"No convergence of nonlinear problem"appears while nonlinear analysis on a model with uplift defined for supports or slab elastic foundation in Robot Structural Analysis

Autodesk Support

Jun 6, 2024

Products and versions covered

Issue:

No convergence of nonlinear problem " message while nonlinear analysis reported in Robot Structural Analysis.

no convergence of nonlinear problem
  Problem reported in a model with uplift supports (UZ+ or UZ-) defined,

uplift supports
or unidirectional soil defined in Robot Structural Analysis.
soil definition with uplift effect
 
 
 
 
 

Causes:

Possible causes:

  • Incorrectly defined uplift direction.
  • Simple load cases not defined as auxiliary.
  • Not modified (default) calculation parameters for nonlinear load cases and combinations.
  • RZ rotation not blocked in nodal supports.
  • Model not supported in panels tangent direction.
  • Too significant elastic support coefficient KZ defined for unidirectional soil simulation.
  • Nodal Mz loads (in plane moments) defined for slab with unidirectional elastic foundation.
  • Too big overturning moment




 

Solution:

Possible solutions:

Verify and modify if defined uplift direction:

  • For uplift defined from Support option uplift direction corresponds to global system of coordinated (UZ+ means blocked node displacement in global UZ-direction).
  • For uplift defined from panel Thickness dialog option uplift direction corresponds to local panel z axis direction.(Uz+ means blocked node displacement in local Uz - direction).
 

Change simple load cases type to auxiliary:

If only simple load cases are divergent define them as auxiliary cases. Define and calculate combinations including structure self weight.  Follow the steps described in the Non convergence of nonlinear analysis for simple load cases for a model with unidirectional supports or soil (uplift allowed) in Robot Structural Analysis article.
 

Change calculation parameters for nonlinear combinations:

If there is lack of convergence for combinations then follow the steps described in "No convergence of nonlinear problem" during analysis in Robot Structural Analysis article.

 

Stabilize model by nodal supports modification. Add small elasticity for RZ rotation:

Follow the steps:

  1. Open Geometry > Supports.
  2. Double-click support label with uplift defined.
  3. Go to Elastic tab.
  4. Define small Elastic coefficient (0.01 kN*m/deg) for KZ.
horizontal elastic coefficient definition

 

Stabilize model by defining tangent elasticity when calculation are divergent for slab with elastic support and uplift effect defined.

Follow the steps:
  1. Open geometry > Properties > Thickness.
  2. Double-click to thickness label to be modified.
  3. Open Parameters of foundation elasticity.
  4. Define Kx and Ky coefficients.
  5. Add then Add.

elastic horizontal elasticity

 

Decrease value of KZ for slab elastic support.

Follow the steps:
  1. Open geometry > Properties > Thickness.
  2. Double-click to thickness label to be modified.
  3. Open Parameters of foundation elasticity.
  4. Decrease Kz value and if necessary Kx and Ky (recommended value for rigid support 2000000 kN/m3).
  5. Add then Add.
too large elasticity in UZ direction

 

Replace supports with uplift effect by supports with nonlinear function (defined to simulate uplift effect):

For models where it's not possible to obtain convergence of combinations by changing the nonlinear analysis parameters, it may be considered replacing uplift only supports with nonlinear function supports with:
  • Linear function with large stiffness coefficient for semiaxis half function in one direction (here negative semiaxis) to simulate fixed direction.
  • Linear function with small (close to zero) stiffness coefficient for semiaxis half function in the other direction (here positive semiaxis) to simulate uplift support "free" direction.
The sample functions are illustrated below:
 nonlinear support definition with function
After calculating the model, check the reaction values to make sure that they are equal to zero or negligible in the direction the nonlinear support has been defined.

 

Distribute nodal Mz moments (in plane moments) applied to slab to nearby nodes using rigid links.

Follow the steps:
  1. Open Geometry > Additional attributes > "Rigid links".
  2. Create new rigid link.
  3. Define label.
  4. Block UX and UY.
  5. Add.
rigid link definition
  1. Activate Selection of secondary nodes in Rigid link dialog.
  2. Select node with in plane moment defined and nearby nodes to be connected with rigid link.
  3. Activate Primary node field.
  4. Click node with in plane moment defined.
  5. Apply.

rigid link- apply to structure

  1. Repeat for all nodes loaded with in plane moments.
Refer to video presenting rigid links definition.
 

Verify applied loads, too big overturning moment cause model with uplift defined not stable.

Verify horizontal load values, buoyancy load cases. Decrease load values if possible. Increase model mass (section sizes, slab thickness) if loads cannot be reduced.
 
 
 
 
 

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