January 10, 2023 at 6:20 amandy_pfuSubscriber
Hello Ansys Forum,
I need a little bit of help at my current project. I work in Ansys 2020 R1.
Short explanation of my model: My model is consists of two parts. Both parts are thin-walled tubes. I need to evaluate the stresses in this tube - but only the stresses in the lower part of the tube are necessary. Therefore the lower part of the tube is made out of volume elements and the upper part of the tube is defined with a surface (in spaceclaim - see picture 1).
Afterwards the surface get thickened in mechanical (see picture 2).
The upper part is defined as surface in order to reduce performance, to shorten the calculation time and to reduce the required storage space.
The problem is the connection between those two parts of the tube. In reality those two parts are one continuous tube. If I connect the two parts in spaceclaim via "share" (picture 3) the connection gets lost as soon as i change the geometry through parameters.
So I tried to connect the two parts in mechanical (see picture 4 and 5). The mesh has no shared points in this case but all objects are fixed and can not be moved.
When evaluating the results you can see there is a deformation there which should not be there (picture 6 and 7).
When I do the same model with only volume elements there is no such deformation (picture 8).
My question is now: How do I connect both parts (volume part and the surface) correctly?
I hope you can understand what I want to say otherwise I can try to explain it a little bit more.
Thanks in advance for everyone who tries to help me out! I would be really happy to solve this problem.
January 10, 2023 at 8:36 amErik KostsonAnsys Employee
I would say contact is one way (MPC type – face of solid body to adjacent edge of shell body – shell should be midsurfaced), or using a compatible mesh (nodes on edge are shared ) via multi-body part or shared topology. Make sure that the element order is quadratic (see below) so we use shell281 and solid186 with midside nodes otherwise we might not have a mid side node connection like you seem to have with progr. default order.
For stress accuracy at the connection, as far as I know there is no magic way to connect them (unless perhaps for very simple cases like pure bending or tension) so I would always place these solid-shell connections far away from the area of interest since the stresses at the connection will not be very accurate and correct, and we do not want them to influence the areas of interest (St Venants principle).
Also a better way is to use solid-shells (solsh190) to connect to 3D solid elements.
All the best
January 10, 2023 at 1:00 pmandy_pfuSubscriber
Hello Erik, thank you for your answer.
When I choose MPC type - I can only choose the edge of the solid body (the face doesnt work) and the edge of the surface and the shell is NOT midsurfaced. The surface of the upper part of the tube gets only thickened to the inside.
The element order is already quadratic.
Does the surface need to be midsurfaced for the midside node connection? Because in this project a midsurfaced shell which gets thickened to both sides is not possible.
Where can I find a compatible mesh, multi-body part and the shared topologie? In spaceclaim?
Would you recommend to just move the connection far away from the area of interest?
January 10, 2023 at 2:09 pmErik KostsonAnsys Employee
Good that it is quadratic so you use shell281 and solid186 higher order elements.
Does not have to be midsurfaced, especially if it is not possible.
As for shared topology in spaceclaim see (this will shared edges or faces and create a connected mesh between parts):
For multi-body part in design modeler search that on the internet (there are videos).
If it was me I would move this connection away from the area of interest.
All the best
- You must be logged in to reply to this topic.
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
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.