May 19, 2021 at 7:42 amChinmaySubscriber
Hi all, greetings.
Here is the initial and final position of my simulation.
Initial:May 19, 2021 at 8:23 amErik KostsonAnsys EmployeeHello
Suppose one way is to apply your air pressure on the component and ramp it up to see when you lose contact completely so your contact is not on and hence your contact pressure is 0 (means the seal is not touching the face anymore).
All the best
May 19, 2021 at 12:52 pmpeteroznewmanSubscriber@chimay
Note that you will have to split the face on the seal at the line where the contact is closed. The contact pressure in psi is plotted below, the transition from grey to color is at 20 psi and the peak pressure is 88 psi, so we can expect that the seal will fail somewhere between 20 and 80 psi.
You would need to split the face at the contour line between grey and blue. That way, you would put a test pressure of say 50 psi on the faces that are above that contour line, and there would be no pressure on faces below that contour line. Solve the model and check how much the 50 psi contour line moved relative to the split line.
May 20, 2021 at 4:21 amChinmaySubscriberThank you for your reply but I am quite new (only few months of experience in Ansys Structural) to Ansys WB. Thus I am really not sure how to perform those activities you guys mentioned. I will look up other resources available and try few ideas on my own.
Btw if the maximum value is 88 Psi or 0.6 MPa for contact pressure, does it mean it will need equal and opposite force to break the contact ? So basically we need to apply pressure on face of seal to bring that value to zero ?
Thank you Chinmay
May 20, 2021 at 1:09 pmpeteroznewmanSubscriberWhile the maximum pressure on the seal is 88 psi, that is only in the corner. On the side, the pressure drops to about 70 psi (light orange color). The seal fails when the lowest value around the perimeter fails. There is a natural split line on the geometry, so simply choose all the faces above that to apply a pressure.
Under analysis settings, make this a 2 step solution. In step 1, the pressure is 0 and the displacement of the center part ramps up to 5 mm in 1 second. In Step 2, the displacement stays at 5 mm and the pressure ramps up from 0 to 100 psi in 1 second.
I followed my own instructions and was interested to learn that the pressure actually helps the seal work better! Below is the pressure at 76 psi (time = 1.76) and you can see the peak contact pressure is now 170 psi because the pressure is pushing down on the top of the seal, which causes it to compress against the bottom and expand sideways making the contact pressure increase.
May 21, 2021 at 4:34 amChinmaySubscriberYou are absolutely right and the solution is correct based on given inputs. My bad I didn't mention the exact parameters of the seal and the pressure direction.
The air flows from the direction shown and applied a 2 bar or 0.2 MPa or 29 psi pressure on highlighted faces, probably pushing seal in right direction (if it is sufficient to overcome friction between seal and other bodies).
But as you correctly mentioned above, this pressure is going to increase the contact pressure between seal and other bodies at the seal lip, so doesn't this mean that there is less chance of failure (air escaping through seal) now ?
May 22, 2021 at 4:18 pmpeteroznewmanSubscriberYes, pressure improves the seal, if there is an initial seal.
One type of failure is if there is a gap after assembly. The air will flow through the gap and the pressure will open the gap.
Viewing 6 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.