May 25, 2022 at 9:00 amhenriquegpoSubscriberHello everyone I am trying to simulate the following situation using Static Structural: an Aluminum box inside of which there will be vacuum, sealed by a Aluminum lid screwed directly to the box with a Viton O-ring in between. The goal is to determine if the seal will work after pumping the air out of the box (my reviewers said that the box wall may not properly support the external pressure and asked me to demonstrate it via FEA).
Note: this is my first hyperelastic simulation and I do not have background on it, so I may be making rookies mistake here.
My first simplified approach was a 2 steps simulation. Starting point is the undeformed state in which the o-ring has a frictional contact with it's slot (in the box) and also with the lid bottom surface. Then first step was for applying a force pushing the lid down, and second step applying 1 atm on the external surfaces of everything. Fixed support on the bottom of the box. That did not converge, and I guess that must be several conceptual mistakes here. I would appreciatte any comments on why it does not work.
Trying to workaround things, I tried a second approach: instead of applying a force in the first step, I set up a displacement for the lid equals to the gap between the lid and the box. Kept applying pressure in the second step. That did converge, so I started refining it to a more realistic situation.
I extended it to a 3 steps simulation: first step with lid displacement only, second step with a force on top of the lid and third step for applying pressure (lid displacement deactivated at this step). Also converged.
Finally, I replaced the force for bolt pretension (using beam connections) loaded at the second step and locked at the third step. This also converged, and apparently to the desired solution: the box supports the external pressure. The problem is that I am not sure if the strategy used for setting up the simulation is correct or if it has conceptual flaws that invalidates the results.
So I would like to ask the community what are your impressions on that and is this set up correctly? Is there a better way to relate the bolt pretension with the lid displacement towards the box without needing to explicitly define this displacement in a previous step?
I attach some pictures of the geometry and I would be glad to share the Archive of this simulation in case you find it useful.
Thank you very much for the support and I am looking forward to hearing from you!
May 26, 2022 at 2:40 pmJohn DoyleAnsys EmployeeThe progression you are going thru to achieve a converged solution makes perfect sense.
Can you get this to solve with bolt pretension only in a two load step solution (LS1=bolt load, LS2=lock bolt load).
If bolt pretension in LS1 fails to converge, you could replace it with an initial adjustment (to establish contacts) at LS1, followed by a bolt preload (LS2), and then lock (LS3).
The bolt pretension approach is probably the most accurate, since it gives the best representation of the system stiffness (assuming all your other inputs are correct) and likely represents how you would assemble the physical parts together. A displacement based load applied to top of entire plate, even if it converges, is artificial and likely too stiff.
The only other suggestion I would make is to re-run with a finer mesh to make sure your critical results are mesh independent.
If your converged simulation results can be validated against any physical test data you have, I would say you are on the right track. ƒæì
May 31, 2022 at 7:43 amhenriquegpoSubscriber
Thank you very much for the answer and feedback. And I am sorry for the late reply, I was trying a few different things before reaching you and the community again.
I tried re-setting the simulation as you suggested. Initially, I simply suppressed the Displacement from LS1 making it an "empty step", and it converged.
Then I removed this step and did a 2-steps simulation: LS1=bolt load, LS2=bolt lock and pressure. That did not converge and right in the beginning I received this error message: "An internal solution magnitude limit was exceeded", pointing out to the UZ DOF of one node to which the beam connection is remotely attached. Searching this forum, I've seen that this error is quite common when there are small gaps between surfaces with frictional contact. I worked around this problem changing the interface treatment of the frictional contacts to Adjust to Touch, although I am not entirely sure if this represents the problem correctly, as it starts from a point where it considers that the seal is already touching the slot's lateral faces.
So the first thing I would like to ask is: what is the best way to deal with such type of contact (surfaces that are not initially touching, but will touch during the simulation)? The way I set in my simulation is a frictional contact having the whole seal surface as 'contact' and the 3 slot surfaces as 'target'.
And moving on to your other suggestion, I've also run the simulation with 3 steps, being the first one for bolt adjustment only, second for bolt load and third for bolt lock and pressure. That worked perfectly, without even the need to set the contact interface to Adjust to Touch (I just let the default setting "Add Offset, No Ramping"). The main difference I noticed between this two methods is that for the first one (2 load steps) I couldn't set bolt pretension to higher values such 200N, otherwise it wouldn't converge (highly distorted elements on seal). But for the second (3 load steps), that didn't seem to be a problem. I would not expect that behavior for such similar settings. Can you think of some reason why that is happening?
Finally, I guess I am also having problems with the material definition. Initially I tried defining an Elastomer Material using the Mooney-Rivlin 5 Parameter curve, but I couldn't manage to make the simulation converge with that material. Then I saw a tutorial in which the guy creates a new material based on Neo-Hookan, and manually input the two parameters needed. I did like that and then it started converging. One funny thing I noticed is that if I use the Mooney-Rivlin with ONLY displacement load steps, then it converges. But if I try using forces, then the elements become highly distorted and the simulation stops. Would have any comments on that?
I am sorry for such a long post, but a lot of different questions came up on this analysis.
Also I am not sure if this post should have been a question topic instead of a discussion topic. All the best Henrique
- 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
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Colors and Mesh Display
- User manual
- material damping and modal analysis
© 2023 Copyright ANSYS, Inc. All rights reserved.