Creo Simulate > Getting Started with Creo Simulate > Configuration File Options > About FEM Mode Modeling, Meshing, and Output Options
About FEM Mode Modeling, Meshing, and Output Options
Use these options to control a variety of settings in FEM mode.
fem_allow_named_mesh_files
Determines whether to enter a name of a mesh file when saving a mesh, and to select a mesh file when loading a mesh. When this option is set to no, the name of model_name.fmp (a) is automatically assigned to the mesh file when you use the File > Save FEM Mesh command, and automatically retrieves the mesh from the model_name.fmp (a) file when you use the File > Open FEM Mesh command.
If you set this option to yes, then when you use these commands, Creo Simulate prompts you to either select the mesh file to load, or to enter the name for the mesh file to store.
no*
yes
fem_ansys_annotations
Allows output of notes as ANSYS annotations.
no*
yes
fem_ansys_grouping
Allows you to output nodes and element groups using the ANSYS CM family of commands when set to yes. The default value is no. For more information on layer grouping in ANSYS, refer to the topic Grouping in ANSYS.
no*
yes
fem_asp_ratio
Sets the value against which FEM mode compares the aspect ratios of the elements it creates. The value type is numeric and the default value is 7.
fem_default_solver
Sets the default solver selection in the Run FEM Analysis. The path is specifies to one of the following solvers:
ANSYS*
MSC/NASTRAN
fem_dist_index
Sets the value against which FEM mode compares the distortion indices of the elements it creates. The value type is numeric and the default value is 0.4.
fem_edge_angle
Sets the angle between two adjacent element edges. Type a value between 0 and 90. The value type is numeric and the default value is 30.
fem_hierarchical_mesh
If this option is set to yes then hierarchal meshing is triggered on starting Creo Simulate in FEM mode. The FEM mesh is automatically stored as a mesh file on creation and retrieved on entering Creo Simulate. If this option is set to no hierarchal meshing is not enabled and the mesh is not stored or retrieved automatically.
No*
Yes
fem_keep_solver_files
To retain all the solver files after running an analysis, set the configuration option to yes. By default, the solver files are not retained after running the analysis.
no*
yes
fem_output_rigid_link_as_rbar
Controls whether rigid links are output to NASTRAN as RBE2 or RBAR. If this option is set to yes then rigid links are output to the input deck as RBAR cards. If this option is set to no, rigid links are output as single RBE2 cards. For more information, refer to the topic Rigid Links in NASTRAN
no*
yes
fem_mesh_auto_retrieve
If this option is set to yes, then on opening Creo Simulate in FEM mode the FEM mesh is retrieved if it is compatible with the model. If this option is set to no the mesh will not be retrieved on opening in FEM mode.
No*
Yes
fem_mesh_auto_save
If this option is set to yes the FEM mesh is automatically saved in the current directory after it is created. If set to no, the mesh is not saved automatically after it is created.
No*
Yes
fem_mesh_link_solid_shell
Controls the default setting of the Create Solid-Shell Links check box on the FEM Mesh Settings dialog box. By default this option is set to yes, and the check box is selected.
yes*
no
fem_mesh_operations
Activates the OPERATIONS menu, which enables you to perform specialized operations on NASTRAN files and the finite element mesh for NASTRAN. When you set this option to yes, the Operations command appears on the Mesh menu. If you set the option to no, the Operations command does not appear.
no*
yes
fem_preserve_mesh
If this option is set to yes a warning is issued every time you carry out an operation like creating, modifying or deleting a simulation object that invalidates the existing mesh. If set to no, the existing mesh is erased without any warning to the user.
yes*
no
fem_mid_ratio
Sets the value against which FEM mode compares the mid ratios of the elements it creates. The value type is numeric and the default value is 0.1.
fem_neutral_version
Specifies the version number of the FEM neutral file.
1
2
3*
fem_shell_elem_type
Sets the default shell element type in FEM mode. The default value of this option is quad, that specifies quadrilateral element type for FEM meshing.
quad*
tri
fem_skew_angle
Sets the maximum acceptable default skew angle value, measured in degrees. Enter a value between 0 and 90. The value type is numeric and the default value is 45.
fem_solver_time_limit
For MSC/NASTRAN solutions, this option interrupts the solver after the specified time limit in minutes. The default value is -1. This negative value allows MSC/NASTRAN to set its own default time limit.
fem_study_directory
Specifies whether the analysis output files are stored in the study directory or in the current working directory. By default, the configuration option is set to yes and all the output files are stored in the study directory. The study directory and all the output files, except for the model snapshot, use the same base name as the selected analysis or the specified name. When you set this option to no, the output files are stored in your current working directory named after the model.
yes*
no
fem_taper
Sets the minimum acceptable default taper value. Enter a value between 0 and 1. The value type is numeric and the default value is 0.5.
fem_twist_angle
Sets the maximum acceptable default twist angle between opposing element faces. Applies to brick and wedge elements only. Enter a value between 0 and 90.
fem_warp_angle
Sets the maximum acceptable default warp angle value, measured in degrees. Enter a value between 0 and 90. The value type is numeric and the default value is 10.
fem_which_ansys_solver
Specifies the ANSYS solver that is to be used for FEM analysis run.
sparse*
iccg
auto
frontal
iterative
powersolver
fem_y_dir_compress
Specifies the Y direction based on compressed and uncompressed geometry. The default value is no, which indicates that uncompressed geometry will be used.
no*
yes
pro_ansys_path
Specifies the path to the ANSYS executable.
pro_nastran_path
Specifies the path to the MSC/NASTRAN executable (nastran).
