Learning Forum

[oamarquezr]

Hello,

 

I am an Ansys beginner and a I am having a problem trying to solve a flexible fiber reinforced actuator, the solver says "the solver engine was unable to converge on a solution". I am submitting the .wbpz file tor you to check it.

Also, I would like to measure the rotation angles, but I cannot add a remote point to the end of the actuator, Ansys replies: "A load transfer error has occurred".

Thank you for your help

 

Regards

[peteroznewman]

The fibers are beam elements wrapped on the outside of the solid and you use bonded contact to connect beam, shell and solid elements together.

Under Analysis Settings, your Initial Time Step is too large and you get two bisections before the solver make progress. Change the Initial Time step to 1e-2 to avoid wasting time at the beginning. That doesn't help the solver get any further than you have already.

On the Solution Information folder, set the Newton-Raphson Residuals number of plots to 5 so you can see where the solver is having problems converging. Once you do that, Solve.  Now you will have a series of plots under the Solution Information folder to guide you where the model needs improvement.  Below is the plot.

The solver cannot achieve equilibrium due to the force imbalance in the model at this location. One corrective action is to use smaller elements. Try that next. It might not let the model get much further.

The beam elements have a linear elastic, isotropic material property so as it tries to bend, large forces build up to limit the bending. But the real material is Kevlar, which has orthotropic material properties. It is very stiff axially, and very flexible in bending. You might need to create a new material for the beams.

A simple idea is to change the beams to LINK180 elements. These will have a hinge at every node. That way, there will be no bending moment in the fiber, but there will still be tensile loads supported. This is probably a more accurate model of the real structure.

After I only reduced the beam element size, the next problem is with the solid mesh. It is too coarse. I recommend going into DesignModeler and using the Slice tool to slice the two ends off the rubber tube. Then pick the three solids and Form New Part to use Shared Topology. Now you will be able to use a Sweep Mesh on the center part of the tube, and put two hex elements through the wall thickness of the tube. Use Multizone Method on the two ends of the tube and again, make sure to get two hex elements through the wall thickness of the ends.

Keep in mind that this is a very complicated model so you will probably have many convergence errors and need to make many adjustments to the model to make progress. It won't be easy.

[oamarquezr]

Dear Peter,

 

Thank you so much for your reply and your suggestions. Effectively, by changing the beams to links, the solver was able to go further and helped to reduce the force imbalance, and, as you mentioned, the real behavior of the fibers is orthotropic.

 

At the moment I am struggling a little trying to perform the "sweep mesh", since the body does not want to become "sweepable", but I will deal with it. The "Newton-Raphson residuals" is providing more information about the force convergence, and I am attacking the contact regions to see if that improves the force convergence.

 

Once I am able to go further than this, I will let you know.

 

Again thank you for your help,

 

Regards

 

 

[peteroznewman]

Glad it's going well.  Here is the result of meshing after slicing the two ends and hiding one of the ends.

ANSYS 19.2 archive attached.

Please mark my post above with Is Solution to show this discussion is Solved, or ask a follow up question.

[oamarquezr]

Thank you again Peter for all your help I really appreciate you are taking your time and experience to help me! Nevertheless, I am a bit confuse, I am still working with the model with all your suggestions and I tested the file attached to the last post, but none of them are converging at the moment, so it is still far from being solved... If I close it, can I reopen it later, if I got stuck again and/or if I finally get to the solution, so people in the future trying to simulate something similar will know how to handle it?

Right now the the system with the improved mesh is failing before that with the coarse mesh and the Newton-Raphson Residuals show at max a force of 0.5 N, so I am still following the hints and trying different possible improvements/methods to achieve a behavior similar to real life.

 

Once more I want to thank you for the assistance,

 

Regards.

[peteroznewman]

Yes, keep the discussion open until you have a model converged to the final state. I did not mean to imply that the model I attached would solve to the final state, only to demonstrate how to slice up the body to create good quality meshes that have several elements through the thickness of the wall.  Please reply if you get stuck.

Hyperelastic material models undergoing large deformations often do better if the solid elements have been set to use Reduced Integration.