SnapFit Non-linear analysis Force Convergence Issue

  • 78 Views
  • Last Post 27 March 2020
AkashVyas posted this 23 March 2020

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

Displacement

 

these are my analysis and contact setting

analysis setting               contact setting

and if I'm reducing the no of load steps or substeps it's not even converging till this point

 

Order By: Standard | Newest | Votes
peteroznewman posted this 24 March 2020

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.

AkashVyas posted this 24 March 2020

What stabilization settings should be used constant or reduce

peteroznewman posted this 24 March 2020

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.

AkashVyas posted this 25 March 2020

new results

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

force convergence graph

peteroznewman posted this 25 March 2020

What are the goals of your analysis?

What questions do you want the simulation to answer?

AkashVyas posted this 26 March 2020

I have to find the mating force

peteroznewman posted this 26 March 2020

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?

AkashVyas posted this 26 March 2020

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

peteroznewman posted this 26 March 2020

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.

AkashVyas posted this 26 March 2020

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

 

AkashVyas posted this 26 March 2020

applied forcefrictional contact force

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

AkashVyas posted this 27 March 2020

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

peteroznewman posted this 27 March 2020

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.

AkashVyas posted this 27 March 2020

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

Should I solve that separately

peteroznewman posted this 27 March 2020

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

NEQIT,100

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).

AkashVyas posted this 27 March 2020

Okay, I will try again

Close