Solution Step dialog box (Abaqus), Implicit Dynamic Step Setup page

For Abaqus Structural and Axisymmetric solutions with an Implicit Dynamic step.

Dynamic Stress/Displacement Step Parameters
Time Duration of Step	Specifies the total time allowed for the step.
Time Incrementation	Controls how Abaqus divides the time within a step into increments in a quasi-static analyses.AutomaticSpecifies automatic time incrementation. Abaqus automatically adjusts the size of the time increments to solve the problem efficiently.FixedSpecifies fixed time incrementation. You directly control the time incrementation through the step.The software writes the DIRECT parameter to your Abaqus input file. If no contact impacts or releases occur during the solution, Abaqus uses the time increment data you specify during the step.
Initial Time Increment	Appears when Time Incrementation is set to Automatic.Specifies the suggested initial time increment.
Minimum Time Increment	Appears when Time Incrementation is set to Automatic.Specifies the minimum time increment allowed. If Abaqus needs a smaller time increment than this value, the solve terminates.If you specify a value of 0, Abaqus uses a value that is either the smaller of the suggested initial time increment or 10–5 times the time period of the step.
Maximum Time Increment	Appears when Time Incrementation is set to Automatic.Specifies the maximum time increment allowed. If you do not specify a value, Abaqus does not impose any upper limit on the time increment. If you specify a value of 0, the default that Abaqus uses depends on the option you select from the Application Type list.
Time Increment Size	Appears when Time Incrementation is set to Fixed.Specifies the amount of time for each increment.
Optional General Implicit Step Parameters
Perform Adiabatic Stress Analysis	Specifies whether to perform adiabatic stress analysis.
Application Type	Controls time integration.DefaultApplies the appropriate default method.Transient FidelityApplies a method with slight numerical damping. This is the Abaqus default option for solutions that do not contain contact conditions.Moderate DissipationApplies a method with moderate numerical damping and a more aggressive time incrementation scheme. However, some solution accuracy may be lost. This method is the default method for solutions that include contact. Quasi-StaticApplies a method with significant numerical that is primarily intended to obtain quasi-static solutions.
Time Integration Method	Specifies a time integration method.DefaultApplies the appropriate default time integration method.Backward EulerSpecifies the Backward Euler time integration method.Hilbert-Hughes-Taylor, Slight Numerical DampingSpecifies the Hilber-Hughes-Taylor time integration method. This method applies slight numerical damping to the solution.Hilbert-Hughes-Taylor, Moderate Numerical DampingSpecifies the Hilber-Hughes-Taylor time integration method. This method applies moderate numerical damping to the solution.
Alpha	Appears when Time Integration Method is set to Hilbert-Hughes-Taylor, Slight Numerical Damping or Hilbert-Hughes-Taylor, Moderate Numerical Damping.Lets you specify a value for α for the numerical (artificial) damping control parameter. Enter a value between 0, which indicates no damping, to –0.5. A value of -0.333 provides maximum damping.
Beta	Appears when Time Integration Method is set to Hilbert-Hughes-Taylor, Slight Numerical Damping or Hilbert-Hughes-Taylor, Moderate Numerical Damping.Lets you specify a value for β in the implicit operator. Specify a positive value.
Gamma	Appears when Time Integration Method is set to Hilbert-Hughes-Taylor, Slight Numerical Damping or Hilbert-Hughes-Taylor, Moderate Numerical Damping.Lets you specify a value for γ in the implicit operator. Specify a value greater than or equal to 0.5.
Time Incrementation Type	Specifies the general time incrementation type.DefaultApplies the appropriate default time incrementation type.AggressiveSpecifies a time incrementation scheme based only on convergence history. This option is similar to a scheme typically used in static problems without rate or history dependence. ConservativeSpecifies a time incrementation scheme that maximizes solution accuracy.
Time Incrementation Involving Contact	Specifies the type of time incrementation to use when contact impacts or releases occur during the analysis.DefaultApplies the appropriate default time incrementation type.NoSpecifies a marching through scheme without impact or release cut backs and without velocity or acceleration compatibility computations.Average TimeSpecifies a time incrementation scheme that employs average time of impact or release cut backs to enforce energy balance and maintain velocities and accelerations compatible on the active contact interface.Current TimeSpecifies a marching through scheme without impact or release cut backs. The velocities and accelerations are compatible on the active contact interface.
Bypass Calculation of Initial Accelerations at Beginning of Step	Appears when Time Incrementation is set to Fixed.Controls whether Abaqus calculates or recalculates accelerations at the beginning of the step.Select the Bypass Calculation of Initial Accelerations at Beginning of Step check box to calculate accelerations.Clear the Bypass Calculation of Initial Accelerations at Beginning of Step check box if you do not want to calculate accelerations. With this option, the software assumes that the initial accelerations for the current step are zero if the current step is the first Implicit Dynamic step in the solution. If the preceding step is also an Implicit Dynamic step, then the software uses the accelerations from the end of the previous step to continue the new step. This is appropriate only if the loading does not change suddenly at the start of the new step.
No Check Of Half-Increment Residual	Appears when Time Incrementation is set to Fixed.Suppresses the calculation of the half-increment residuals. This can reduce solve time because the software skips some accuracy checking for the automatic time incrementation scheme. This option corresponds to the NOHAF parameter for the *DYNAMIC keyword.
Ignore Convergence Tolerance After Max. Number Of Iterations Is Reached	Appears when Time Incrementation is set to Fixed.Controls whether the solution is accepted after the maximum number of allowed iterations is reached.
Half-Increment Residual	Appears when Time Incrementation is set to Automatic.Controls the calculation of half-increment residuals. The half-increment residual is the equilibrium residual error (out-of-balance forces) halfway through a time incrementDefaultAbaqus does not write any half-increment residual parameters to the solver input file.No CheckSuppresses the calculation of the half-increment residuals, which can reduce solution time because Abaqus skips some accuracy checking for the automatic time incrementation scheme. This option corresponds to the NOHAF parameter for the *DYNAMIC keyword. Force ToleranceSets the half-increment residual tolerance to use with the automatic time incrementation scheme. This option corresponds to the HAFTOL parameter for the *DYNAMIC keyword.Scale FactorApplies a scale factor to the calculated time average force and moment values to use as the half-increment residual tolerance with the automatic time incrementation solution accuracy checking scheme. This option corresponds to the HALF INC SCALE FACTOR parameter for the *DYNAMIC keyword.
Half Increment Residual Force Tolerance	Appears when Half Increment Residual is set to Force Tolerance.Sets the half-increment residual tolerance to be used with the automatic time incrementation scheme.This option corresponds to the HAFTOL parameter for the *DYNAMIC keyword.
Scale Factor of Time Average Force	Appears when Half Increment Residual is set to Scale Factor.Specifies the appropriate scale factor tolerance.
Diagnosis for Errors Associated with Mass Properties	Controls how Abaqus makes velocity and acceleration adjustments if it a singular global mass matrix during initialization or during contact impact/release computations.Error MessageAbaqus issues an error message and stop execution if a singular global mass matrix is detected when calculating the velocity and acceleration adjustments.Warning MessageAbaqus issues a warning message and avoids these velocity and acceleration adjustments. Abaqus continues the time integration using the current velocities and accelerations if it detects a singular global mass matrix.Make AdjustmentsAbaqus adjusts velocities and accelerations even if a singular mass matrix is detected. This setting can result in large, non-physical velocity and acceleration adjustments. This can cause poor time integration solutions and artificial convergence difficulties. This approach is not generally recommended.This option corresponds to the SINGULAR MASS parameter for the *DYNAMIC keyword.

