Load step options refer collectively to options controlling how loads are used during solution, and other options such as output controls, damping specifications, and response spectrum data. Load step options can vary from load step to load step.
Several categories of load step options are available:
These include such options as time at the end of a load step in transient and static analyses, number of substeps or the time step size, stepping or ramping of loads, and reference temperature for thermal strain calculations. A brief description of each option follows.
The TIME command specifies time at the end of a load step in transient and static analyses. In transient and other rate-dependent analyses, TIME specifies actual, chronological time, and you are required to specify a time value. In other, rate-independent analyses, time acts as a tracking parameter. You can never set time to zero in an analysis. If you issue TIME,0 or TIME,(blank), or if you do not issue the TIME command at all, the program uses the default time value: 1.0 for the first load step, and 1.0 + previous time for other load steps. To start your analysis at "zero" time, such as in a transient analysis, specify a very small value such as TIME,1E-6.
For a nonlinear or transient analysis, specify the number of substeps to be taken within a load step via the DELTIM and NSUBST commands.
NSUBST specifies the number of substeps, and DELTIM specifies the time step size. By default, the program uses one substep per load step.
The AUTOTS command activates automatic time stepping.
In automatic time stepping, the program calculates an optimum time step at the end of each substep, based on the response of the structure or component to the applied loads. When used in a nonlinear static (or steady-state) analysis, AUTOTS determine the size of load increments between substeps.
When specifying multiple substeps within a load step, indicate whether the loads are to be ramped or stepped by issuing the KBC command. KBC,0 indicates ramped loads, and KBC,1 indicates stepped loads. The default depends on the discipline and type of analysis.
Note: There is a third option specific to rotational velocity loads
(OMEGA, CMOMEGA, and
CMROTATE). The load can be quadratically interpolated
(OMGSQRD on KBC). For
more information, see Ramped and Stepped Loads.
The concept of stepped versus ramped loading does not apply to temperature-dependent film coefficients (input as -N on a convection command). These are always applied at the value dictated by their temperature function.
Consider the following when issuing the KBC command:
Stepped loads:
The program handles all loads (constraints, forces, surface loads, body loads, and inertia loads) in the same manner. They are step-applied, step-changed, or step-removed, as the case may be.
Ramped loads:
All loads applied in the first load step, except film coefficients, are ramped (either from zero or from the value specified via BFUNIF or its GUI equivalent, depending on the type of load; see Table 3.12: Handling of Ramped Loads (KBC = 0) Under Different Conditions). Film coefficients are step-applied.
All loads changed in later load steps are ramped from their previous values. If a film coefficient is specified using the temperature-dependent format (input as -N) for one load step and then changed to a constant value for the next step, the new constant value is step-applied. Note that in a full harmonic analysis (ANTYPE,HARM with HROPT,FULL), surface and body loads ramp as they do in the first load step and not from their previous values.
For tabular boundary conditions, loads are never ramped but rather evaluated at the current time. If a load is specified using the tabular format for one load step and then changed to a non-tabular for the next, the load is treated as a newly introduced load and ramped from zero or from BFUNIF and not from the previous tabular value.
All loads newly introduced in later load steps are ramped (either from zero or from BFUNIF, depending on the type of load; see Table 3.12: Handling of Ramped Loads (KBC = 0) Under Different Conditions).
All loads deleted in later load steps are step-removed, except body loads and inertia loads. Body loads are ramped to BFUNIF. Inertia loads, which you can delete only by setting them to zero, are ramped to zero.
Do not delete and respecify loads in the same load step; otherwise, ramping may lead to unpredictable results.
Table 3.12: Handling of Ramped Loads (KBC = 0) Under Different Conditions
| Load Type | Applied in Load Step 1 | Introduced in Later Load Steps |
|---|---|---|
| DOF Constraints | ||
| Temperatures | Ramped from TUNIF[2] | Ramped from TUNIF[3] |
| Others | Ramped from zero | Ramped from zero |
| Forces | Ramped from zero | Ramped from zero |
| Surface | ||
| TBULK | Ramped from TUNIF[2] | Ramped from TUNIF |
| HCOEF | Stepped | Ramped from zero[4] |
| Others | Ramped from zero | Ramped from zero |
| Body | ||
| Temperatures | Ramped from TUNIF[2] | Ramped from previous TUNIF[3] |
| Others | Ramped from BFUNIF[5] | Ramped from previous BFUNIF[3] |
| Inertia [1] | Ramped from zero | Ramped from zero |
Rotational velocity loads (OMEGA, CMOMEGA) are ramped linearly; the resulting forces vary quadratically over the load step.
The TUNIF command specifies a uniform temperature at all nodes. Because TUNIF (or BFUNIF,TEMP) is step-applied in the first iteration, issue a BF,ALL,TEMP,
Valuecommand to ramp on a uniform temperature load.In this case, the TUNIF or BFUNIF value from the previous load step is used, not the current value.
