bisection errors on rubber parts

[pquenzi]

I am using Inventor 2021 and Inventor NASTRAN 2021. 

I am trying to model a simple round rubber compression spring (2" dia x 1" long) using one of the rubber materials listed in the Autodesk library and a nonlinear analysis. For constraints I fix one flat surface and permit no radial movement on the other flat surface and apply a normal load or pressure to that surface. I can get that to solve okay but when I add a hole through the center of the spring I start getting fatal error E5076 (Maximum number of bisections permitted reached). Is that because the program cannot decide whether to bulge the inner wall in or out and is there some way around this?

Thanks.

[John_Holtz]

Hi @pquenzi 

You should not be using a rubber material from the Autodesk library. You need real material properties for the rubber that you are using. (In other words, one steel may be the same as another steel, but each type of rubber is different.) In particular, the Poisson's Ratio is often 0.5 in the material library which is technically correct, but 0.5 leads to a math instability somewhere. You can try changing the Poisson's Ratio to 0.48.

But let's assume the material properties are "close enough" or that the analysis fails to converge with real material properties. It is difficult to know why a nonlinear analysis fails to converge, but it is often some type of buckling: either the entire model wants to buckle, or an element has such a high compression load that the element wants to "buckle". Transitioning from one static state to another static state after buckling (if there is a post-buckling static state) is difficult for the solver.

You can try to use enforced motion instead of a force load. In some models, the load decreases as the displacement increases. This will converge with the enforced motion. It will not converge with a force load since you are telling the analysis to increase the load, and the solver is not converging because there is no solution with an increasing load.

By the way, rubber material should use hyperelastic material properties instead of isotropic material if the displacement is large. The stress-strain curve is rarely linear beyond a small range.

John

[pquenzi]

John,

I assumed it had something to do with buckling since it runs fine in tension and in compression with low loads and will run in compression without the center hole. I know that rubber material I selected with isotropic properties and elastic stress strain curve is not correct but I just wanted to get it to work with that material and then change to a more realistic material with actual properties. Lowering the Poisson's ratio did not help. 

I have not used enforced motion up till now, but what I did was put a compressive load on one face and then added an enforced motion load to that same face and it solved, but when I increased the force load but maintained the same enforced motion displacement I got the bisection error again. Am I using enforced motion in the proper way?

Is there some way to increase the maximum number of bisections?

Phil

[John_Holtz]

Hi Phil,

I would say that the analysis does work with the material from the library, and now is the time to enter more accurate material properties. (It is not necessarily reasonable to expect the analysis to run to completion with "wrong" materials, but at least the analysis is setup properly to the point where it runs.) One suggestion is to enter the "Nonlinear Setup > Number of Increments" instead of leaving it blank. When blank, the solver tries to increase the load factor in steps that get larger and larger. That is not a good approach when the analysis gets harder to converge as the load increases. You may want 20 or more steps to handle the large displacement, nonlinear materials. (I doubt the number of steps or number of bisections will help with the current material properties. The washer is trying to buckle elements around the ID as shown in the images below.)

The enforced motion load should be instead of the force. (One result of the enforced motion is what force is required to cause the motion, so you will get the information that you want of force versus displacement.) What's missing in the enforced motion setup is you need a fixed constraint in the same direction (Tz in your model). The enforced motion moves the (fixed) constraint, and the constraint is what moves the model. Without the constraint, the enforced motion does not do anything.

Although increasing the number of bisections (or the number of iterations for an increment) will not help in this model because the element is failing, those values can be changed under "Nonlinear Setup > Advanced Settings". Some of the input for convergence is described in this article: Understanding convergence in a Nastran nonlinear analysis | Inventor Nastran | Autodesk Knowledge Ne....

John