Stuck? 
support@mecway.com
support@mecway.com
Mecway
FEA
Impact but no visible stresses
I am simulating a project of impacting a ring to another ring(fixed) which signifies the action that happens in the barrel due to recoil. I took the load curve from a research paper and started to simulate in ccx. So here is the weird thing that happening. SO after impact there is no generation of stress and the most abnormal thing is that the movable ring penetrates into the fixed ring and it keeps on moving. CHeck out the gif to get the clear picture. Here all the files that may be needed by you. PLease tell me the reason for why this is happening.I am this close to losing all my hairs.
Howdy, Stranger!
It looks like you're new here. If you want to get involved, click one of these buttons!
Comments
Do you find there's no stress data in the .frd file or that it's too low? If too low, how different is it from what you expect?
You should be able to reduce penetration by increasing the contact stiffness (slope of pressure-overclosure curve) but beware that you can't eliminate it entirely and tuning this parameter is one of the tedious things about using contact.
What worries me more is the random looking displacements of the nodes around the contact. Maybe try 10 node quadratic elements instead? 4 node tets will give poor accuracy in many problems anyway so they're not something you'd usually use in a real analysis.
1)Where are the stress values in .frd files.I don't know which coloumn specifies what values
2)No matter how low i make the increment , the convergence is not reached.I made the mesh finer too and it took lot of time but at last it showed "Too many cutbacks"
3)I chose contact as "Linear no penetration" So is it normal that it shows the penetration
4)How to create a graph of force acting on the contact surface of the ring with time.
1) No need to look in the .frd file by hand. CGX and Mecway can both display stress. I don't remember a lot about CGX but they should be alongside displacement in a menu somewhere. You can also open the .frd file in Mecway - including the free version - and stress should appear in the outline tree if it exists in the .frd file. See attached picture.
2) That might be related to the weird distortions around the contact surface. I get a solution for a while, but it eventually fails too. I suppose the elements are becoming too badly distorted. My guess would be because they're linear instead of quadratic.
I just realised that the deformations are enormous. The rings are being crushed by a visible proportion of their thickness which is surely unrealistic and might be why it fails. Maybe there's a problem with the units?
3) Yes, linear is the most common kind of contact but it always has some penetration. Are you using a preprocessor that calls it no penetration? Maybe it really means "low penetration" and chooses a high contact stiffness to cause that. As far as I know, CCX doesn't have a truly no-penetration contact.
4) One way is to add external force as an output in *NODE FILE. That gives you force on each node. You have to sum them over one contact surface to get a single value at each point in time. I'm sure CGX must have a function to do that but I don't know how.
Another way is to output contact pressure (see CCX manual). That might be more uniform so you could just pick a couple of representative nodes instead doing a sum.