Large Displacement Issue - Twisting Wires

[kab343]

I am trying to run a simulation to investigate the force required to twist two pieces of wire together. Ideally, I want the simulation to complete 2 - 3 complete revolutions. So far I have managed to get the simulation to complete almost one revolution, but it never goes over one (my best so far is 0.96 of load). The error I seem to consistently get is:

FATAL ERROR E5076: MAXIMUM NUMBER OF BISECTIONS PERMITTED REACHED

I am using an enforced rotation of 360 degrees placed on a rigid body connector work point to 'twist' the model. I have changed RigidElemType to BAR as noted elsewhere in the forums for large displacements. I also have a constraint placed on the same workpoint in the same direction as the forced rotation. The other end of the wire pair is fully constrained. And there is a surface contact enabled between the two wires.

I have tried a number of different configurations:

1. Upping the number of increments in Nonlinear Setup to 360 and then 720.
2. Enabling and disabling different convergence criteria.
3. Turning large displacements on (and off) in Analysis/Options

Nothing seems to make the simulation anymore successful. Anyone else have any ideas on what else I could try?

[shigeaki.k]

Hello @kab343,

could you keep RigidElemType=BAR and try changing the contact settings? Try unsymmetric and swap the master/slave if required. 

Regards,

Shigeaki K.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[kab343]

Tried unsymmetric contact, had the same error.

The number of iterations was initially set to 180, and displacement only selected as convergence criteria in Nonlinear Setup.

[shigeaki.k]

Hello @kab343

is the activation distance for the contact definition set manually?

I might be good if you could also share the model for others to look at.

Regards,

Shigeaki K.

[kab343]

Yes, I have it set to contact distance set to 5mm to capture the extent of both wires.

I've attached the model I have been using.

[John_Holtz]

Hi @kab343

I do not know why the analysis is failing, but here are a couple of things that I noticed.

1. The nonlinear material properties do not have a yield stress entered. (Materials > Nonlinear > Initial Yield Stress) Are you sure that this is what you wanted to be using? (What yield stress is the analysis using? Zero?)
2. The warnings and errors such as "no convergence in maximum number of iterations permitted" and "maximum number of bisections permitted reached" are not referring to the input of 180, 360, and 720 that you have been changing. (Although changing that "Number of increments" can be helpful.) The increments that the warnings are referring to are under "Nonlinear Setup > Advanced Settings > "Maximum iterations for bisecting load increment" and "Maximum bisections for each increment".

I would start by entering a proper yield stress.

[kab343]

@John_Holtz I entered a yield stress of 80% off tensile (350Mpa) and ran again. The simulation failed with the same error (FATAL ERROR E5076: MAXIMUM NUMBER OF BISECTIONS PERMITTED REACHED) but at an earlier stage, 0.866 of load.

I've also tried:

• Creating a simulation model using surfaces and shell elements to simulate this also did not work.
• Creating a solid part to twist the wires rather than using a connector and beam elements etc, this didn't work.

What should I try changing the parameters in "Nonlinear Setup > Advanced Settings > "Maximum iterations for bisecting load increment" and "Maximum bisections for each increment" it is not obvious to me reading through the help documentation what I can change in these parameters to help.

Thanks everyone for your help so far!

[shigeaki.k]

Hello @kab343,

thanks for attaching the model. I am still investigating but could you tell me if turning one end of the model by 360 deg. is necessary? I ask as I see that the von Mises has gone much higher than the tensile limit you have set. There is a limit to what FEA can do and I was wondering if you were pushing the analysis past what might also be realistic.

Regards,

Shigeaki K.

[kab343]

@shigeaki.k I ideally want to 2 - 3 full rotations. I'm running 1 rotation at the moment as a test and to keep simulation solve time manageable. 

And yes, axially the enforced rotation it is not constrained (I think) so I have been expecting the wires to shorten as they twist which would cause less stress in the simulation. We have physically twisted wire like this in this configuration so it is possible in real life. 

And yes, I've thought the same about the von mises, I could raise the tensile limit of the material if that is causing the error? 

[shigeaki.k]

Hello @kab343,

couple of thoughts that I have. Are you seeing necking and or complete plastic failure? You are using bi-linear model so you are not modelling the behavior past the ultimate tensile stress. Instead, if I recall correctly, I think the stress-strain line just keeps on going. 

I would use a finder mesh. The mesh pattern on the cross-section looks a bit "rough".

You are using rigid connectors which would stop the cross-sectional areas or the shape from changing. Is that the case in real life. How are you holding the ends of the cables?

Regards,

Shigeaki K.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[kab343]

@shigeaki.k yes, I've tried a much finer mesh but it still failed with the same E5076 error and took significantly longer to solve, I changed the mesh back to coarser mesh so the simulation study didn't take so long to solve.

One end of the wires is clamped solid, the other end is fed through a slot slightly larger than the wire diameter which is then rotated. Good point on the connector, I disabled the TZ and RZ DOF for Connector 2 and re-ran. Simulation failed at 0.95 of load with same E5076 error, I've attached the model.

What non-linear material model should I try instead?

[shigeaki.k]

Hello @kab343、

I have gone back to your first model and testing to see if the solve type make a difference e.g. using PCGLSS. You can change the solver type using the parameter DECOMPMETHOD.

Regards,

Shigeaki K.

[kab343]

@shigeaki.k how did you get on with the different solver? Any luck?

[shigeaki.k]

Hello @kab343 ,

apologies for the late reply. I have contacted the Product Team with regards to this issue. Working off the 1st model you attached, the below setting is apparently what helped the analysis to converge. Apparently, they were able to get approximately 1.5 rotation.

1) Lowered the MAXAD on the contact to be equal to the radius of one of the wires (I used a maxad=1.0) this greatly cuts down on the amount of contact and helps it converge.
2) I constrained the node that has the enforced rotation on it in the X and Y directions. This ensures the axis of rotation stays the same.

Regards,

Shigeaki K.

[kab343]

Hi @shigeaki.k, ok excellent that looks much better than mine!

Can you please send me the model so I can see what was changed please? I can PM my email address to you if needed?

[shigeaki.k]

Hello @kab343 

attached is the file from the Product Team.

Regards,

Shigeaki K.