Unit Systems

OptiStruct runs are typically unit agnostic, that is, you do not need to explicitly specify the unit system in which the model is defined. Instead, units are incorporated indirectly within the model, for instance, using the material data and associating it with the model dimensions.

Generally, you should specify input data based on a consistent units system for an OptiStruct run. Refer to Consistent System of Units for more information.

In certain conditions, it may be necessary to explicitly specify the unit systems for the run. A few such instances are:
  • Multibody Component Mode Synthesis (CMSMETH with CC or CB flex body generation)

    When CMS flex body generation is used to output a flexible body to be used subsequently in a different solver, say,MotionSolve, then it is important to identify the units associated with the flex body. This can be done using the DTI,UNITS Bulk Data Entry or the equivalent UNITS I/O Entry.

  • Flexbody H3D generation for MotionSolve

    The units in which the model has been defined should be mentioned on the DTI,UNITS entry. The CMS flexbody (CC and CB options on CMSMETH Bulk Data Entry) will always be output in the units of Kilogram, Newton, millimeter, second. Units for the flex H3D output are always fixed and if you identify the model as having units different from this on DTI,UNITS entry, then OptiStruct converts the output units from the units mentioned on DTI,UNITS to Kg,N,mm,s when generating the flex h3d file.

    MotionSolve will always expect the flex h3d file to be generated with the Kg,N,mm,s units set.
    Note: This unit set is not a consistent set of units.

    If you specify a different set of units for the multibody model inside MotionSolve, then MotionSolve will convert the flex body h3d from Kg,N,mm,s to the user-defined units for the multibody run.

  • Explicit Dynamic Analysis (via Radioss Integration – EXPDYN)

    When Explicit Dynamic Analysis is run by using ANALYSIS=EXPDYN subcase to integrate with Radioss, it is important to clearly identify the unit system of the OptiStruct model. This is accomplished by using the DTI,UNITS Bulk Data Entry or the equivalent UNITS I/O Entry.

  • Fatigue Analysis
    Fatigue analysis in OptiStruct uses the stress results coming from a preceding analysis run (for instance, Linear Static), to perform some fatigue calculations and output corresponding Fatigue Life and Damage results. There are multiple sections within the Fatigue module which requires explicit understanding of the unit system of the model:
    Identifies the units of the stress tensor coming from the preceding FE analysis. This is necessary because the SN/EN curve (on FATPARM entry) may be defined in a different unit system compared to the stress coming from analysis. Therefore, the stress should be converted prior to looking up the fatigue life for a given stress level on the SN curve. If UNITS or DTI,UNITS is present, the default value of STRESSU is determined by UNITS or DTI,UNITS entry (UNITS takes precedence over DTI,UNITS). If UNITS, DTI,UNITS, and STRESSU are not provided, the default value of STRESSU is MPa. If UNITS or DTI,UNITS is present, and STRESSU is specified, but they are not consistent, then an error will be issued.
    Identifies the units of stress values defined on the Yield Strength (YS), Ultimate Tensile Strength (UTS), SRI1, Fatigue Limit (FL), Sf, and Kp fields on the MATFAT entry.
    This is applicable to the stress gradient effect for the GRDFKM method.
    This informs the fatigue module what units the model is in and based on this, it will be able to calculated the stress gradient effect for the GRDFKM method by locating the 1 mm depth necessary for the calculations.
    This is applicable to the GRDCD method.
    This informs the fatigue module the units in which the critical distance value defined on the CRTDIS field is input.
    LENUNIT is based on the Stress units on FATPARM by default. If the model has MPA units for Stress, then the model is in units of mm.
  • Aeroelastic Trim Analysis

    Accelerations are specified by default in units of gravity (g’s) on the TRIM Bulk Data Entry. These can be converted into other units (for instance, m/s2) using the PARAM, AUNITS entry.

  • Sound Pressure

    For sound pressure level (SPL) calculations in Decibels, the reference sound pressure value is defined via the PARAM, SPLREFDB entry. The units of the reference sound pressure is specified on the UNITS I/O Options Entry.

  • Radiation Heat Transfer Temperature

    The units of temperature for Radiation Heat Transfer is assumed to be Kelvin, and based on this default, the value of PARAM, SIGMA can be set equal to the SI unit value of the Stefan-Boltzmann constant.

    Since input temperatures and SIGMA should be defined in consistent units, the PARAM, TABS can be used if the input temperatures are in Celsius or in Fahrenheit.

  • SIMPACK flex body generation

    Similar to the discussion regarding flex body generation for MotionSolve, the DTI,UNITS entry can be used to specify the units during the creation of the SIMPACK flex body via PARAM, SIMPACK.

  • Aeroelastic Flutter Analysis

    The velocities in Aeroelastic Flutter Analysis are divided by the value specified on PARAM, VREF. This can be used to convert the velocity units.