HyperX analysis requires element forces, pressures, and temperatures to be output to the results file. Nodal displacements are not required for analysis but can be used to visualize deformation in the FEM Viewer form.
|
Solver |
Supported Results Format |
|---|---|
|
MSC Nastran |
*.OP2, *.F06 |
|
NX Nastran |
*.OP2, *.F06 |
|
OptiStruct |
*.OP2 |
|
Autodesk Nastran |
*.OP2, *.ELS |
|
Abaqus |
*.FIL, *.ODB |
MSC Nastran & NX Nastran, OptiStruct
Both the F06 (ASCII) and OP2 (binary) results file formats are supported for MSC Nastran, NX Nastran, and OptiStruct. The OP2 format is more compact than the F06 which results in quicker FEA solution times, smaller file sizes, and quicker import into HyperX. For these reasons, the OP2 is recommended for large models.
OUTPUT2 (OP2) Example
Using the OUTPUT2 format requires the use of the PLOT modifier as well as the PARAM,POST,-1 bulk data entry. The PARAM,POST,-1 entry is typically included in most FEM preprocessors by default.
INIT MASTER(S)
SOL SESTATIC
CEND
TITLE = Wing box
ECHO = NONE
FORCE(PLOT) = ALL
$ For OPTISTRUCT this command is ELFORCE(OUTPUT2) = ALL
DISPLACEMENT(PLOT) = ALL
$ For OPTISTRUCT this command is DISPLACEMENT(OUTPUT2) = ALL
SUBCASE 101
SUBTITLE = Wing Pressure
SPC = 100
LOAD = 101
SUBCASE 201
SUBTITLE = Wing Temperature
SPC = 100
TEMP(LOAD) = 201
BEGIN BULK
PARAM,POST,-1
F06 Example
The most common method is to specify the FORCE(PRINT) = ALL and DISP(PRINT) = ALL command before the subcase definitions. FORCE=ALL is valid, but this is not recommended for large models due to the potential for redundant output to the OP2 file. SORT2 is not supported.
INIT MASTER(S) $ Required so that Nastran deletes temporary files after each run.
SOL SESTATIC
CEND
TITLE = Wing box
ECHO = NONE
FORCE(PRINT) = ALL
DISPLACEMENT(PRINT) = ALL
SUBCASE 101
SUBTITLE = Wing Pressure
SPC = 100
LOAD = 101
SUBCASE 201
SUBTITLE = Wing Temperature
SPC = 100
TEMP(LOAD) = 201
BEGIN BULK
Supported Solution Sequences
|
101 |
Linear Static |
|
103 |
Modal |
|
105 |
Buckling |
|
106 |
Non-Linear Static |
|
112 |
Modal Transient Response |
|
400 |
Non-Linear Static and Dynamic (implicit) |
Note
For solutions for multiple load steps per subcase, only the last load step is used.
Autodesk Nastran
For Autodesk Nastran, the standard Nastran OP2 format is supported. Additionally, the Autodesk Nastran element results neutral file format (ELS) and the grid point results neutral file format (DIS) are also supported (binary only).
In the Autodesk Nastran Editor or Nastran.INI file, use the RSLTFILETYPE output control directive to control which format is exported.
|
Format |
RSTLTFILTYPE |
|---|---|
|
OP2 |
NASTRANBINARY |
|
ELS, DIS |
NORANBINARY |
The bulk data file format is shown below.
SOL SESTATIC
CEND
TITLE = Wing box
ECHO = NONE
FORCE(PLOT) = ALL
DISPLACEMENT(PLOT) = ALL
SUBCASE 101
SUBTITLE = Wing Pressure
SPC = 100
LOAD = 101
SUBCASE 201
SUBTITLE = Wing Temperature
SPC = 100
TEMP(LOAD) = 201
BEGIN BULK
PARAM,POST,-1
Supported Solution Sequences
|
101 |
Linear Static |
|
103 |
Modal |
|
105 |
Buckling |
Note
For solutions for multiple load steps per subcase, only the last load step is used.
Abaqus
Abaqus FEA results are imported using either the .ODB or .FIL results files.
Each step definition needs to contain the proper output options. All steps should output the centroidal element forces (SF), element pressures (LOADS), element temperatures (TEMP), and nodal displacements (U). Output requests do not need to be repeated for each step provided they are the same as the previous step.
Although the results file is not exposed in Abaqus/CAE, the required keywords can be input using Model | Edit Keywords.
Use linear perturbation steps to run multiple load conditions in a single input file.
The Abaqus commands to print the section forces and displacements output to the .FIL file are shown below. HyperX v7.3.20 and newer also support the .odb output.
*Step, Name=Wing_Pressure_101, Perturbation
*Dsload
...
*El File, Position=Centroidal
SF
*El File
LOADS
*El File
TEMP
*Node File
U
*End Step
**
** ------------------------------------------- **
**
*Step, Name=Fuselage_Pressure_102, Perturbation
*Dsload
...
** No output requests are necessary for subsequent steps.
*End Step
Abaqus steps that use the *STATIC, *DYNAMIC, *BUCKLE, or *FREQUENCY options are supported for linear or non-linear analysis. For each step, HyperX will pull loads from the FEA results corresponding to the last increment in each step. The last increment always corresponds to the time period of the step.
When pressure is applied to finite element models, secondary bending effects can be missed due to insufficient mesh resolution. HyperX has the ability to import pressure loads in order to perform an "offline" pressure deflection analysis to capture this effect.
In Nastran, pressure loads are imported from the input file. In Abaqus, pressures are imported from the results files.
For offline pressure analysis, HyperX computes the average element pressure load for each zone. Then the reaction moments and shear loads caused by the pressure are superimposed on the FEA loads. This process is done for each load set. See Superimposed Loads.
Nastran, Optistruct
Element pressure loads are imported from PLOAD4 entries in the input file. In Nastran, multiple PLOAD4 cards from the same load set are additive. Meaning that, if more than one pressure load is encountered for an element, the pressures are added together.
Double Recording Nastran Pressure Loads
A problem arises if pressure loads are used for the finite element model as well as the offline pressure analysis. This results in doubly recording the pressure induced response. To avoid this problem, use the following procedure to import the pressure loads into HyperX while removing them from the finite element model.
-
Cut all PLOAD4 entries from the FEM file and paste them into a new "pressure" file (model.pload).
-
Save the pressure file in the same directory as the FEM input file (model.bdf). Use an include statement in the input file to call the pressure file.
-
Comment out the pressure include statement to run FEA. This will prevent the FEA solution from returning any shear and moment loads resulting from the external pressure loads.
-
Uncomment the pressure include statement in the FEM for import into HyperX.
-
Import the model into HyperX.
-
Comment out the pressure include statement again to prepare the model for iteration with HyperFEA.
Abaqus
Abaqus pressure loads (DLOAD and DSLOAD) are imported using the results file; use the EL FILE with the LOAD option. See Supported Results Formats.
Thermal mismatch between ply layers can cause residual stresses that are not captured by FEA. Also, the operating temperature of a structure directly impacts the material properties used when performing stress and failure analysis. For these reasons, thermal loads (element temperatures and temperature gradients) are imported into HyperX.
Nastran
For Nastran, TEMPP1 and TEMPRB entries are imported for shell and beam elements respectively. These entries are used to define the element temperature and through-thickness temperature gradients for material properties and offline thermal stress calculations.
Abaqus
For Abaqus, temperatures are read from the results file using the EL FILE with the TEMP option. See Supported Results Formats.