Ansys 13 Workbench Converge Error

[Michael1988]

Hi Everyone

I am currently having problems with my Ansys dissertation. I have a problem where I need to move a spring unit up a slope, then along the surface, then into a notch and back out.

Every time I solve it I the error "The Solver engine was unable to converge on a solution for the nonlinear problem as constrained.

Please can someone help I am running out of time. I have uploaded the problem If someone could please advise or even solve it, that would be so amazing

Kind Regards

 

[flash3780]

There are quite a lot of issues with your model which, many dealing with it likely being more complicated than necessary. Answer these questions and I may be able to help you:
- What are you trying to learn from your model?
- Is there symmetry that can be invoked?
- Can the model be truncated? Can parts be left out that don't affect the result?

I would guess that your model is having convergence difficulties because you're taking too large of a load step. Auto time stepping may help.

 

[Michael1988]

I am trying to Produce the results of the spring probe. That is my main goal, I had one of my lecturers try and help but he seemed to confuse me more.

Typically the spring values should start off at zero then increase to around a value of -200n at the top of the slope and along it until it reaches the notch. Once in the notch the value should range from approx -200n to -100n the back to -200n when out of the notch

Yes symmetry can invoked. Though I am not sure about the model being truncated as I am not sure what that is.

Thank you for trying to help it is much appreciated.

 

[flash3780]

So, you're looking for the force on the spring? Why is an FEA necessary at all? F = -kx, right?

 

[Michael1988]

Yes just the spring force.

I have to use the FEA part for my dissertation in order to compare the simulated results to the actual results to prove that FEA can be used. I actually have no choice as it was decided by my lecturer.

 

[flash3780]

Generally student posting is disallowed on this forum, but I'll do my best to get you pointed in the right direction.
Okay, well in that case let's start by simplifying the model down to only what is necessary to find a solution. The slider track does not contribute to the solution in any significant way, so you should remove it. The cup that the probe slides into also does not contribute to the force on the spring. There should only be three parts of your model: The slider, the probe, and the spring.
Once you've suppressed the other parts, I'd suggest that you utilize symmetry. Also, you could recognize that the probe will never interact with anything outside of the notch and cut off the slider at the vertical edge of the notch. You will also not need any of the geometry beyond the notch, so you could cut that off as well. Finally, you'll want to bring the surfaces into initial contact; Ansys will have difficulty seeing the initial interaction if you try and simulate them coming into contact... so move the slider such that it is just touching the probe. You can accomplish all of the above geometry manipulations in DesignModeler.
After you've utilized symmetry, truncated the model to a more managable size, and brought the surfaces into initial contact, you should then bring the model back into Ansys Mechanical Simulation and apply your boundary conditions. You'll want to use a Pure Penalty or Augmented Lagrange (slightly more accurate) contact formulation to simulate the interaction between the probe and the slider. You'll probably want to use the "Auto-Axisymmetric" option if you're interested in the contact pressure at the interface, otherwise the results may be difficult to interpret. I'd start with friction turned off, and then turn it on once you get your model to converge.
Before solving the model, be sure to turn on "Auto time stepping". Ansys is using nodal force iteration to determine the interaction at the interface between the probe and the slider. If you take too big of a load step, it may have difficulty converging. Auto time-stepping allows Ansys to automatically bisect the loads until it is able to find a solution (or until it hits the max number of bisections).
Hopefully that gets you pointed in the right direction. Keep an eye on your mesh quality and try to use a brick mesh where possible, as it is more efficient. You should be able to brick mesh this entire model. Let me know if you have any questions.

 

[flash3780]

I forgot to note... half the model would be half of the spring stiffness... and when you get your results you should multiply your spring force by two.

 

[Michael1988]

HI

Thanks for the help. I have added most of your suggestions. As I normally import my geometry from Solid Edge I have never utilized symmetry or truncated the model. But currently I am reading into it.

Also how do I change the mesh from triangular to rectangular?

Other than that I have been running the simulation. But I do not understand why I cannot get the probe to go up the slope. It just decides to go through the material instead of on the surface, why does that happen?

Also when I create loads of substeps they are not evely spaced out at the end of the solution, why is that?

Hope you can help.