Hertz contact between 2 spheres in Abaqus 1

[ImperialStudent]

Hi everyone,

I'm trying to solve a Hertz contact problem between two spheres.

My model is axisymmetric and comprising 2 elastic semi-spheres that are initially in contact (on single point at the top of the spheres).

I use a surface-to-surface contact with a "Hard contact" normal behavior and frictionless.

If I impose a displacement to one of the spheres, the simulation converges. But if I apply a pressure or a concentrated force on one of the spheres, it does not.

I tried to use the contact controls stabilize option but it did not help.

I want to validate my simulation against the analytical solution that is defined for an applied load...that's why I really need to make my simulation work in this configuration.

Thanks in advance for your help.

Regards.

 

[corus]

Apply a displacement and then in the 2nd step remove it and add your load/pressure.

 

[rstupplebeen]

In addition to corus's suggestion, other options to try in no particular order:
1. Make sure nonlinear geometry is checked NLGEOM
2. Reduce your minimum step size and initial step size
3. Have the load reference an amplitude using smooth step
4. If both spheres are the same you can model 1 with a rigid symmetry plane to contact with.

I hope this helps.

Rob Stupplebeen

http://www.optimaldevice.com

 

[ImperialStudent]

Thanks for your suggestions.

@ corus

I m afraid that between having both spheres initially in contact and applying a displacement to put them in contact, it does not change anything.

@ rstupplebeen

1. Check
2. Done
3. I m afraid I did not understand. What should I use instead of a ramp?
4. You re right, and I m in this case, but replacing the two spheres by one sphere against a rigid plane did not help.

Otherwise, if I use node-to-surface interaction instead of surface-to-surface interaction, it's working but I m not confident in the results. In the Abaqus documentation it is stated that the error with the node-to-surface interaction is much bigger than with the surface-to-surface one. Do you have any thoughts about this?

 

[IceBreakerSours]

A couple of the following points have already been suggested to you:

1. How do you know that the two spheres are, in fact, in contact? Have you looked at the COPEN in *Preprint?
2. Add *contact stabilization
3. Check the documentation for *Amplitude and smooth step.


Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[ImperialStudent]

Hi IceBreakerSours and thank you.

1. Yes, I had a look at the COPEN output.

2. Already done. That's what I meant by "I tried to use the contact controls stabilize option".

 

[IceBreakerSours]

When you say the simulation does not converge, what do you mean? Tell us more about what you see in the .sta file.

Also, what type(s) of warning messages do you see in .dat/.msg files?

You may look at the residuals and warnings in the Job Diagnostics menu as well in order to understand what's going on with your model.

Are you new to this forum? If so, please read these FAQ:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[rstupplebeen]

For number 3. of my previous post Amplitudes is right above Loads in the tree and about half way down is 'Smooth Step' create a smooth step"
0,0
1,1
It's basically a ramp with a asymptotic ramp at the beginning and end.
Reference this Amplitude in your force.

Another option is to put the parts in slight interference and in the first step's contact definition click 'interference Fit' 'gradually remove' 'Automatic'

Basically the contact will push the nodes until they are no longer in contact with each other.

On a separate note I'm sure that I have helped with this exact problem before so try searching with my name and you can probably find it.

I hope this helps.



Rob Stupplebeen

http://www.optimaldevice.com