Geometry Importation

StressCheck provides a facility for importing CAD geometry that may be used as the basis for the construction of a finite element model, as well as importation of other data types such as NASTRAN mesh, point load and constraint data, StressCheck legacy input files and StressCheck parameters. Currently supported CAD import formats include Parasolid, Unigraphics, CATIA V4 and V5/V6, Pro/E, STEP and IGES according to the following detail.

Parasolid and Unigraphics

Parasolid is StressCheck Professional’s native CAD format. Supported Parasolid file extensions include: *.x_t and *.prt (extension *.prt must be changed to *.ug to avoid conflict with Pro/E files). Supported Parasolid versions include 9.0 to 32.1.

Unigraphics Part (*.prt) files may be a single part or an assembly. Supported Unigraphics versions include v11 to v18, NX1 to NX5.

CATIA V4 and V5

Supported file extensions for CATIA V4 include: *.model, *.session and *.exp for versions 4.1.9 to 4.2.4. Supported file extensions for CATIA V5 include: *.CATPart, *.cgr, and *.CATProduct for versions V5 R8 to V5-6 R2021.

3DExperience (CATIA V6)

Supported file extensions for 3DExperience (CATIA V6) include: *.CATPart and *.CATProduct for versions up to V6 R2021.

Pro/E and Creo

Supported Pro/E file extensions include: *.prt , *.asm, *.xpr, *.xas for versions 16 to Creo 7.0. Note: before attempting to import Pro/E files with extension *.prt.* or *.asm.*, the extensions for these files must be changed to *.prt or *.asm.

STEP

File extensions *.stp and *.step for versions AP203, AP214 and AP242 are supported.

IGES

File extensions *.igs and *.iges for versions up to 5.3 are supported.

Importing CAD Geometry

Use the File > Import menu option, then set the file filter to identify which type of file you wish to import. A warning will be issued to make sure the Units setting in StressCheck is consistent with those of the model to be imported:

If the units are not consistent, then change the Unit selector before proceeding.

The type of file to be imported is determined by the file extension, so if the file extension of your file does not match one of those provided in the filter selector, you must change the file extension on your file to match one of the options provided. More than one file can be imported at once, simply hold the Ctrl key while selecting all the files to be imported, and then click on Open.

As each file is imported, the native CAD file format is translated into a Parasolid representation, and the result is displayed in the Model View. Although the model may have been parametric in the native CAD system, it is imported with static dimensions, and with no feature information. It is not possible to change dimensions or to alter any of the relationships between various components in the solid model. On the other hand, it is possible to add new details to the model using boolean, blend, and clipping operations provided in StressCheck, as well as move the geometry to another location and/or orientation via Body-Copy operations. And, of course, you may construct a geometrically associative finite element model using the solid model as the basis.

When importing CAD geometry, it is always a good practice to check if the imported CAD bodies are valid. To check, go to the Geometry tab in Input dialog, set the A/O/M combo-boxes to Check > Any Body and select the CAD geometry. The selected body will turn gray if valid. If it is invalid, it will turn green wireframe and highlight the problem areas in red. Invalid bodies are less likely to be automeshed. These problem areas must be corrected in the native CAD tool.

Exporting CAD Geometry

StressCheck provides a facility for exporting its part geometry to 3rd party CAD systems using the File > Export menu option. StressCheck’s geometry may be exported to Parasolid or IGES formats. The geometry exported from StressCheck will represent a static snapshot of the model in the current Units, and will not provide parametric or feature level information to the receiving CAD system.

An ASCII *.stl file (known as a stereo lithography or a standard tessellation language format) can be exported from StressCheck using File > Export. This exports whatever element faces are currently shown in the Model View, whether undeformed or deformed. The resolution of the exported file can be controlled with the Edge Resolution option in the View Controls window.

Mesh Importation

StressCheck supports the importation of finite element meshes generated by other analysis tools and saved in NASTRAN bulk data format (*.bdf), as well as *.nas and *.dat formats. The current StressCheck implementation supports the importation of coordinate systems, material properties, nodal forces, nodes (grid points), and planar/solid elements.

StressCheck also supports the importation of LS-Dyna (*.k) files for initial stress mapping purposes, and Simmetrix MeshSim mesh data files (*.sms) for importation of MeshSim-generated meshes.

