The procedure for selecting the output formats you want to save is as follows:
In the top-level Ansys Polydata menu, select Outputs.
Outputs
Choose one or more of the items below to enable output for your postprocessor(s) / application of choice:
-
Enable Patran output
-
Enable Ideas output
-
Enable CSV (Excel) output
-
Enable Polyflow output
-
Enable Iges file output
-
Enable Fidap output
-
Enable FieldView UNS output
-
Enable CFD-Post output
-
Enable EnSight output
-
Enable Ansys Mechanical APDL output
-
Enable Ansys Mapper output
-
Enable STL (StereoLithography) output
The Polyflow output refers to a results file that can be read by Ansys Polyflow itself and is saved at each step of an evolution or time-dependent calculation. The CFD-Post format refers to CFD-Post, the standard postprocessor for Ansys Polyflow. The Fidap format refers to FIPOST, and the Ansys Mapper format refers to files that are compatible with Ansys Mechanical (note that only thickness and temperature data from Polyflow can be written in this format). See the descriptions that follow for information about the other output formats.
By default, the CFD-Post output is enabled, as listed under Current output(s) at the top of the menu. Certain output formats, including CFD-Post, Ansys Mechanical, and IGES, require that you specify the system of units used in the Ansys Polydata so that this information can be passed on with the results. See step 4. for further details.
Important: Note that the information you provide for CFD-Post, Ansys Mechanical, and/or IGES regarding the system of units will not affect any of the data entered in your Ansys Polydata session.
A final results file is always saved in Ansys Polyflow format at the end of a calculation, so you need not enable this option to ensure that your final results are saved. You only need to enable this option if you want Ansys Polyflow to save the results at each evolution or time step (or as often as specified by the triggering in Output for Time-Dependent, and Evolution Calculations).
If you want to turn off any of the current outputs, select the corresponding Disable menu item. (Each Enable menu item will become a Disable item after you select it.)
If CFD-Post, Ansys Mapper, and/or Iges output is enabled, you must approve the system of units that will be passed to CFD-Post, Ansys Mechanical, and/or the CAD/CAM program with the results. This approval is accomplished using the Change System of Units for specific outputs menu. Perform the following actions, starting in the Outputs menu:
Open the Change System of Units for specific outputs menu by clicking the Set units for CFD-Post, Ansys Mapper or Iges menu item.
Set units for CFD-Post, Ansys Mapper or Iges
Note that the Change System of Units for specific outputs menu will open automatically when you click Enable CFD-Post output, Enable Ansys Mapper output, or Enable Iges file output.
Review the list of units currently selected for each quantity, as displayed in the Change System of Units for specific outputs menu. If you want to revise any of the units listed under Current, click the Modify system of Units menu item.
Modify system of Units
The Current System of Units menu will open, where you can make your selections:
You can specify the units for all of the quantities at once by clicking the Set to <system> menu item, where <system> is the appropriate set of units for your inputs (e.g., metric_MKSA+Kelvin corresponds to meter, kilogram, second, Ampere and Kelvin). The units displayed at the top of the menu will be immediately updated.
You can specify the unit for an individual quantity by clicking the Modify the <quantity> unit menu item, where <quantity> is a quantity with inappropriate units (for example, length). The menu will then display your options for this quantity; click the Select <unit> menu item, where <unit> is the appropriate unit for your inputs (e.g., millimeter). Then click Upper level menu to return to the previous menu display and to update the units listed at the top of the menu.
Note that some units (including hectometers, decameters, and decimeters) are available for selection in Polydata, but do not exist in the IGES format. If you select one of these units, the coordinates will be converted into units recognized by IGES: hectometers will be converted to meters (that is, the coordinates will be multiplied by 100); decameters will be converted to meters (that is, the coordinates will be multiplied by 10); and decimeters will be converted to millimeters (that is, the coordinates will be multiplied by 10).
If you have enabled more than one output format that requires units, the same unit system will be applied to all of the formats. This means that you do not need to reset the units repeatedly, but you do have to make sure that the unit system is appropriate for all of the formats.
