# SnapFit Non-linear analysis Force Convergence Issue

AkashVyas
Delhi, IndiaMember

in Structures

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

## Comments

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.

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.

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

What are the goals of your analysis?

What questions do you want the simulation to answer?

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?

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

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.

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

this time Input displacement is 6.8mm last time it was 8.2mm

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

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.

Yes, I also need that part, how to solve that part

Should I solve that separately

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).

Okay, I will try again