If more than one file is imported during a StressCheck session, or if the importation is performed after some geometric or mesh entities were created in StressCheck, then the program will automatically offset the grid points and element numbers of the imported objects to avoid conflict with existing objects.

For an example of mesh importation, refer to Helpful Hints and Tips: Application of TLAP Bearing to HyperMesh Import.

NASTRAN

When importing NASTRAN files, the importation of linear or quadratic (midside node) 2D and 3D elements is supported. Other cards, such as 1D elements (e.g. rods, beams) and loads/constraints, will be ignored.

LS-Dyna

LS-Dyna ASCII keyword files (*.k ) can be imported into StressCheck. The following keywords are supported:
*KEYWORD, *NODE, *ELEMENT_SOLID, *INITIAL_STRESS_SOLID, *END

When a LS-Dyna file is imported into StressCheck, any INITIAL_STRESS_SOLID data is converted to a StressCheck solution which becomes immediately available for post-processing. If this data is intended to be mapped to a StressCheck mesh as an initial stress state with a BRS load, be sure to create a StressCheck Part and set it as the active part before importing. Then the imported mesh will be put into the part and its solution associated with the part.

MeshSim

Simmetrix MeshSim mesh data files (*.sms) may be imported into StressCheck. If the Parasolid file (*.x_t), used to generate the mesh is imported prior importing the sms file, associativity to the geometry may be recovered. Note this is only possible for meshes that contain midside node elements only.

Importation of Point Loads & Constraints

This section describes how to import point load or point constraint data from global models, available in NASTRAN BDF/NAS/DAT formats, text file format (ASCII) or PATRAN format (CSV), into StressCheck for global-local analysis. To import point load or point constraint data into a StressCheck session, use File > Import. Set the filter to the appropriate format: “NASTRAN Files (*.bdf, *.nas, *.dat)”, “ASCII (*.txt)”, or “PATRAN (*.csv)”. Click “Open” to import the file. A dialog should appear when “Open” is clicked allowing the user to enter “First point #:”, and also “Case ID #” if the type of file is NOT a PATRAN/CSV input file (*.csv). If a PATRAN/CSV input file is selected, StressCheck will obtain the Case ID from the file. The below Figure 1a shows the interface for when “ASCII (*.txt)” is selected as the filter, and Figure 1b shows the interface for when “PATRAN (*.csv)” is selected as the filter:

Note: NASTRAN files containing NASTRAN-format gridpoint point loads can be directly imported, and do not require the Import Point Loads/Constraints interface. Imported NASTRAN point loads may be found under Edit > Point Load Info… Descriptions and examples of how to import point constraints and point loads into StressCheck are given below. Point loads can be running loads (loads per unit length) or total loads at a point (TLAP).

Importation of Point Constraints

Figure 2 shows the displacements (Tx, Ty and Tz) and rotations (Rx, Ry, and Rz) provided in an excel spreadsheet and obtained from the solution of a global shell model. Below are the steps to import point constraints:

• An ASCII text file must be created containing the displacements and rotations together with their corresponding locations and excluding repeated information. This can be accomplished by cutting and pasting the data from the excel file into Notepad and then deleting the repeated records. In Figure 3 the first three columns are the global coordinates of the points, the next three are the translations (Tx, Ty and Tz), and the last three are the rotations (Rx, Ry, and Rz).
• The ASCII text file can be then imported into StressCheck by selecting File > Import, changing the filter to “ASCII (*.txt)”, selecting the ASCII text file and clicking “Open”. Then, in the Import Point Loads/Constraints dialog set the data type to Point Constraints. Click Accept.
  • If the number of columns in the text file is different from nine (9), an error message will be issued indicating the required number of columns and the ones found.
• The imported point constraints can be found under Edit > Point Constraint Info…
  • The Point Constraint Case Definitions dialog (Figure 4) will appear with access to the point constraint objects.

For more information on using imported point constraints, refer to Point Displacements/Rotations Implementation.