Click Upper level menu repeatedly to return to the Outputs menu.
Note that if you fail to perform step 4.(a), the Change System of Units for specific outputs menu will open automatically before you are allowed to navigate away from the Outputs menu or save the data file; this is to ensure that you approve of the system of units passed to CFD-Post, Ansys Mechanical, and/or the CAD/CAM program.
If CFD-Post output is enabled, you can specify whether the names of the boundaries and subdomains in the output are those defined via Named Selections in the Ansys Meshing application (the default) or the short names generated by Ansys Polydata. (For more information about Named Selections, see Named Selections and PMeshes in the separate Polyflow in Workbench User's Guide.) The currently selected convention is displayed near the top of the Outputs menu. To change the naming convention, click either of the following at the bottom of the menu, as appropriate:
Switch to mode: using short names in CFD-Post
or
Switch to mode: using named selections in CFD-Post
When you are satisfied with the Current output(s), click Upper level menu to return to the top-level menu.
When you save the data file, as described in Writing a Data File, Ansys Polydata will give you the opportunity to specify names for all of the output files that you have requested in the procedure above. See Table 5.1: Files Written and Read by Ansys Polydata and Ansys Polyflow for file types and default naming conventions corresponding to the different postprocessors.
Problematic mesh elements (too small an angle, too large an angle, an improper aspect ratio, etc.) occasionally appear during a Ansys Polyflow calculation, and when combined with mesh deformation, can lead to convergence difficulties. When a problematic element is detected, Ansys Polyflow generates a bad_mesh.stl file so you can check the mesh quality and/or recreate a better mesh. In addition, Ansys Polyflow generates a bad_mesh.csv file that contains the results and allows you to resume the computation with the new mesh. See Results Interpolation Onto Another Mesh.
The STL output file contains the facets describing the boundaries of the domains of the geometry, such that each boundary of each sub-domain corresponds to a "solid". For example, if the geometry is made of two sub-domains "SD1" and "SD2" with boundary B1, B2, B3 and B4. The STL output contains
solid SD1_B1, solid SD1_B2, solid SD1_B3, solid SD1_SD2; solid SD2_B1, solid SD2_B3, solid SD2_B4
The output files for PATRAN are a neutral file containing the
connectivity tables and the nodal coordinates (called
patm, by default), and a results file containing
the nodal values of the fields (called patr, by
default). The header of the results file contains a short description of each
variable.
Since PATRAN does not understand all of the interpolation types available in Ansys Polyflow, results will be converted according to Table 5.2: Conversion of Interpolation Types for PATRAN Output.
Table 5.2: Conversion of Interpolation Types for PATRAN Output
| 2D | 2D | 3D | 3D | |
|---|---|---|---|---|
| Interpolation in Ansys Polyflow | P1_C0 | other | P1_C0 | other |
| P0_C-1 | P0_C-1 | |||
| Converted to | TRI3 | TRI6 | TET4 | TET10 |
| QUAD4 | QUAD9 | WED6 | WED15 | |
| (low order) | (high order) | HEX8 | HEX20 | |
| (low order) | (high order) |
For mixed interpolation types (for example, velocity-pressure), high-order elements will be generated for all fields whenever one of the fields in the PATRAN results file is interpolated with high-order elements.
The output files for I-deas are two universal files: one containing the
connectivity tables and the nodal coordinates (called
stbm, by default), and one containing the nodal
values of the fields (called stbr)
Table 5.3: Conversion of Interpolation Types for I-deas Output
| 2D | 2D | 3D | 3D | |
|---|---|---|---|---|
| Interpolation in Ansys Polyflow | P1_C0 | other | P1_C0 | other |
| P0_C-1 | P0_C-1 | |||
| Converted to | linear | parabolic | linear | parabolic |
| (low order) | (high order) | (low order) | (high order) |
Since I-deas does not understand all of the interpolation types available in Ansys Polyflow, results will be converted according to Table 5.3: Conversion of Interpolation Types for I-deas Output.
For mixed interpolation types (for example, velocity-pressure), high-order elements will be generated for all fields whenever one of the fields in the I-deas results file is interpolated with high-order elements. Note that 2D 9-node quadrilaterals are converted to 8-node serendipity elements. 3D quadratic bricks are converted to 20-node elements, because of I-deas limitations.
The IGES output file contains lines that describe the geometry. If you save IGES files during a time-dependent or evolution calculation, they will describe the modified (updated) geometry calculated as part of the solution.
This is particularly useful for inverse extrusion problems, where the geometry of the die is calculated by Ansys Polyflow. This IGES file contains the precise die geometry (adaptive section, constant section, inlet section, etc.), which can be postprocessed in most CAD/CAM programs, allowing for a direct interface to die cutting machines.
You must approve the system of units that will be passed to the CAD/CAM program with the results, either when you Enable Iges file output, or by clicking Set units for CFD-Post, Ansys Mapper or Iges in the Output menu. Note that some units (including hectometers, decameters, and decimeters) are available for selection in Polydata, but do not exist in the IGES format. If you select one of these when specifying the units, the coordinates will be converted into units recognized by IGES: hectometers will be converted to meters (that is, the coordinates will be multiplied by 100); decameters will be converted to meters (that is, the coordinates will be multiplied by 10); and decimeters will be converted to millimeters (that is, the coordinates will be multiplied by 10).
A CSV (comma separated variables) file is a common format for tabulated data that can be read into spreadsheet programs such as Excel. The CSV file that Ansys Polyflow can read or write contains a list of data points and a list of values. Fields are recognized by their (case-sensitive) names.
When you save Ansys Polyflow results in a CSV format, a data entry is written for each nodal location at which the quantity is defined. When Ansys Polyflow reads a CSV file, it will interpolate the data (if they do not correspond exactly to the nodes in the mesh) between the listed values.
CSV files can be used for interpolating results between different meshes and setting velocity boundary conditions. See Results Interpolation Onto Another Mesh and Velocity Profile from a CSV File for details. You can also initialize solution variables with a CSV file, as described in Using the CSV File to Initialize Solution Variables.
The output file for FieldView contains the geometry and the computed
fields. The suffix of the file is .uns. Actually,
Ansys Polyflow creates a fv.uns file for steady-state
simulations and a series of fv#.uns files, where # is
the step index for evolution or time-dependent problems. This numbering and
syntax allows FieldView to load all the files of a transient calculation in
one single step.
The .uns file is in a portable binary format (that
is, a .uns file created under Linux can be read under
Windows and vice-versa). FieldView supports linear interpolation only. All the
fields of an Ansys Polyflow simulation are therefore converted into linear fields
(that is, defined at the vertices of the FEM mesh).
The output file for CFD-Post (identifiable by the
cfx.res suffix) contains the geometry and the
computed fields. By default, Ansys Polyflow creates a
cfx.res file for steady-state simulations and a
series of #_full.trn files in a cfx directory, where
# is the step index for evolution or time-dependent
problems. This numbering and syntax allows CFD-Post to load all the files
of a transient calculation in one single step.
The cfx.res file is in a portable binary format
(that is, a cfx.res file created under Linux can be read
under Windows and vice-versa). CFD-Post supports linear interpolation only.
All the fields of an Ansys Polyflow simulation are therefore converted into
linear fields (that is, defined at the vertices of the FEM mesh).
Note that names for CFD-Post files should be carefully selected. For
enabling a proper file identification and for avoiding possible confusion, a
short filename should be cfx.res, while a long file
name should preferably and at least contain the string
_cfx.res.
You must specify the units used by Ansys Polydata and Ansys Polyflow. CFD-Post will
convert the results in the MKSA system of units when
reading the results files. In the Output menu, select
Set units for CFD-Post, Ansys Mapper or Iges. You can
also define the units by selecting Enable CFD-Post output,
which opens a new menu named Change System of Units for specific
outputs.
The output files for the EnSight graphic postprocessor are based on the
EnSight gold format. The typical output consists of a case file
(.case) and several files for geometry and fields.