Look up more details

Solution Step dialog box tabs (Abaqus)

Solution Step dialog box (Abaqus), Change Friction page

Solution Step dialog box (Abaqus), Complex Eigenvalue Extraction

Solution Step dialog box (Abaqus), Control Parameters page

Solution Step dialog box (Abaqus), Dynamic Coupled Heat Transfer and Stress Setup Step page

Solution Step dialog box (Abaqus), Cyclic Symmetry Modes page

Solution Step dialog box (Abaqus), Cyclic Step Setup page

Solution Step dialog box (Abaqus), Data Line page

Solution Step dialog box (Abaqus), Coupled Heat Transfer and Stress Setup Step page

Solution Step dialog box (Abaqus), Explicit Dynamic Step Setup page

Solution Step dialog box (Abaqus), General page

Solution Step dialog box (Abaqus), Heat Transfer Setup page

Solution Step dialog box (Abaqus), Mass Scaling page

Solution Step dialog box (Abaqus), Other Step Options page

Solution Step dialog box (Abaqus), Other Step Parameters page

Solution Step dialog box (Abaqus), Output page

Solution Step dialog box (Abaqus), Steady-State Modal Dynamic Step Parameters page

Solution Step dialog box (Abaqus), Transient Modal Dynamic Step Setup page

Solution Step dialog box (Abaqus), User Defined Text page

Solution Step dialog box (Abaqus), Visco Step Setup page

Solution Step dialog box (Abaqus), Implicit Dynamic Step Setup page, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });