December 3, 2019 at 11:58 pmishaniisSubscriber
I am unable to work through this error.
The geometry file has been duly attached in IGS format
December 4, 2019 at 1:00 ampeteroznewmanSubscriber
I opened the iges file and find a solid body that represents a tube with reinforcement at 24 stations around the tube.
This is an example of a structure that would best be converted to a midsurface model. You need the tube to be a separate solid to the reinforcement ribs. Extract a midsurface of the tube, and a midsurface of each reinforcement rib. Then you can mesh them and bond the reinforcement ribs to the tube.
December 4, 2019 at 1:14 amishaniisSubscriber
I am new to this, I could not follow this effectively.
Can you help me with the same changes ?
December 5, 2019 at 12:40 amparkersheafferSubscriber
Your model is a tube with ribs welded inside of it, if you convert this to a midsurface model not only will it resolve your meshing issues but your model size is going to be significantly less. Anytime you have a constant thickness part(plates,tubes,etc) you can model it as a surface. When this surface is imported into mechanical and meshed it will be equivalent in thickness to the solid body you created it from.
ANSYS provides a tool in spaceclaim and design modeler to quickly create midsurfaces and assign the thickness of the solid to them. Its convientently called "Midsurface" and you will find it under the prepare tab in spaceclaim.
As i mentioned before you will need a constant thickness to correctly midsurface a part, your model in its current state does not have this so you will have to split the ribs from the tube. There are many ways to split the ribs from the tube, the method I used was creating a solid cylinder with the length and inner diameter equal to the tube and using the tool "combine" to split the bodies apart.
Due to the curvature of the tube your ribs cant be directly midsurfaced as the thickness isn't a constant 2mm anymore. These will need to be modified to midsurface. If you want you can leave the ribs as solid because it requires modifying the geometry a bit. If you choose to modify the ribs its important when you create the midsurfaces for the ribs that you select the same top(shown in blue) and bottom faces(in green) for each rib otherwise when you setup contacts you will have issues.
If you do not misurface them this does not apply.
When you import these surfaces(or surface and solids) into mechanical you will need to setup a contact to attach the ribs to the tube. To do this insert 1 bonded contact(delete any contacts automatically generated) select the tube as the target and the 48 faces of the ribs as the contact. In the window if the colored faces are not facing the each other you will need to reverse the shell face of one of the bodies, then turn on shell thickness effect.
Hopefully that helps explain the process a bit further. I have the cleaned up models if you need them but i think it might be useful to try it first yourself.
December 5, 2019 at 1:59 ampeteroznewmanSubscriber
Welcome to the Community parkersheaffer! That is a very good and detailed explanation. I hope ishaniis can follow it.
December 6, 2019 at 9:16 pmparkersheafferSubscriber
Thanks! I have used this as a resource for a while and figured I could contribute a little while i'm not busy.
- 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.
- how to improve the inflation quality at sharp corners?
- ANSYS Workbench Measuring within Design
- check element type
- The mesh file exporter could not resolve cyclic dependencies in overlapping contact regions error
- Meshing Error
- Error in meshing
- Conformal vs Non-Conformal Mesh
- execution error inside the mesher. The process suffered an unhandled exception or ran out of memory
- How to resolve Mesh Failure
- inflation created stairstep mesh at some location
© 2023 Copyright ANSYS, Inc. All rights reserved.