The case file is the entry file to EnSight; it is an ASCII file that contains
the key information about the simulation. For a steady simulation, the case file
contains the file names of the files for geometry and fields.
For evolution and transient simulations, the content of a case file is richer. In particular, it contains generic names for the various files (geometry and fields), where wildcards or * characters refer to the sequence of calculation steps. The number of wildcards depends on the maximum number of transient/evolution steps that you define in the Ansys Polydata session. The case file also contains the list of steps that produce the output files, as well as the sequence of corresponding values of time or evolution parameters. Note that a large number of files can be created, for individual fields and for individual transient/evolution steps.
Upon restarting a calculation, Ansys Polyflow checks whether the former case file can be reused. If an incompatibility is detected in the early stage, the calculation will stop. The most typical incompatibility is caused when a risk exists of making former output files simply inaccessible for subsequent analysis. This typically occurs when the number of wildcards is modified. In most cases, the causes of incompatibility can be circumvented by selecting a new name for the EnSight output file when restarting a calculation.
All files created on Windows or Linux are portable. This concerns not only the case file, which is ASCII, but also the geometry and field files, which are in binary format. Binary format is used for reasons of reading efficiency. This argument is especially true when a large number of files is involved. In the production of EnSight output files, only the linear interpolation is available. All fields of an Ansys Polyflow calculation are converted into linear fields, that is, defined at the vertices of the mesh file. It is interesting to note that PMeshes are visible.
The Ansys Mechanical APDL output file can be selected when you are interested
in a subsequent structural analysis. The output file for Ansys
Mechanical APDL contains the geometry as well as temperature and thickness fields
when available. The suffix of the file is cdb. You can
import the .cdb file containing thickness and/or
temperature as fields only in Ansys
Mechanical APDL Classic. By default,
Ansys Polyflow creates a .cdb file for steady-state
simulations and a series of cdb.# files, where
# is the step index for evolution or time-dependent
problems. The .cdb file is in a portable ASCII format.
Next to the geometry, default values are also created for material properties. For nonisothermal cases, the temperature field is provided. For shell models, only information from the fluid region is provided, whereas the mold information is discarded (for more information about shell models, refer to Blow Molding and Thermoforming). For fluid domains with multiple layers, the total thickness distribution is provided.
For 2D applications, including shells, triangles and quadrilaterals are supported. In 3D, tetrahedrons, pyramids, prisms and brick elements are supported. However, if a pyramid element is encountered, it will be advised to take appropriate actions in Ansys Mechanical APDL and selecting the quadratic interpolation for the entire geometry. When this occurs, a message, similar to the following, will appear in the Ansys Polyflow listing file:
During the production of a results file for ANSYS, at least one linear pyramid has been detected. ANSYS will require a conversion towards element 186 with the commands ’ET,#,186’ and ’EMID,ADD,ALL’. Please refer to ANSYS user’s manual.
The Ansys Mapper format can be selected when you are interested in performing additional simulations in Ansys Mechanical (for example, in an Explicit Dynamics analysis system). For example, you could use the results of your Polyflow thermoforming or blow molding simulation in a subsequent Mechanical structural analysis.
Two kinds of output files are generated when the Ansys
Mapper format is selected. The first kind of file has a
.txt extension, and provides the coordinates for
mesh nodes, along with the associated values of temperature and thickness (note
that a node can have more than one thickness value in the case of a multilayer
system). The second kind of file has a .xml extension,
and provides information about the data contained in the
.txt file. Both kinds of files are in a portable
ASCII format. By default, Polyflow creates a single
.txt and .xml file for
steady-state simulations. For evolution or time-dependent problems, a series of
.txt and .xml files are
generated; the names of these files are appended with a number to indicate the
step index.
Note that if you want to use your output files to initialize the temperature and the thickness for a Mechanical structural analysis, you need to link the Polyflow and Mechanical systems in the project schematic of Workbench. For more information, see Polyflow to Mechanical Data Transfer in the Mechanical User's Guide.