April 1, 2018 at 1:46 pmtrayCSubscriber
I am basically trying to model two hyper-elastic bodies, a ball squeezing out of a cylinder. But I keep getting an error which states that a solution could not be found at some points in my model.
I was wondering if anyone had any tips regarding how to solve this issue?
I already changed my settings to have large deflection turned on.
April 1, 2018 at 5:16 pmpeteroznewmanSubscriber
Is this a multi-step Static Structural model?
Is the ball inside the cylinder at the beginning and contact resolves the initial penetration?
How are you getting the ball to move to the end of the cylinder?
There comes a time when the force the cylinder exerts on the ball propels the ball dynamically out of the cylinder.
You can see that in a Transient Structural model, but there is no static equilibrium past that time.
I can be more helpful if you attach your project archive to your reply. Use File, Archive... to create a .wbpz file that you can attach if it is < 120 MB.
April 3, 2018 at 12:26 pmtrayCSubscriber
Hi! thank you so much for replying
I am actually trying to model a very simplified version of the process of childbirth, whereas the "ball shape" in the middle is the baby and the cylinder outside is the uterus.
I am trying to squeeze the baby out by applying a pressure around the uterus. At the moment it is just one step - applying a single pressure to the mode but I keep getting the error " the solver engine was unable to converge on a solution for the nonlinear problem as constrained".
April 3, 2018 at 5:10 pmpeteroznewmanSubscriber
This sounds like an interesting and challenging model.
To get started, I recommend you attempt to get a 1/4 model running. By using two planes of symmetry, and one Y=0 Displacement BC on the flat face at the cervix, the model is fixed without using a fixed support. This will allow the cervix to dilate as the head moves forward.
I made those changes to your model, but I had to make two new revolves in DM to clean up the geometry for meshing. What CAD system are you using?
You have initial interference between the baby and the uterus, so you want at least a 2 step solution. Step 1 has no pressure, and is used to resolve the interference in the contact. If that is successful, step 2 will apply pressure.
How much interference did you want to stretch the uterus? It is difficult to get the contact to resolve the large overlap, so another method is to create the geometry so the baby is just touching the uterus wall. A thermal expansion coefficient is included in the fetus material model so a temperature increase will "grow" the baby to the interference you wanted. Now this is a 3 step model. Step 1, resolve contact, Step 2, grow the baby using temperature, Step 3, apply Pressure.
You need a minimum of 3 elements through the thickness of the uterus wall. Are you limited to the Student license or do you have access to a Research license? It is a challenge to stay below the 32k limit of nodes+elements in the Student license. The attached ANSYS 18.2 archive model does that and is able to move the baby along by pressure for some distance before failing to converge.
Why does it fail to converge?
Newton-Raphson Residual plots are saved to show why the solver could not find an equilibrium beyond this load increment.
This plot shows where a mesh refinement will help the solver to converge. Below is a finer mesh that was able to converge on the next pressure level.
Unfortunately, we are already at the limit for the Student license. The next step is to take this model to a fully axisymmetric model and use a 2D slice to represent the 3D object. The 2D bodies have to be around the Y axis for this type of model and you have to select 2D on the Geometry properties before you start drawing. Unless you are on a Research license, then you can stay in 3D.
April 5, 2018 at 1:58 amtrayCSubscriber
Hello! Answering your questions
What CAD system are you using? SolidWorks 2016 x64 edition
How much interference did you want to stretch the uterus? just enough to allow the passage of the baby
Are you limited to the Student license or do you have access to a Research license? I have a research license but only with Ansys 18.0
I shall follow your advice and try to perform the next few steps of creating axisymmetric model and increase mesh density !
- 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.