×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Hertz contact between 2 spheres in Abaqus

Hertz contact between 2 spheres in Abaqus

Hertz contact between 2 spheres in Abaqus

(OP)
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.

RE: Hertz contact between 2 spheres in Abaqus

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

RE: Hertz contact between 2 spheres in Abaqus

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
www.optimaldevice.com

RE: Hertz contact between 2 spheres in Abaqus

(OP)
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?

RE: Hertz contact between 2 spheres in Abaqus

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

RE: Hertz contact between 2 spheres in Abaqus

(OP)
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".

RE: Hertz contact between 2 spheres in Abaqus

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

RE: Hertz contact between 2 spheres in Abaqus

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
www.optimaldevice.com

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources