assembled system. Then in the assembled system, set the read only property on the contact to NO, and scope the composite body, where the dummy body is currently being used. Suppress the dummy body.nInclude the non composite rigid body in the ACP system. I am not familiar with ACP but I would imagine if no layup is defined on the body, it won't transfer the data to Mechanical. But this seems easy enough to give it a shot.nlet me know how you go.n
March 31, 2021 at 12:32 pmrahmanmahfuz11SubscriberArraynHi Benjamin, thanks for the reply. setting up read-only property to No, the first error Rigid bodies scoped to contacts will require remeshing to solve successfully, but cannot be meshed because meshing is blocked. goes away. However, when I set up the contact and want to update the mesh this error (The model cannot be remeshed. The imported mesh for this model has been resumed.) keeps popping up. Would you please tell me what may I be doing wrong? Thank you.nRemeshing is always required in rigid bodies after their contact parameters have been updated. So, there's no way around it.n
April 1, 2021 at 1:10 amBenjaminStarlingSubscribernI was able to do this on a dummy model, changing the contact scoping, and suppressing the unwanted body. Are you able to attach an archive of your project here so I can check if this is possible.n
April 15, 2021 at 6:59 amrahmanmahfuz11Subscriber@BenjaminStarlingnnSorry for the late reply. I had a deadline. So, I had to find alternative ways to solve this. What I did this is I added another 2mm coating layer around the composite layer. So now the contacts were between coating layer & the rigid bodies not with composite & rigid bodies. So, it was doable as the solid coating layer wasn't coming from ACP. nHowever, I believe this is a hack and not a solution, also in some models one might not have a coating layer. But ANSYS forum was locked from April 5 till now, so I couldn't reply.nI am attaching the original file (without the coating layer) of the set up. I feel like it's better to give a brief description about the project. So, I have a tube of polyethylene with 4mm thickness with a 2mm helical hole inside it. Outside the polyethylene layer is my solid composite layer. I am trying simulate rolling of the tube with three rollers. I have modeled the composite layers in ACP and the rest in Mechanical Model.nWhen you open the project there might be a prompt for missing files. Just ignore it. I had to force delete some files those were not part of the project. The prompt is about those. n
April 16, 2021 at 7:04 amrahmanmahfuz11SubscriberArray nThe mentioning feature wasn't working then.n
April 19, 2021 at 11:07 pmBenjaminStarlingSubscribernGood to see you found a solution. This is in general a limitation or oversight with the way mechanical handles assembled models. Composites do not form a considerable part of my work, so this is the first example that has really highlighted this issue with the ACP workflow, that you are essentially forced straight into using an assembly system. This issue arises with other models also, but the solution most of the time is to model as much as possible before assembly. In future releases the assembly workflow should become a bit more flexible, allowing users to add/modify geometry and meshes a bit more freely. (fingers crossed)nHaving looked at your model though another solution may also have been to mesh the rollers coarsely, then use contact geometry correction to ensure the contact behaved as a perfect cylinder.nn
April 20, 2021 at 4:25 pmrahmanmahfuz11SubscriberHelloArray,nYes, I am also keeping my finger crossed on assembly workflow being flexible in future releases. nAnother thing, Having looked at your model though another solution may also have been to mesh the rollers coarsely, then use contact geometry correction to ensure the contact behaved as a perfect cylinder. - I haven't been able to clearly understand what you meant by that. Have you meant not defining the cylinders as rigid bodies & use contact geometry correction to ensure that they behave as rigid bodies although they have been defined as deformable?n
April 22, 2021 at 1:29 amBenjaminStarlingSubscriberArraynThe bodies will remain deformable, I would have just increased their young's modulus by 10x or 100x to ensure they are not deforming too much. The advantage of using a rigid body is that it allows the solver to only use the elements required for the contact (i.e. less elements). Other than this there is no advantage to using a rigid body in your analysis, or many other analyses. If we switch to using a deformable body, our solution time may suffer, or even preprocessing time to split bodies and mesh etc., if we use an appropriately sized/fine mesh. Because we know we are not interested in results on the rollers for your analysis, we can then decide to mesh coarsely, to save pre processing time and solution time, but this will effect the contact accuracy and possibly even convergence. Contact geometry correction allows the user to specify a cylindrical surface through a coordinate system and radius which helps smooth the contact across the discretised mesh.nIn both instances, rigid or deformable, contact geometry correction could have been utilised, as even the rigid body requires the contact elements to be created, however the rigid body can have the contact elements meshed much finer than the deformable body.n
April 22, 2021 at 7:13 amrahmanmahfuz11SubscribernGot it.nMy main purpose for defining rigid body was to decrease mesh size & thus solving time. I'll look into the contact geometry correction.nAnyway, thank you for your replies.n
- 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.
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- 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
- whether have the difference between using contact and target bodies
- User manual
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Colors and Mesh Display
- material damping and modal analysis
© 2023 Copyright ANSYS, Inc. All rights reserved.