June 22, 2018 at 2:27 pmFarhanSubscriber
I simulate (in shell) a pull out test with a silocone joint in between the frame and a bar. The silicone joint has E=0.8MPa and v=0.45. If i put tensile force higher than 200N at the end of the bar, the simulation stopped in the middle and I got an error of nonconverged results. This is normally because the joint in non linear deformation isn't?
What should I do to make sure the simulation continues till the end.
Thanks in advance.
June 22, 2018 at 4:12 pmpeteroznewmanSubscriber
In this model, I assume the green is silicone, the gray is the bar and the brown is the fixed frame.
Is this a 2D model? Are these three parts put into a Multibody part with Topology Sharing or is the Bonded Contact between the faces?
I expect that after 200 N is applied, the solver stops because one of the elements has become highly distorted and cannot continue.
You call this a pull out test, but if there is no damage law included in the material, there will be no tearing of the silicone.
June 25, 2018 at 7:51 amFarhanSubscriber
Yes, it's a 2D model with 40mm thick when viewing the results profile. The three elements have bonded contact in all sides.
Yup, after a certain time the solver stops and I can see the joint becomes distorted. So, what can I do in Ansys to put damage law for the silicone joint to simulate the tearing?
June 25, 2018 at 8:10 amFarhanSubscriber
I learned that we can put Mullins effect to simulate the damage on hyperelastic material like the silicone. What is material constant R, M and B?
June 25, 2018 at 9:27 pmsk_cheahSubscriber
An approach is perhaps to use CZM to capture the fracture between the silicone and frame/bar?
June 29, 2018 at 1:29 amBhargava SistaAnsys Employee
What is the end goal of your simulation? Are you trying to calculate the max. force required to pull the silicone joint out? If that is the case, then you may want to apply a displacement boundary condition and calculate the reaction force on it to answer your question.
Now coming to a bigger question, how is the silicone joint held inside? You defined a bonded contact between them but in reality is it glued to it or is it similar to a push pin where the friction is holding them together?
- If this is a press-fit assembly, then you don't need any failure models. You'll need to start by solving for interference fit first so that contact pressure is developed and friction will be sufficient to hold them together. Then in the second step, you can apply the displacement and measure the force required to remove the silicone joint.
- If there is a glue, then cohesive zone material modeling is the way to go. You'll need the max. shear bond strength of the glue and the max. distance at which it fails. I'd recommend you read about it in the help documentation to gain insight.
- If you want to model the failure of silicone, then Mullins effect is not the way forward. You'll need to use explicit solve (Explicit STR or ANSYS LS DYNA) and turn on element erosion so the elements are deleted when they meet a user-defined criteria (e.g., max. strain).
Also, if you're reducing it to a 2-D model make sure that you're using the appropriate 2-D behavior. For instance, 2-D axisymmetric would not be suitable for what you're doing, plane strain is probably what you want.
June 29, 2018 at 8:07 amFarhanSubscriber
My objective is to find suitable contact parameters frame-bar with adding silicone joint in between for a full scale prototype. So I did this simple pull-out test to compare it with my experiment result (force-displacement of bar).
The silicone joint is acted as glue between frame and bar so I did put bonded contact for both frame-silicone and bar-silicone contact. So, if I define CZM on silicone, are the bonded contacts became redundant? The Mullins effect is used in this simulation to add stress-softening on the hyperelastic material like silicone.
For the next step, I would like to make force push downwards at the end of the bar to simulate small sliding of the bar from the frame (if there is), do I need to change the contact parameters to simulate the real problem or the contact remains the same?
June 29, 2018 at 6:32 pmBhargava SistaAnsys Employee
OK, sounds like CZM is the way forward for you. CZM is used for defining a breakable bonded contact so you still need the bonded contact. When the bond strength as defined in CZM is reached, the bonded contact will break and act as a frictional/frictionless contact. Also, in CZM you don't create a geometry for the glue, it is modeled as either contact or interface elements. For your application, you may use debonding which uses the contact elements. Check out these sections in the documentation for further reading:
Regarding the Mullins effect, as you've stated, the damage is accounted for by softening the material. So, if you continue to pull the part, its elements will simply stretch out and eventually distort instead of rupturing. This will give you element distortion errors. If you wish to use Mullins effect for this case, you'll need to use explicit solver where you can use element erosion option to delete the elements that have sustained max. damage.
July 2, 2018 at 10:00 amAshish KhemkaAnsys Employee
Just a note: We don't support 2D models now for WB Ls-Dyna.
- 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.
- 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.