March 23, 2020 at 8:53 pmAkashVyasSubscriber
I was trying to solve this snap-fit problem but I'm getting these msgs every time ever time, I'm not sure what is the issue
The material for snap is polycarbonate and for the block it's steel
these are my analysis and contact setting
and if I'm reducing the no of load steps or substeps it's not even converging till this point
March 24, 2020 at 1:08 ampeteroznewmanSubscriber
It might be that convergence was easy up to this point, and now much, much smaller steps are needed to show equilibrium as the snap moves around that corner.Try to add Stabilization in the Nonlinear Controls under Analysis Settings. Also try much smaller elements around each corner.
Another suggestion is to treat this as a dynamic event and simulate this using Transient Structural.
Either way, it is going to take a long time to simulate.
March 24, 2020 at 2:49 pmAkashVyasSubscriberWhat stabilization settings should be used constant or reduce
March 24, 2020 at 5:11 pmpeteroznewmanSubscriber
Try Reduce, but use more elements around each corner first, and use smaller time steps at the point in the simulation when the corners start to slide on each other.
March 25, 2020 at 7:23 pmAkashVyasSubscriber
sir, I have solved this problem with fine mesh and stabilization and also I have given 35 loadsteps this time for the same dispalcement last time it was 20 loadsteps. but still same issue
last time node count was 10525 and element count was 3301
and this time node count is 39903 and element count is 12757
this is the force convergence graph
March 25, 2020 at 7:38 pmpeteroznewmanSubscriber
What are the goals of your analysis?
What questions do you want the simulation to answer?
March 26, 2020 at 3:04 amAkashVyasSubscriberI have to find the mating force
March 26, 2020 at 3:21 ampeteroznewmanSubscriber
Plot the data so far...
Don't you have the mating force already?
Isn't the convergence problem when there is a pull in force after the resistance to mating is over?
March 26, 2020 at 4:44 amAkashVyasSubscriber
I have the mating force, I just wanted to compare the FE generated force and hand calc force. This is just for practice
Sorry I don't understand what do mean "Isn't the convergence problem when there is a pull in force after the resistance to mating is over?"
Will it be okay if I plot the force till this point
March 26, 2020 at 1:48 pmpeteroznewmanSubscriber
Yes, you can plot the results up to the point when the convergence failed. All the data is valid except for the last point that it adds "for debug purposes".
Please reply with the plot of Reaction Force Probe on the insertion.
March 26, 2020 at 4:37 pmAkashVyasSubscriber
I'm using probe tool to plot force but It's not active/ working maybe because this problem is not solved completely
also, that file got corrupted so I'm again doing the simulation with less displacement till the point its converging
March 26, 2020 at 4:59 pm
March 27, 2020 at 4:37 amAkashVyasSubscriber
Is it possible to reduce the computation time and also file size
It Took more than an hour to solve also file is quite large almost 4GB, I thought plain stress problem will take much less computational time and space then solid model
March 27, 2020 at 6:06 pmpeteroznewmanSubscriber
Okay, you have your insertion force graph.
Do you need the part where the snap goes around the corner and the force reverses from pushing to being pulled in as the snap closes?
Yes, it takes time to solve. Yes, it will take longer to solve a 3D model than a 2D plane stress model.
March 27, 2020 at 6:10 pmAkashVyasSubscriber
Yes, I also need that part, how to solve that part
Should I solve that separately
March 27, 2020 at 6:18 pmpeteroznewmanSubscriber
Just continue the same analysis for another few hours. When convergence fails, take more substeps and make the elements smaller as necessary to continue convergence.
There are lots of tweaks that can be done on the Frictional Contact Details to help it out. You also should put in the Command Object
This will tell the solver to keep trying for 100 iterations before doing a bisection. Without that it will bisect in 26 iterations or less.
You are waiting longer than necessary by using small elements along the entire boundary. You only need small elements where the contact is occurring. Use large elements everywhere else.
You can also change the square to be a rigid part, then you won't get a mesh on the interior, only on the surface, but you have to use a joint to keep it fixed (or moving as the case may be).
March 27, 2020 at 6:25 pmAkashVyasSubscriber
Okay, I will try again
- 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.