Nonlinear - Solution

The Solution tab in the Nonlinear dialog box sets solution-related options. You can set the following options on this tab.

Stepping Options

Time information is associated with the definition of time curves for loads and boundary conditions. Time is a pseudo variable for static problems without creep, viscoelasticity, or thermal loading using time-dependent results from a transient thermal study.

Start time Starting solution time. Not used by the Arc-Length method.
Restart Restarts from the last successful solution step. Available only if the restart data exists with Save data for restarting the analysis activated in the previous run.
You can change any load parameters (Time curve dialog box) when restarting the analysis.
You can change fixture conditions from free to fixed degrees of freedom and vice versa when activating the Restart option.
For example, to change a fixture condition from fixed to free when restarting the analysis:
  • Under Translations (Fixture PropertyManager), enter 1 in the direction that you apply the fixture.
  • Under Variation with Time, select Curve and click Edit. In the Time curve dialog box, enter the curve data:
    X (Time, sec) Y Value Fixture condition
    0 0 fixed
    1 0 fixed
    1.05 Off (restart) change from fixed to free
    2 Off free

To change a fixture condition from free to fixed when restarting the analysis:

  • Under Translations, enter 1 in the direction that you apply the fixture.
  • Under Variation with Time, select Curve and click Edit. In the Time curve dialog box, enter the curve data:
    X (Time, sec) Y Value Fixture condition
    0 Off free
    1 Off free
    1.05 0 (restart) change from free to fixed
    2 0 fixed

    During the first run (remember to select Save data for restarting the analysis for the first run ( Start time = 0 < t < End time = 1 sec) the solver ignores this fixture and the selected entity where the fixture is applied is free to move. Activating Restart and rerunning the analysis (Start time = 1 sec < t < End time = 2 sec), the solver applies the fixture and the selected entity is restrained from moving in the specified direction.
End time Ending solution time. Not used by the Arc-Length method.
Save data for restarting the analysis Check this flag before running the study for a possible restart. The software takes some time and disk space to save the data required for a proper restart. If you clear this check box, you must start from the beginning.
Remeshing the study deletes all restart information.
Time increment Sets the procedure for incrementing time at each solution step for the Force and Displacement control methods. For the Arc-Length control method, the program uses this value to estimate an arc-length increment.

Automatic (autostepping)

When checked, the program determines an increment internally for each solution step to improve the chances of convergence. This option supports all control techniques. If the flag is checked, the following entries are used:

Initial time increment

The program uses this increment as the initial guess for the time increment.

Min

Minimum time step. The default is 1e-8 seconds.

For nonlinear dynamic studies only, if the specified minimum increment is equal or greater than the initial time increment, the program resets the minimum time step to 10% of the initial time increment.

Max

Maximum time step. Default is the End time for the Force and Displacement control methods.

For nonlinear dynamic studies only, the specified maximum time step is not used. The program resets the maximum value to the initial time increment.

No. of Adjustments

Maximum number of time step adjustments for each solution step.

Fixed

Fixed time step increment. Default is to run 10 steps.

The program stops the analysis if:
  • The number of step-size adjustments in any step exceeds the maximum number of step adjustments.
  • The step increment required for convergence becomes smaller than the minimum step increment.

Geometry nonlinearity options

Compute free body forces After the analysis completes, lists the free body forces of selected entities at each solution step. The free body forces can come from contact, external loads, restraints, or connectors.
Right-click Results, and click List Result Force. Select Free body force, the geometry entities (body, face, edge, or vertex), and a solution step to list the free body forces and moments.
Use large displacement formulation Uses the large displacement formulation.
Update load direction with deflection If checked, the direction of the applied load (normal uniform pressure or normal uniform force) is updated for every solution step with deflection.
Examples
(a) Applied normal load on undeformed geometry.
(b) Flag for Update load direction with deflection is cleared. Original load direction is maintained on deformed geometry.
(c) Flag for Update load direction with deflection is checked. The load direction is updated, and remains normal to the deformed geometry for each solution step.

When you apply a torque, the program calculates the force and the moment arm that creates the torque, and applies the force to the nodes. These forces retain their initial directions throughout the solution and ,therefore, may cause high unexpected stresses to develop.
Large strain option Uses the large strain formulation. Select the large strain formulation for Nonlinear elastic, von Mises Plasticity, Nitinol, Viscoelastic, and Hyperelastic material models.
When selecting the large strain option, you must enter the stress/strain curve data depending on the material model. See topic Simulation Help: Defining Stress-Strain Curves to learn about valid input data for the stress/strain curve.
Keep bolt pre-stress

When this option is cleared, the bolt's length at zero stress state L0 is determined based on the length of bolt at the start of analysis Lst, which corresponds to the undeformed geometry state of the components attached through the bolt connector. The bolt's length at zero stress state is calculated from:

L0 = Lst / (1+(P/A*E))