pro_solver_name
Specifies the name of the user-defined solver to be included in the Run FEM Analysis dialog box.
pro_solver_path
Specifies the path to the user-defined solver whose name is included in the Run FEM Analysis dialog box.
sim_additive_mass
Adds any masses that reference the same geometrical entity or resolve to the same mesh node. If you set this option to yes, FEM suppresses the precedence rules that apply to masses.
no*
yes
sim_check_jacobian_corners
When running a FEM analysis for ANSYS and NASTRAN solvers, if this option is set to yes, Creo Simulate checks and fixes elements that have non-positive Jacobian determinants measured at the corner nodes as well as at integration points. It checks and fixes elements that have a distortion ratio of 1e-3 or smaller. It also removes the ANSYS card SHPP, LSTET, ON from the ANSYS output file filename.ans. For a NASTRAN solver, for parabolic elements, this option introduces the executive card GEOMCHECK TET_DETG MSGTYPE=FATAL in the output NASTRAN file filename.nas.
no*
yes
sim_fem_nastran_use_pshell
For MSC/NASTRAN solutions, this option determines the form that FEM mode uses to output laminated composite shell properties to the solver. When you set this option to no, FEM outputs laminated composite shell properties using PCOMP cards that reference MAT8 material cards. If you set this option to yes, FEM outputs laminated composite shell properties using PSHELL cards that reference MAT2 material cards.
no*
yes
sim_nastran_use_coupmass
For MSC/NASTRAN solutions, this option enables you to enforce consistent mass matrix generation. When you set this option to yes, FEM adds PARAM,COUPMASS,1 to the NASTRAN deck to ensure that the solver generates a consistent mass matrix. If you set this option to no, FEM does not add this statement, and NASTRAN generates a lumped mass matrix.
no*
yes
sim_output_obj_names
Output beam sections name, analyses name, coordinate systems names as comments.
sim_output_ids_for_layers
Determines whether Creo Simulate will generate an XML file containing layer data when you output a NASTRAN deck. If you set this option to yes, the XML file is generated, that provides a listing of node and element IDs for any idealizations such as beams, shells, and masses that you place on layers. The file provides lists for all layers that contain simulation entities.
The filename for the XML file is outputfilename_layers.xml, where outputfilename is the name that you specified for the .nas file on the Run FEM Analysis dialog box. The XML file is placed in the same directory as the .nas file.
no*
yes
sim_ignore_unpaired
Sets the default value of the Ignore Unpaired Surfaces check box on the FEM Mesh Settings dialog box in FEM mode. If you set this option to no the ignore unpaired surfaces check box is not selected. You are alerted whenever unpaired surfaces are found during a compression test and shown the entire model while the unpaired surfaces are highlighted.
If you set this option to yes, the Ignore Unpaired Surfaces check box is selected and you are not notified about unpaired surfaces. Instead, it your model is displayed without the unpaired surfaces.
no*
yes
sim_remove_unopposed
Defines the default value of the Remove Unopposed Surfaces check box on the FEM Mesh Settings dialog box in FEM mode. The Remove Unopposed Surfaces check box determines whether unopposed surfaces are retained or ignored during compression.
If you set this option to yes, the Remove Unopposed Surfaces check box is selected by default and the system removes the unopposed surfaces it finds when meshing the model. When you set this option to no, the Remove Unopposed Surfaces check box is not selected by default and the system retains the unopposed surfaces in the shell model. You are alerted about any unopposed surfaces during meshing.
no*
yes
sim_smooth_aspect_ratio
Determines the element aspect ratio criterion that is used when smoothing a FEM mesh during mesh optimization. You must specify a real number for this option, and the default setting is 7.0. As a general rule, you should not change the default setting unless the first optimization pass shows that the overall element quality has degraded such that setting a new aspect ratio criterion would result in better shaped elements.
sim_smooth_edge_angle
Determines the element edge angle criterion that is applied to quadrilateral elements when smoothing a FEM mesh during mesh optimization. You must specify a real number in degrees for this option, and the default setting is 30. As a general rule, you should not change the default setting unless the first optimization pass shows that the overall element quality has degraded such that setting a new edge angle criterion would result in better shaped elements.
sim_smooth_skew
Determines the element skew angle criterion that is applied to quadrilateral elements when smoothing a FEM mesh during mesh optimization. You must specify a real number in degrees for this option, and the default setting is 45. As a general rule, you should not change the default setting unless the first optimization pass shows that the overall element quality has degraded such that setting a new skew angle criterion would result in better shaped elements.
sim_smooth_taper
Determines the element taper criterion that is applied to quadrilateral elements when smoothing a FEM mesh during mesh optimization. You must specify a real number for this option, and the default setting is 0.5. As a general rule, you should not change the default setting unless the first optimization pass shows that the overall element quality has degraded such that setting a new taper criterion would result in better shaped elements.
sim_smooth_warp_angle
Determines the element warp angle criterion that is applied to quadrilateral elements when smoothing a FEM mesh during mesh optimization. You must specify a real number in degrees for this option, and the default setting is 10. As a general rule, you should not change the default setting unless the first optimization pass shows that the overall element quality has degraded such that setting a new warp angle criterion would result in better shaped elements.
simulation_fem_mode
Determines the initial state of the FEM Mode check box on the Model Type dialog box. The default is no, indicating that the FEM Mode check box is cleared on the Model Type dialog box when you enter Creo Simulate with a new or unsaved model.
If you select yes, the software assumes you always want to work in FEM mode, and the check box is selected.
no*
yes
std_nastran_template
Sets the file path of a NASTRAN deck template. Use the full path to avoid problems.
這是否有幫助?