"No convergence of nonlinear problem" during analysis in Robot Structural Analysis

Autodesk Support

Feb 5, 2025

Products and versions covered

Issue:

"No convergence of the nonlinear problem" message appears during model calculation in Robot Structural Analysis.

Warning message: "No convergence of the nonlinear problem..."  

 

 

Causes:

The lack of convergence of nonlinear analysis can be caused by the following factors (among others):
  • Not activated DSC algorithm.
  • Imprecisely defined model.
  • Model behavior when a small increase of load causes significant change in the deformation shape which makes obtaining converged solution difficult.
  • Overturning moment (equivalent horizontal force * distance to the rotation axis) being larger than stabilizing one (equivalent vertical load * distance to the rotation axis).
  • Excessive load causing lost of stability either for single element of a model or a structure as a whole.
  • Statically unstable model.
  • Large displacement analysis method not activated.
  • Simple load case calculation while combination of load with self weight it's necessary for structure stabilization.
  • Loads transferred from claddings to flexible bracings.
  • Incorrect properties of selected model members.
Example
Incorrect section properties
  • Tension members defined by mistake as compressed only.




 

Solution:

Not activated DSC algorithm

Activate DSC algorithm for calculation.
Follow the steps:

  1. Open Tolls > Job Preferences > Structure Analysis.
  2. Activate "DSC algorithm (bar releases)" option.
  3. Click OK button.
  4. Run calculation.

DSC activation

 

Imprecisely defined model

Increase tolerance for model generation:
Follow the steps:

  1. Go to scroll-down menu Analysis > Analysis types.
  2. Select Structure model tab.
  3. Set Tolerance to User-defined.
  4. Increase tolerance value.

Tolerance definition 
If tolerance modification does not help correct model geometry, refer to:

 

Model behavior when a small increase of load causes significant change in the deformation shape which makes obtaining converged solution difficult

Make the following changes (one by one) and check if the convergence is obtained:

  1. Change the calculation method for divergent load cases and combinations.
  2. Go to scroll-down menu Analysis > Analysis Types > "Change Analysis Type" to access Nonlinear Analysis Algorithm Options and set the Newton-Raphson algorithm for divergent cases and load combinations using the following settings:
    Modification of non linear analysis parameters
  3. Increase number of iterations for one increment from 40 to for example, 100.
  4. Change the default Load increment number (5), to larger (10-20). Sometimes, for instance for cable structures, decreasing increment number helps.
  5. Increase the value of tolerances.

Note: 
Tolerances should be small and it is not recommended to set them larger than 0.005. If this is done, carefully examine obtained results, verifying that:

  • The deformation shape is as expected.
  • There are no suspiciously large displacements or rotations of nodes.
  • The sums of applied vertical and horizontal forces equal the sums of FX, Fy, and FZ reactions.

 

Overturning moment (equivalent horizontal force * distance to the rotation axis) being larger than stabilizing one (equivalent vertical load * distance to the rotation axis)

This typically happens in simple load cases with only a horizontal load (for example, wind acting alone). Such cases may not converge in nonlinear analysis because the structure will overturn. To resolve this issue, these load cases can be set as auxiliary, limited to load definition only, provided that all combinations they are part of do converge.

 

Excessive load level

  1. Check if load values are defined in correct units.
  2. Create a combination with reduced load factors (for example, 0.5 instead of 1.2).
  3. Set buckling analysis.
  4. Calculate the model, and check the critical coefficient. If its value, divided by the load factor (as defined in point 2) is larger than 1, then the load is excessive. In that case increase section sizes or change the model static scheme.
  5. Switch off large displacement effect for not converging load cases.
Large displacement activation
  1. Define small elasticity for rotational degrees of freedom in releases used in model.
Small elasticity rotation

Note
For nonlinear releases with Uplift for Ux defined 
UX uplift in release definition
Definition of large elastic coefficient for UX improves convergence.
Elastic coefficient for UX

 

 

Statically unstable model

Correct model geometry, modify supports, reduce number of released members, modify existing releases.

Note:
Before running nonlinear calculation, it is recommended to run linear model version. It helps to identify and correct model geometry (identify nodes with excessive displacements or rotations). Change all nonlinear objects (tension/compression bars, nonlinear supports) to linear objects (truss members, linear/elastic supports) and run analysis to verify linear model stability.

 

Large displacement method not activated


Sometimes convergence can be obtained by activation of large displacement effects. Activate large displacement analysis for divergent load cases.

  1. Open Analysis > Analysis types.
  2. Type in divergent cases list in Case list field.
  3. Click Change analysis type.
  4. Activate "Large displacements" option.
  5. Click OK to validate.
Large displacement method

 

Nonconvergence for simply load cases

Set simple load cases as Auxiliary.
Follow the steps:

  1. Open Analysis > Analysis type.
  2. Select nonconvergent load case (all simple load cases) in Case list.
  3. Click "Change analysis type" button.
  4. Check "Auxiliary" then OK.
  5. Run Calculation. 

Refer to: Why it is recommended to set simple load cases as auxiliary for nonlinear models in Robot Structural Analysis.
 

Incorrectly defined section properties

Change section for incorrectly defined members. Use Geometry> Properties>Sections option.
 

Load transferred form claddings to flexible bracings

Remove bracings from load distribution. Follow these steps:
  1. Open Geometry>Additional attributes>Load distribution>Options.
  2. Activate Member and panel list.
  3. Select bracings.
  4. Click Ignore.
Members not considered during load transfer  

 

Check and correct properties - tension members only

Follow these steps:
  1. Select members which should work for tension
  2. Check Element type in Object Inspector.
Tension bar properties in object inspector 
  1. If necessary (different values or compression presented in Object Inspector) correct members properties.
    1. Open Geometry >Additional Attributes>Advanced member properties.
    2. Check truss members - only axial forces act.
    3. Check Tension/Compression members.
    4. Select Tension members button.
    5. Apply for selected members.
Setting tension bar only

 
 
 
 
 
 

Products:

Robot Structural Analysis Products;

Was this information helpful?

Need help? Ask the Autodesk Assistant!

The Assistant can help you find answers or contact an agent.

Ask the Assistant

What level of support do you have?

Different subscription plans provide distinct categories of support. Find out the level of support for your plan.

View levels of support