As the nonlinear analysis progresses, the bolt's length Lstep at each analysis step adapts itself to the deformed geometry of the attached components as they deform due to the applied loads. The bolt's final stress at the end of the nonlinear analysis differs from the user-defined pre-load stress. The bolt's axial load at each analysis step is calculated from:

Pstep = A* E* (Lstep - L0) / L0

When this option is checked, the program first runs an analysis with the user-defined pre-load P as initial condition without any external loads. The deformation of the parts connected through the bolt is calculated and is used to determine the bolt's length at zero stress state L0. Let us define Lf as the deformed length of bolt that corresponds to the settlement of the connecting parts due to prestress. The bolt’s length at zero stress is then calculated from:

L0= Lf / (1+(P/A*E))

For the second step of the analysis, all applied loads are included. The bolt's axial load at each analysis step is calculated from:

Pstep = A* E* (Lstep - L0) / L0

During the analysis, if (a) Lstep <= L0 then the bolt is loose, and if (b) Lstep > L0, the bolt is under tension and keeping parts together.

Notation:
  • P: User-defined axial pre-load
  • Pstep: Axial load of bolt at current analysis step
  • A: Bolt section area
  • E: Bolt material modulus of elasticity
  • L0: Original length of bolt at zero stress state
  • Lst: Length of bolt at start of analysis (corresponds to the undeformed geometry state of the components attached through the bolt)
  • Lf: Deformed length of bolt after settlement of connecting parts due to prestress (Keep bolt-prestress selected)
  • Lstep: Deformed length of bolt at current analysis step

Solver

Sets the solver to use in performing nonlinear analysis.

Automatic solver selection The program selects the most robust between two solvers depending on the size of the model and available RAM:

Intel Direct Sparse

For small and medium size models with slim geometry. The Intel Direct Sparse solver requires more RAM than the FFEPlus Iterative Solver.

FFEPlus

For medium-size models with bulky geometry, and large models.
Intel Direct sparse Use the Intel direct sparse solver. This solver has more chances of convergence for highly nonlinear problems.
FFEPlus Use the FFEPlus iterative solver. This solver is less demanding on memory. It maybe faster for large problems.
Large Problem Direct Sparse The Large Problem Direct Sparse solver, by leveraging enhanced memory-allocation algorithms, can handle cases where the solution is going out of core.
Contact penalty stiffness scale factor Specifies a scale factor for the penalty stiffness for the surface-to-surface contact interactions.

To reach a precise solution for nonlinear static studies with many surface-to-surface contact interactions, use 1.0 for the penalty stiffness factor.

To assess design iterations and the overall behavior of a model, specify a value lower than 1.0 to obtain an approximate solution faster.

When you select the FFEPlus solver and the Node-to-surface contact formulation, the solver automatically switches the contact formulation to Surface-to-surface (FFEPlus does not support the Node-to-surface formulation). The Contact penalty stiffness scale factor is always active for the FFEPlus solver, regardless of the selection of contact formulation.

The function of the contact penalty stiffness is analogous to a constant spring stiffness, which relates a contact force to the distance of penetration. The contact penalty stiffness is active only when a penetration is detected from the previous contact iteration. The contact iterations continue until the external loads and contact forces reach an equilibrium.

Save Results

Save results to 3DEXPERIENCE

Saves the simulation results with the associated SOLIDWORKS model on the 3DEXPERIENCE platform in a storage area known as a collaborative space.

After saving SOLIDWORKS Simulation results along with the associated SOLIDWORKS model on the 3DEXPERIENCE platform, you can search for these database objects in the collaborative space in which they are saved, and download them directly in SOLIDWORKS.

See also Saving SOLIDWORKS Simulation Results on the 3DEXPERIENCE Platform.

The option to save simulation results (.cwr) files on the 3DEXPERIENCE platform is available only when you activate the appropriate 3DEXPERIENCE SOLIDWORKS role.
Save Results to disk Saves the simulation results (*cwr) file to your local disk drive.
Save results to SOLIDWORKS document folder Saves the simulation results (*cwr) file to the same local folder where the associated SOLIDWORKS model is stored.
Select a folder to store the results file Selects a folder path to save the simulation results (*cwr) file. The selected folder path is shown in Results folder.
The location you enter here overwrites the default result folder location set in Default Options > Results.

Average stresses at mid-nodes (high-quality solid mesh only)

Select this option to get better stress results when irregular high stresses occur at midside nodes of high-quality solid elements that are located at areas with steep curvature.

For a high-quality solid element, the stresses at the midside nodes are calculated by averaging the stress values of the nearest corner nodes. An example of the stress-averaging scheme is shown.
  • Stresses at corner nodes (1, 2, 3, and 4) globally averaged over the shared elements.
  • Stresses at midside nodes (5, 6, 7, 8, 9, and 10) averaged over the nearest corner nodes. For example, stress (node 5) = (stress (node 1) + stress (node 2)) / 2