Learning Forum

[lvelasquez]

Hello,

Im trying to run a simple simulation of symmetry. One plastic plate bolted to a metalic side bar. A 2000 newton force is applied to the internal face of the plate in -Y direction and the bolts have a pretension of 3500 newtons each. I´ve run the simulation before without pretension but all contacts where bonded, and it runs fast, about 25 mins to run with 165K elements. I made a few runs changing to frictional and it took about 2 hours to finish.

Large deflections are on, 3 steps (load the pretension, lock, and finally apply the external force), autostepping (tried with 50 initial, 25 minimum and 500 maximum - didnt work), solver programmed controlled (tried direct but same).

 

I made the local coordinate system to cut the bolt just between the end of the side bar internal face and the plate side face.

Its been like two hours and it hasn`t even finished the first substep.

Without large deflections, I got a result but it was weird.

The bolt penetrated it self and when inside out.

Any idea what is happening or what am I missing?

[Harshvardhan]

Hi,
There can be many reasons the solution to not converge. The best option to look for a specific issue is to check the Solver Output and see what error message is present there and what steps has the solver been doing before it.

The solver output can be found in the Solution Information tab under the Solution tree.

Regards,
Harshvardhan
Ansys Help
Ansys Learning Forum (Rules & Guidelines)

[lvelasquez]

Hello Harshvardhan,

After a some research and changed the formulation of the contacts (making sure all were closed)  to pure penalty, activated line search and activating weak springs, the solution was able to converge. Now I got a max stress of 30 GPa (yes, 30,000 MPa). I tried using translational joints but the behaviour was weird. 

Now my new questions arrises:

1. Can weak springs cause elevated stress?
2. Can I use translational joint or bolt pretension with this concept of geometry? The bolt is inserted to the plastic using an insert, which I removed to reduce the number of elements. But it has no nut at the lower end, so I´m thinking this is why I got the "self penetration" of the bolt body. Aslo I need to know the shear stress in the bolt so I can´t go with bolt pretension, but with translational joint I get the "constraint conditions are not satisfied for 3 joint elements with lag mult option".

[Harshvardhan]

Hi,
To answer you questions:
1. If your model is properly constrained, there should be no difference in stress values due to addition of weak spring. The stiffness of weak spring is calculated by Mechanical and is kept at a very low value to not affect the stress results.

2. You can apply bolt pretension even if there is no nut in your model. Simply divide the bolt shank into 2 parts depending on the geometry. One clearance part, one threaded part. Threaded part can be in contact with the body and you can apply pretension in the clearance part. (Or in the interface of clearance and threaded part if you have split body instead of face).

 

I hope this helps.

Regards,
Harshvardhan
Ansys Help
Ansys Learning Forum (Rules & Guidelines)

[lvelasquez]

Hi again,

1. Ok, a found the 3-2-1 rule and got rid of the rigid body motion warning so I took off the weak springs
2. Yeah, I found a webinar about how to model bolts and found my error. I was applying a rough contact in the clearance face, so at the "breaking" of the shank ANSYS needed a large force and that might explained the "self penetration" of the bolt. I had to cut the face of the bolt to correctly apply bolt pretension object.

Now my simulation is able to converge and I got my results. Thanks

[Harshvardhan]

Hi,
Glad to hear that the simulation is now able to converge.

All the best for future simulations.

Regards,
Harshvardhan
Ansys Help
Ansys Learning Forum (Rules & Guidelines)