February 13, 2020 at 1:19 amjoestabileSubscriber
Am I understanding all the posts correctly in that if you want to model a fluid contained within a structure you have to use APDL code to add the Hydrostatic 242 elements? And is the fluid then NOT a geometric part?
February 13, 2020 at 4:00 ampeteroznewmanSubscriber
What do you mean the fluid is not a geometric part?
The fluid cavity has a volume, and that volume is filled with a geometric solid body so that the fluid can be meshed. In that sense it is a geometric part.
During the solution, the fluid creates a uniform pressure field on the walls of the structural parts it is touching.
February 13, 2020 at 9:06 pmjoestabileSubscriber
Pete I am using Workbench. I have created a model with the fluid as a separate body. Basically trying to model a fluid filled rubber bladder. Made the walls of the bladder a rubber material. What kind of analysis do I drag onto the project page? Static structural? Static Acoustics? Do I have to include APDL code? Can you point me to an example?
February 15, 2020 at 1:39 amjoestabileSubscriber
Pete I used a static acoustic module to model a fluid filled flexible bladder. I used static acoustic because it has an fsi. Please see the archive sample problem below and see if it makes sense.
Many thanks for your time and comments.
February 15, 2020 at 4:23 ampeteroznewmanSubscriber
Very interesting Joe, good try. I never used static acoustics with a liquid. The times I have used acoustics regions, it was to compute sound waves traveling through air. The thing about acoustic medium is it is compressible, which is required for sound waves to travel through it.
I think you want a nearly incompressible fluid in the bladder, since you named the fluid material Glycerin. But it has acoustic properties of density and speed of sound, not elastic properties like Young's modulus and Poisson's Ratio. Since the element used in your model is for acoustic purposes, it is not giving the correct response for large deflection structural analysis.
I created an elastic solid for water in this discussion. At the time I did this model, I did not know about element type 242. You should try that. Or better yet, you should build an axisymmetric model and use element type 241.
One improvement would be get at least two elements through the wall thickness. That requires slicing the bladder into 3 pieces, the flat base, the side wall, and the ring of material between the flat base and the side wall. Once those are separate pieces, each can have a sweep mesh control to force 2 hex elements through the thickness.
I used shared topology between the fluid and the bladder and the cap and for the sliced bladder pieces, so bonded contact was completely eliminated from the model.
I used 2 planes of symmetry to cut down on the node count to keep it under the Student limit.
Incompressible fluid is going to put pressure on the bladder to deform the wall as the cap moves down to maintain the constant volume of the liquid. I don't think that was maintained in your acoustic model.
Incompressible material like the water and the silicone rubber in this model are very difficult to get to converge. The water filled model failed to converge after only a few increments.
I made a copy of the model and suppressed the water to show what the deformation looks like with no water. That converged with no issue, but the internal volume is much reduced. Compare this deformed shape with the one from your model.
An ANSYS 2019 R2 archive is attached for you to examine this in more detail. Note that there is no results file in this archive. That means you have to Clear Generated Data on the Solution and Solve to create your own results file (which is very large).
February 15, 2020 at 5:12 ampeteroznewmanSubscriber
One more suggestion, on the 1/4 model, delete the Fixed Support and replace it with a Displacement and set Y = 0 but leave X and Z Free. That will allow the base to stretch as the cap gets pushed down, simulating the bladder being on a frictionless surface. Note: you can't do this on your full model because it won't solve since you don't have symmetry planes keeping it in one place on the frictionless surface.
I also changed the Cap displacement from -5 to -1 mm and it is makes is a bit further, but still fails to go the distance before stopping with a highly distorted element error. I need three layers in the bottom, but have run out of elements to stay under the Student limit.
February 16, 2020 at 2:53 ampeteroznewmanSubscriber
I suggest you take the faces in the XY plane and use them in an axisymmetric 2D model. It will be so much faster to solve. You can also use HSFLD241 for the fluid volume. It might solve more easily than the elastic nearly incompressible solid that I hacked to be "water".
Here is what it is going to look like. In Workbench, I created a Remote Point at (0, connected to the inside walls. The remote point would be the Q node of the HSFLD241 elements that monitor the pressure inside. The red lines would be replaced with actual HSFLD241 elements. I think you have to use the ESURF command to make the elements. I don't yet know how to do that.
I hope this approach converges much more easily that the hack I did with the "water" above. I have an updated archive at the 2019 R2 release.
February 18, 2020 at 3:02 pmjoestabileSubscriber
So lets separate the problem into two regimes. One: What is the correct way to model a fluid or gas within an enclosed flexible structural volume?
Two: What is the best way to build the model to enhance convergence.
I am still struggling with what is the correct way to model the fluid or gas within a flexible structural volume.
February 18, 2020 at 4:06 pmpeteroznewmanSubscriber
It depends on what you want the fluid to do. If you don't need any flow, and the useful property of the fluid is the ability to share pressure throughout the fully enclosed volume, and provide a compressibility property, then HSFLD241 for 2D and HSFLD242 for 3D are what you want.
Please read Chapter 15 in the ANSYS Help. Here are the instructions for using the URL below.
February 19, 2020 at 2:09 amjoestabileSubscriber
So just wondering if there is a tutorial on how to execute the material in Chap 15 using mechanical interface or must we use apdl code in the mechanical interface.
Are there any examples you can point me to? (using the mechancal interface)
February 19, 2020 at 4:12 ampeteroznewmanSubscriber
I haven't used HSFLD elements before, but I expect you would use a Command object in Mechanical to create them with a few lines of APDL code. I don't have any examples of that other than the example in the ANSYS Help shown above.
You can use an orthotropic material with the properties of water, as shown above, without needing any APDL code.
February 21, 2020 at 2:41 pmjoestabileSubscriber
Will spend the weekend trying to do a hydrostatic in workbench. I understand apdl, just have not used it in the past 20 years...but old habits die hard...
Found a good example here: https://www.simutechgroup.com/tips-and-tricks/fea-articles/158-fea-tips-tricks-ansys-hsfld242-elements
February 24, 2020 at 7:44 pmpeteroznewmanSubscriber
Good find Joe! I am interested in seeing this work myself.
September 14, 2020 at 8:39 pmMontassarSubscriberHi,nMy current project is quite similar to your model, but additional complexities prevent me from implementing it using the APDL environment. So I wonder if you have successfully used Workbench. nI found this link, it might be useful in some way.nThank you in advance,n
- 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.
- 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.
- What is the difference between bonded contact region and fixed joint
- Massive amount of memory (RAM) required for solve
© 2022 Copyright ANSYS, Inc. All rights reserved.