July 16, 2020 at 11:13 pmjuhuang7Subscriber
I wasn't sure if I should start a new post or continue this discussion but I'm having the same issue again with a different snap-fit. I've tried moving the part until it just touches the contact but I'm still experiencing the 'inactive' status. As a result, it's not detecting the contact between the 2 parts. I've attached my archived project here. Here are some pictures of my contacts and settings.
July 17, 2020 at 12:00 pmpeteroznewmanSubscriber
I recommend putting a small radius on the tip of the snap that has the 45 degree sharp point and the same small radius on the 90 degree corner at the bottom of the lines in blue if you want to simulate the snap going around the corner.
Don't put any edges in the contact set that will never make contact such as the left and bottom red edges.
Finally, increase the pinball radius until you get closure.
It is better to start a New Discussion once you mark an old discussion with Is Solution. Also, shorter discussions are easier to read than long ones.
July 18, 2020 at 2:46 amjuhuang7Subscriber
Hi Peter, thanks for the recommendation.
No matter how big I make the pinball radius, the status keeps appearing as 'near open'. I'm not sure what to do from here. On another note. I keep receiving the following messages when I run my simulations:
- One or more objects may have lost some scoping attachments during the geometry update. You can identify these tree objects by filtering the tree using the Scoping option set to Partial.
- One or more bodies may be underconstrained and experiencing rigid body motion. Weak springs have been added to attain a solution. Refer to Troubleshooting in the Help System for more details.
- Contact status has experienced an abrupt change. Check results carefully for possible contact separation.
July 18, 2020 at 1:48 pmpeteroznewmanSubscriber
I just noticed the link to your project in your original post.
1) The two parts should be tangent. They are not. I moved them to be tangent and added the radius fillets recommended above.
2) You should do this as a 2D Plane Strain model. That requires the geometry to be in the XY plane, so I used SpaceClaim to move the surfaces to Z=0.
3) Change the 2D behavior to Plane Strain.
4) I only included the needed edges in the contact definition. I set the Normal Stiffness to a Factor of 0.1 which means a little more penetration in exchange for an easier contact convergence.
5) I added keyopt(6)=1 to the elements for mixed u-P formulation, which helps convergence in high pressure situations like the tip of the snap.
ANSYS 2020 R1 archive attached.
July 19, 2020 at 7:57 amjuhuang7Subscriber
Hi Peter, thanks for replying.
In which setting can I add 'keyopt(6)=1'?
July 20, 2020 at 5:33 pmpeteroznewmanSubscriber
Look under the Geometry category, under each surface body, there is a Command Object.
- 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 work with STL file?
- drawing a geometry by importing a table of points
- Using Symmetry in DesignModeler and Expanding the Results
- section plane
- material properties
- Rotate tool in ANSYS Design Modeler
- ANSYS FLUENT – Operation would result in non manifold bodies
- Parameters not imported into Workbench 18.2 from Solidworks/Inventor
- Geometry scaling
- Convert Surface body to solid
© 2022 Copyright ANSYS, Inc. All rights reserved.