Learning Forum

[Abhijit Bhandari]

I am trying to make a transient structural analysis of flat belt driven pulley system.
The analysis settings is as follows:

No of steps: 50
Minimum and Maximum is based on tabular data: ranges upto 50

For initial time its 1 sec and the minimum and maximum time step is also 0.1 sec.

Large Deflection is turned On.

Mesh resolution is set at 7.

Joints and contact regions are well defined. The joints are body-ground type revolute joint applied to both driver and driven.

For constraints remote displacement is provided to driver and driven and they are free to rotate about z -axis. Along with that a joint load is applied to the driven pulley. For geometry, only the belt is deformable rest is rigid.


The error I am getting is :
The solver engine was unable to converge on a solution for the nonlinear problem as constrained. Please see the Troubleshooting section of the Help System for more information.


And the multiple warnings are:

The solution failed to solve completely at all time points. Restart points are available to continue the analysis.

Although the solution failed to solve completely at all time points, partial results at some points have been able to be solved. Refer to Troubleshooting in the Help System for more details.

The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose.
Contact status has experienced an abrupt change. Check results carefully for possible contact separation.

One or more MPC or Lagrange Multiplier formulation based contact regions or remote boundary conditions may have conflicts with other applied boundary conditions or other contact or symmetry regions. This may reduce solution accuracy. For MPC based remote points, setting the relaxation method may help eliminate overconstraint. Tip: You may graphically display FE Connections from the Solution Information Object for non-cyclic analysis. Refer to Troubleshooting in the Help System for more details.

Two or more remote boundary conditions are sharing a common face, edge, or vertex. This behavior can cause solver overconstraint and is not recommended, please check results carefully. You may select the offending object and/or geometry via RMB on this warning in the Messages window.

Please help

[Sai Deogekar]

Hi,

1. You have 50 steps defined. Is the non-convergence happening in step 1 itself?
2. Why do you have 50 steps? A step is used to define the load profile. Does your load profile need 50 distinct points to be defined?
3. "Initial time is 1 s": Does this mean step 1 is 1 second long? If min and max substeps are 0.1s, then that means 1/0.1 = 10 substeps will be used. Maybe 10 substeps are not enough. You can turn on Auto Time Stepping, and reduce minimum substep size to 100 or 1000. That way the solver can use a smaller substep and achieve convergence,

Hope this helps.

[Abhijit Bhandari]

I am still having the same error even after making a change to my analysis settings. I am allowing large deflection as the material used for the belt is neoprene rubber and both the driver and driven pulley material is structural steel. All of the components considered are flexible.

My current analysis settings:

[Sai Deogekar]

Hi, based on the pictures that you shared, I think you need 1 "step" and multiple "substeps". You are using a minimum and maximum time step of 1 s. So if the solver needs a smaller time step to converge, it can't use a time step of say 0.1s or 0.001 s. Try the following:

Number of Steps: 1

Auto Time Stepping: On

Define By: Time

Mininum Time Step: 0.001s

Maximum Time Step 0.1 s

If it still doesn't converge play around with these values (try reducing the minimum time step) and see if that helps.

 

 

[Abhijit Bhandari]

Thank ypu so so much. Finally, it worked.

[Sai Deogekar]

Glad to be of help :)