Importation of Point Loads per Unit Length (Running Loads)

StressCheck allows importing point load information (forces and moments per unit length) from a global shell model. Note however that the output of global shell models obtained by a free-body approach is in the form of total point load and moments. For example, Figure 5 shows the total point force (Fx, Fy and Fz) and moment (Mx, My, and Mz) components provided in an excel spreadsheet and obtained from the solution of a global shell model. The data are in the global coordinate directions, and force and moment vector components are positive when in the direction of the positive coordinate axes. To import point load data the following steps are needed:

• The total point forces and moments must be converted to forces/moments per unit length. This is accomplished by dividing the magnitude of the force/ moment at each point by a length equal to the sum of half the distance to the two neighboring points at each side.
• An ASCII text file containing the forces and moments per unit length, together with their corresponding location plus the plate thickness must be created excluding repeated information (Figure 6).
  • The data is organized such that the first three columns are the global coordinates, the next three columns are the three components of the point force per unit length followed by the three components of the point moment per unit length, and the last column is the thickness of the plate at the location of the point load.
• The ASCII text file can be then imported into StressCheck by selecting File > Import, changing the filter to “ASCII (*.txt)”, selecting the ASCII text file and clicking “Open”. Then, in the Import Point Loads/Constraints dialog set the data type to Point Loads. Click Accept.
  • If the number of columns in the text file is different from ten (10), an error message will be issued indicating the required number of columns and the ones found.
• The imported point loads can be found under Edit > Point Load Info…
  • The Point Loads Case Definitions dialog (Figure 7) will appear with access to the point loads objects.

For more information on using imported point loads, refer to Point Running Loads Implementation.

Importation of Total Loads at a Point (TLAP)

To import total load at a point (TLAP) data the following steps are needed, depending on if it is in ASCII text format or PATRAN CSV format:

ASCII Format

The following ASCII (.txt) format is supported by StressCheck (Figure 8):

• An ASCII text file containing the total forces and moments must be created excluding repeated information as was done in Figure 6 for the case of point load per unit length.
  • The data is organized such that the first three columns are the global coordinates of the points; the next three columns are the three components of the point force followed by the three components of the point moment. For TLAP the plate thickness can be added to the last column for compatibility with the running load case, but is not required.
  • If the ASCII text (*.txt) file does not contain thickness information, StressCheck will use a unit value since the format for the running loads and TLAP is the same.
• The ASCII text file can be then imported into StressCheck by selecting File > Import, changing the filter to “ASCII (*.txt)”, selecting the ASCII text file and clicking “Open”. Then, in the Import Point Loads/Constraints dialog set the data type to TLAP. Click Accept.
  • The program will accept either 9 or 10 columns in the ASCII file (Figure 8). An error message will be issued if the ASCII file contains fewer than 9 columns or more than 10 columns.
• A message will appear indicating the number of load cases successfully imported by StressCheck, as well as a project log summary of the imported TLAP loads by Case ID.
• The imported TLAP loads can be found under Edit > Point Load Info…
  • The Point Loads Case Definitions dialog (Figure 7) will appear with access to the point loads objects.

CSV/Excel Format

The following CSV/Excel format is supported by StressCheck (Figure 9):

• First row: Header information (can be blank)
• From second row to last row: 14 columns, comma delimited with the data of interest:
  • 1st column represents the Case ID
  • 2nd to 4th are the coordinates of the point x, y, z
  • 9th, 10th, and 11th are the forces Fx, Fy, and Fz
  • 12th 13th and 14th are the moments Mx, My, Mz
  • Other columns may contain “dummy” (i.e. blank or null) values

Multiple Case ID’s may be included in one CSV file, but separated by a row.

• The PATRAN CSV can be then imported into StressCheck by selecting File > Import, changing the filter to “PATRAN (*.csv)”, selecting the PATRAN CSV file and clicking “Open”. Then, in the Import Point Loads/Constraints dialog click Accept.
  • If the number of columns is different from 14, StressCheck will issue an error.
• A message will appear indicating the number of load cases successfully imported by StressCheck, as well as a project log summary of the imported TLAP loads by Case ID.
• The imported TLAP loads can be found under Edit > Point Load Info…
  • The Point Loads Case Definitions dialog (Figure 10) will appear with access to the TLAP objects.

For more information on using imported TLAPs, refer to Total Load at a Point (TLAP) Implementation.