Temperature-dependent film coefficients are always applied at the value dictated by their temperature function, regardless of the KBC setting.
The BFUNIF command is a generic form of TUNIF, meant to specify a uniform body load at all nodes.
You can also specify the following general options:
The reference temperature for thermal strain calculations, which defaults to zero degrees (TREF).
Whether a new factorized matrix is required for each solution (that is, each equilibrium iteration) KUSE). You can do this only in a static (steady-state) or transient analysis.
By default, the program decides whether a new matrix is required, based on such things as changes in DOF constraints, temperature-dependent material properties, and the Newton-Raphson option. If KUSE is set to 1, the program reuses the previous factorized matrix. This setting cannot be used during a multiframe restart. KUSE,-1 forces the factorized matrix to be reformulated at every equilibrium iteration. Analyses rarely require this; you use it mainly for debugging purposes.
To generate and keep the sparse solver workspace files (Jobname.DSP
xxxx), issue the command EQSLV,SPARSE,,,,KEEP command.A mode number (the number of harmonic waves around the circumference) and whether the harmonic component is symmetric or antisymmetric about the global X axis (MODE). When you use axisymmetric harmonic elements (axisymmetric elements with nonaxisymmetric loading), the loads are specified as a series of harmonic components (a Fourier series).
The type of scalar magnetic potential formulation to be used in a 3D magnetic field analysis (MAGOPT).
The type of solution to be expanded in the expansion pass of a mode-superposition analysis (NUMEXP, EXPSOL).
These are options used primarily in dynamic and other transient analyses:
Table 3.13: Dynamic and Other Transient Analyses Commands
| Command | Purpose |
|---|---|
| TIMINT | Activates or deactivates time integration effects |
| HARFRQ | Specifies the frequency range of the loads in a harmonic analysis |
| ALPHAD | Specifies damping for a structural dynamic analysis |
| BETAD | Specifies damping for a structural dynamic analysis |
| DMPRAT | Specifies damping for a structural dynamic analysis |
| MDAMP | Specifies damping for a structural dynamic analysis |
| TRNOPT | Specifies transient analysis options |
Three primary output controls for specifying the amount and nature of output from an analysis are shown in this table:
Table 3.15: Output Controls Commands
| Command | Purpose |
|---|---|
| OUTRES | Controls what the program writes to the database and results file and how often it is written. |
| OUTPR | Controls what is printed (written to the solution output file, Jobname.out) and how often it is written. |
| OUTGEOM | Controls the type of geometry data the program writes to the results file. |
The example below illustrates using OUTRES, OUTPR, and OUTGEOM:
OUTRES,ALL,5 ! Writes all data every 5th substep OUTPR,NSOL,LAST ! Prints nodal solution for last substep only OUTGEOM,MAT,NONE ! Suppresses the writing of the material property data to the results file
You can issue a series of OUTPR, OUTRES, and OUTGEOM commands (up to 50 of them combined) to meticulously control the solution output, but be aware that the order in which they are issued is important. For example, the commands shown below write all data to the database and results file every 10th substep and nodal solution data every fifth substep.
OUTRES,ALL,10 OUTRES,NSOL,5
However, if you reverse the order of the commands (as shown below), the second command essentially overrides the first, resulting in all data being written every 10th substep and nothing every 5th substep.
OUTRES,NSOL,5 OUTRES,ALL,10
As another example,
OUTRES,NSOL,10 OUTRES,NSOL,ALL,TIP
writes the solution at all DOFs every 10th substep and the solution at the node component TIP every substep. Again, if you reverse these you only obtain output at all DOF every 10th substep.
The program default for writing out solution data for all elements depends on the analysis type. See the OUTRES command description for more information.
To restrict the solution data that is written out, use OUTRES
to selectively suppress (Freq = NONE) the writing of
solution data, or first suppress the writing of all solution data
(OUTRES,ALL,NONE) and then selectively turn on the writing of
solution data with subsequent OUTRES commands.
The OUTGEOM command is used to either write or suppress the geometry data from the results file for all substeps. The only valid frequency specification for this command are ALL and NONE. See the OUTGEOM command description for more information.
Another output control command, ERESX, enables you to review element integration point values in the postprocessor.
By default, the program extrapolates nodal results that you review in the postprocessor from integration point values for all elements except those with active material nonlinearities (for instance, nonzero plastic strains).
By issuing ERESX,NO, you can turn off the extrapolation and instead copy integration point values to the nodes, making those values available in the postprocessor.
ERESX,YES forces extrapolation for all elements, whether or not they have active material nonlinearities.
These options are used in a magnetic field analysis:
For more information, see the Low-Frequency Electromagnetic Analysis Guide.
Many commands are available in this category, all meant to specify response spectrum data and power spectral density (PSD) data. Use the commands in spectrum analyses, as described in the Structural Analysis Guide.