30 Replies Latest reply on Apr 2, 2014 3:45 PM by Jared Conway

# Nonlinear problem on Elastic couplings.

Hi, everyone. I have a problem with nonlinear simulation of elastic coupling. I want to simulate the deformation of the elastic element (rubber) with 80 Nm torque. Everytime I get a different error of the simulation. I was trying everything  to get done, but that simulation it pissing me off. Can anyone help me for that? Now I will write every option and settings, that I have given to the simulation.

1. Nonlinear simulation study.

2.Simulation properties.

2.1. Autostepping.

Initial time increment - 0.01;

Min - 1e-008; Max - 0.1;

2.2 Geometry nonlinearity options.

Use large displacement formulation.

2.3. Solver.

Direct Sparse.

2.4. Incompatible bonding options.

More accurate.

Control - Force;

Iterative - NR;

Integration - Newmark;

Do equilibrium iteration every - 1 step;

Maximum equilibrium iterations - 30;

Convergence tolerance - 0.001;

Maximum incremental strain - 0.01;

Singularity elimination factor - 0.

3. Material properties.

3.1. Coupling - ANSI 1020.

3.2. Elastic element - Rubber.

Model Type: Hyperelastic - Mooney Rivlin;

Poisson Ration - 0.4995;

Thermal Expansion Coefficient - 0.00066 /K;

First constant - 5.79 N/mm^2;

Second constant - 1.45 N/mm^2;

Mass Density - 1000 kg/m^3;

Tensile Strenght - 13.79 N/mm^2.

P.S. I was trying with Stress - Strain Curve, too.

4. Connections.

4.1. Component Contacts - Global Bonded Contact with Compatible Mesh.

4.2. Contact Sets - No penetration (for all faces); Surface to Surface; Friction - 0.8.

P.S. Contact face between eight cylindrical faces and thumbs of coupling is 100 mm^2.

5. Fixes.

5.1. Half of the coupling is fixed.

5.2. On a bore of the other half of the coupling is set on Fixed Hinge.

6.1. On a bore of the same half of the coupling is set 80 Nm torque.

7. Mesh.

7.1. Standart mesh - size 6.5 mm; tolerance - 0.15 mm; draft quality mesh.

7.2. Mesh control of the Rubber - size 3 mm; a/b - 1.5.

I am attach picture of the coupling.

• ###### Re: Nonlinear problem on Elastic couplings.

What are the error messages that you're getting? Can you post your model?

Just a word of warning: expect to deal with a lot of frustration. Any non-linear analyses can be trial-and-error intensive, as there are a great deal of factors that come into play when trying to create a numerically stable model. You also a fairly complex non-linear model on top of that (contact, large-displacement, large strain, hyper-elasticity).

• ###### Re: Nonlinear problem on Elastic couplings.

One of all different errors is: Out of Balance Force is diverging, Automatic Reset

• ###### Re: Nonlinear problem on Elastic couplings.

That sounds like a numerical stability issue. Suppress you toque load and add in a enforced rotation constraint (do something small, like 0.1 degrees) and try running it again.

On the inner surface were you have you 80 Nm torque load, is the only allowed DOF an on axis rotation?

• ###### Re: Nonlinear problem on Elastic couplings.

Hi, Shaun. Thanks for replay. I have tryed that with the rotation fixture and it works, but my job is to see how that elastic element is deformed on 80 Nm applied nominal torque. It has to be working with torque, but I make mistake somewhere. And yes, inner surface is the only allowed DOF an on axis rotation.

• ###### Re: Nonlinear problem on Elastic couplings.

OK, so we have good news and bad news. If it worked with an enforced rotation, but not with an applied load (your 80 Nm torque), then you have a numerical stability issue. The good news is that we've narrowed down and located the issue...the bad news is that issue is a numerical stability issue. I say bad news because resolving this kind of issue could take some trial-and-error. Some analysis settings you'll need to play with are:

1. Reducing step size.
2. Changing solution control method.
3. Increasing convergence tolerance.

Under the Advanced Options button in the Solution tab, do you have Arc-Length control selected? If not, select it and try the analysis again.

• ###### Re: Nonlinear problem on Elastic couplings.

if enforced rotation works and force isn't working

stefo, iterate your rotation until the reaction torque = 80N/m and save yourself some hassle of trying to get the force (torque) to converge

• ###### Re: Nonlinear problem on Elastic couplings.

Here is other errors.

• ###### Re: Nonlinear problem on Elastic couplings.

Hello guys, I am kinda new to solidworks and i am getting some problems: 1) I downloaded the librabry but when I am dropping in flanges and stuffs ain't getting no routing/auto routing/. What can I do? Please help!!!!

• ###### Re: Nonlinear problem on Elastic couplings.

probably worth posting in the routing forum

• ###### Re: Nonlinear problem on Elastic couplings.

Thanks for advices friends. Tomorrow I will try everything that you wrote and will write you for my results. Thanks again.

• ###### Re: Nonlinear problem on Elastic couplings.

Hi, now I am trying with different methods:

1. Control method - Displacement

1.1. RX: X Rotation with liner graph (Xmax = 0.2 rad, Ymax = 9 sec)

and

1.2. Control Method Arc Lenght - max rotation 0.2 rad

It give me: Negative roots for quadratic equation, Automatic Reset

Now I am trying with different Iterative Solution (MNR) for control method Force. Now it is good 15% for 17 min.

• ###### Re: Nonlinear problem on Elastic couplings.

Stefo,

I don't know how your coupling behaves, but 0.2 radians seems like a lot of rotation. That is 11.5 degrees. I would try smaller values, if that seems reasonable to you.

Jerry S.

• ###### Re: Nonlinear problem on Elastic couplings.

I have stopped the simulation, because it restart everytime from 1 hour between 50% and 60%.

• ###### Re: Nonlinear problem on Elastic couplings.

On Integration method (Wilson - Theta) give me this:

• ###### Re: Nonlinear problem on Elastic couplings.

Hi Jared, what you mean about "iterate your rotation until the reaction torque = 80N/m"? Sorry for that question,but I am new in this nonlinear simulation thing.

I dont now on T=80 Nm torque what is the deformation angle.

• ###### Re: Nonlinear problem on Elastic couplings.

try this on a cantilever beam to understand the concept

fix one end

displace the other

your goal is to determine the behavior when there is 1lb of force

we could go directly to that by applying the force but you can't do this

so how could you do it?

apply a displacement

run the analysis

then do a guess to increase/decrease the displacmeent to get the force you want

change the setup

run the analysis

rinse repeat

in the long run, is this a problem you can get some help from your reseller on? or is this something in the educational space?

• ###### Re: Nonlinear problem on Elastic couplings.

Hi Jared, this problem is a part of my dissertation.

• ###### Re: Nonlinear problem on Elastic couplings.

• ###### Re: Nonlinear problem on Elastic couplings.

I increased convergence tolerance to 0.01 and reduced the max autostepping to 0.01 and No. of adjustments to 10.

And again get: Out of Balance Force is diverging, Automatic Reset on 58%

• ###### Re: Nonlinear problem on Elastic couplings.

Stefo,

I'm not familiar with the way SolidWorks Simulation handles this, but I suspect it is the same as ANSYS. A non-linear analysis is solved in a sort of quasi-time. You set the values you want for your force or torque or displacement at each time step. The first step is from 0 to 1 "second", the second is from 1 to 2, and so on. You can also choose different numbers for your "time" increment, so you could decide to go from 0 to 0.1, 0.1 to 0.3, 0.3 to 1.0, or whatever you like. You also choose how high to make each step, so you could make your rotation, for example, be 0.01 rad, 0.03 rad and 0.05 rad.

SolidWorks will take smaller steps to approach the solution. I think that the max autostepping of 0.01 tells you that it will give up when it can't get an incremental solution with a step size of 0.01. You might need to decrease this size to 0.001 or even 0.0001 or lower.

You might also try increasing the convergence tolerance; 0.01 seems very tight to me, but I am not familar with SolidWorks Simulation. Try 0.2 for a start. If you get a solution, you can decrease it until you get an acceptable convergence or you get as low as it can go.

Jerry S.

• ###### Re: Nonlinear problem on Elastic couplings.

Generally Jerry is pretty good but on this one I think he has made an error. NL  static works like this: time allows you to control a sequence of events. For yours most would use 0 to 1 to sequence from no load or displacement to the full load or displacement you want. Auto stepping allows an algorithm to control what sort of increments are required to ensure you stay on the load displacement path over the course of the full load or displacement. The maximum displacement is not critical unless you need to have a minimum number of increments to ensure you get the path resolution you need. With the minimum increment size you tell the auto stepping algorithm when to give up and pack it in. To be fair to Jerry I think in ANSYS there is a lot more emphasis on manual control of increments so his remarks fit more closely with that code. In Abaqus they speak in terms of steps, they don't bother with time in NL static - in your case it would be a single step. If a fixed displacement provides a stable solve then put in a displacement that requires a force greater than what you are looking for then plot the reaction force vs time. Time equals the fraction of displacement if you use 0 to 1 for the time increment of the step. Then just look down the curve and see where it hits the number you are looking for. This what Jared was suggesting. If you are totally confused don't worry it takes a bit to develop a mental model of how NL analysis goes. Keep with it &amp; Good luck.

• ###### Re: Nonlinear problem on Elastic couplings.

It doesn't like an edit from an iPad so to correct above - I used the term ....maximum displacement is not critical....when I meant maximum increment. Sorry about that. The one finger typing on the iPad did me in.

• ###### Re: Nonlinear problem on Elastic couplings.

Hi All, I wonder if I set a Uniaxial tension curve, Pure shear curve and Biaxial tension curve of material will be that decision of my problem?

• ###### Re: Nonlinear problem on Elastic couplings.

the problem solves with displacement

adding complexity will improve the accuracy potentially but may make it more difficult to solve

• ###### Re: Nonlinear problem on Elastic couplings.

What does you stress-strain curve look like for your rubber material? Typically, numerical instabilities due to material properties only happen with shape changes in the stress-strain curve that result in either a negative or zero slope. For example, a perfectly plastic curve could cause this because once you hit the yield point, your stiffness remains constant with further displacements.

• ###### Re: Nonlinear problem on Elastic couplings.

Hi all, I have found my errors on this simulation, now I am more clear of that. Thanks to all for replays.

• ###### Re: Nonlinear problem on Elastic couplings.

Stefo,

If you would be good if you could tell us what the errors weres. It might save us from having similar problems.

Jerry S.

• ###### Re: Nonlinear problem on Elastic couplings.

Yes, no problem.

1. It is very important to set correct stress-strain curves or constants (if you have only tension, you need stress-strain curve of simple tension;if you have tension and  pure shear, you need both curves; and like this), because for best results the solidworks need more accurate date for the model. (experimental date);

2. Reduce mesh control size;

3. I was set wrong friction coefficient between rubber and steel.

That is all.