May 15, 2021 at 11:20 amChinmaySubscriber
Greetings of the Day.
I am doing a project where I wish to find out the seal compression and the contact pressure between seal and housings. Please find attached images for reference. I have used 2 plane symmetry thus only quadrant is shown below.
All except Seal have material as steel. Seal is Silicone rubber. Behavior of all parts is selected as flexible. No NLAD meshing used.May 15, 2021 at 1:21 pmpeteroznewmanSubscriberYou can save time waiting for the solution by changing all the steel parts to Rigid behavior.
Using Frictionless contact hurts the ability of the solver to converge and is unrealistic. You are better off using some small amount of friction. Very high friction is also difficult to converge.
Here is the solution with the plunger 5 mm down.
You were going for 7 mm of displacement, but nothing changes, except without friction, the seal wants to jump vertically.
Attached is a model that uses friction of 0.1
May 17, 2021 at 6:34 amChinmaySubscriberThank you for your valuable help, I have few follow-up queries for this:
1) I inserted pressure in contact tool as shown below, so my question is if this contact pressure is seal pressure (Amount of pressure required to overcome the sealing) ?
2) In your APDL commands, you added 'neqit, 100' ; I guess default is 25 ?
So how did you decide how many equilibrium steps you need to solve this particular problem ?
3) Can and should we use NLAD meshing for seals in general ?
4) In total deformation, I need complete seal deformation, thus I made changes in symmetry settings accordingly but unfortunately the result is not as expected.
and lastly 5) You added "nd001_MXUP_Elements" & "nd002_MXUP_Elements" in the solution information, I did not find this on any online resource available, could you please tell me what was the purpose for doing this and what conclusion do we get from it or how do we infer the result obtained in this step ?
Thank you and sorry for so many queries Chinmay
May 19, 2021 at 1:09 ampeteroznewmanSubscriber1) Pressure in the contact tool is contact pressure. That is the normal force of the seal pressing against the rigid part per unit area. That is not the air pressure that the seal would support before leaking. The question of how to determine the air pressure that a particular seal will support is worth its own separate discussion.
2) Yes, the default maximum iterations is 26. It doesn't hurt to put NEQIT, 100 into the model. If a substep converges in 7 iterations, it increments the load.
3) I never use NLAD. I have not found it necessary and I have not found it helpful.
4) I don't understand what you changed and what went wrong.
5) Click on the Solution Information Folder and see in the Details window the is a line to put in N-R Force Residual Plots and a line to put in Deformed Elements. When you put a non-zero number on this second line, Mechanical automatically creates a group of the Highly Distorted Elements found during the solution. If the elements get too highly distorted, the solution will stop with an error. Other times, the solver might bisect the increment and try again with smaller substeps and be able to keep going.
May 19, 2021 at 3:21 amChinmaySubscriberThank you for this wonderful explanation & solution and also spending you valuable time helping all of us here on this platform. You are awesome. :)
P.S. I will make a new discussion on "how to determine the air pressure that a particular seal will support" if there is none here or other internet sources.
Viewing 4 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
- 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
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.