April 9, 2020 at 2:48 pmusman786Subscriber
I am trying to simulate a rubber bellow using the VMQ silicone hyperelastic material. The bellow is deformed in the x-direction by 16 mm. I am trying to solve this problem in the static structural using the implicit solver. However no matter what I do, I always run into convergence problems after passing approx. 8 mm travel in x-direction. I also activated the Nonlinear Adaptive Region with 10 loops and removed the cyclic symmetrie, which I had before. Since activating the Nonlinear Adaptive Region I get the following Error:
The result cannot be evaluated because it has (1) an invalid scoping on a body with a changing mesh or (2) an invalid scoping when the result file is the mesh source. Body scoping is required for the result.
I know, explicit dynamics with this kind of large nonlinearity is the way to go, but as I am simulation multiple geometry variants, the explicit solver will be too time-consuming. Can you guys please help me out?
April 9, 2020 at 5:45 pmpeteroznewmanSubscriber
ANSYS staff are not permitted to open attachments, so you should use the Insert Image button to put the image into the post as well as attach them.
I recommend you use an Axisymmetric model if you want fast solution times.
Go back to CAD, reorient the solid body so that the axis of rotation is along the global Y axis. Slice the body in the XY plane and the YZ plane so you have 4 solids. Delete 3 of the 4 solids and keep one that is on the +X side of the Y axis. Make a surface body on the face in the XY plane and delete the solid body. Now you will have a single surface body that is a radial slice in the XY plane of the bellows.
In Workbench, drag out a new Static Structural model. You can drag the Engineering data from the first Static Structural to the Engineering Data on this new one. Click on the Geometry cell of this new block. In the Properties, change the Analysis Type from 3D to 2D. Import the geometry into the Geometry cell. Start Mechanical.
In Mechanical, click on the Geometry and set it to Axisymmetric. Now you can put your fixed support on the bottom edge and your displacement on the top edge. You can apply the same contact conditions, only now they are on edges instead of faces.
This geometry will have a much better mesh and the solver will run a lot faster.
April 12, 2020 at 1:45 pmusman786Subscriber
thanks for you answer. I did what you've said and created a 2D axissymmetric model, but I am still facing convergance issues due to "highly distorted elements". And for some reason, the Nonlinear Adpative Region is not triggered. I have attached the archive file now, maybe you can have a look?
April 12, 2020 at 6:12 pmpeteroznewmanSubscriber
Don't use Nonlinear Adaptive Region. Do use good square quad elements.
Force the solver to take small time steps.
Use keyop(1)=1 and keyop(6)=1. Look that up in the Element Reference if you want to know what that means.
The solution has gone past the point where self intersection begins, so it is time to unsuppress the contacts that prevent that.
April 17, 2020 at 3:41 pmusman786Subscriber
so I followed your instructructions and activated the contacts using the settings shown in th figure below. But for some reason no matter what Lagrange formulation I use for the contacts I use, I always run into convergence problems. The most complete result (0,91s) was achieved when I set the contact behaviour to asymmetric with augmented Lagrange formulation using the programm controlled auto-time-stepper. Attached you will find the updated projekt-file. Maybe you can have look again peteroznewman? Thank you very much
April 17, 2020 at 6:22 pmpeteroznewmanSubscriber
Good try usman!
I tried for a while then converted the model to Explicit Dynamics, which has a very robust self-contact algorithm that worked on my first try.
Note that the solution is a dynamic solution, which means you will get different deformations depending on how fast you move down, but that to move 10 times slower will take 10 times longer to solve.
April 18, 2020 at 7:06 pmusman786Subscriber
so as you suggested I ran this simulation in Explicit Dynamics, but unfortunately the force over travel plot is not representative any more as the kinetic effects are to dominent now. The solver output of this run showed a time increment of 4.096E-09s.
In a second run I used the Quasi-Static preset and entered the mentioned time increment for the Minimum CFL Time step. The damping cofficent was set to 0.1. This resulted in this:
April 18, 2020 at 9:09 pmpeteroznewmanSubscriber
I suggest moving the load application point from the ID edge to the flat face of the top of the bellows (which is the left edge in the image above).
What did you use for a Boundary Condition? Please show a screen snapshot. Did you do a Step Change in Displacement of 16 mm and ran the simulation for 0.01 s? You need to ramp the displacement up from 0 to 16 mm over a long time, like 1 second. Note that ramping displacement causes a step change in velocity which creates some transients in the structure.
A smoother way to create the motion is to ramp the velocity of that top edge from zero up to some value at 0.5 s and then hold the velocity constant until time 1 s. Choose the velocity that results in 16 mm of displacement at 1 second. This motion and some damping in the material will greatly reduce the contribution of transients to the deformed shape in the structure at time 1 s.
April 21, 2020 at 10:05 pm
April 22, 2020 at 1:59 am
- 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
- whether have the difference between using contact and target bodies
- Colors and Mesh Display
- 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
© 2022 Copyright ANSYS, Inc. All rights reserved.