In this Article:
For Parasolid Imports
Tips & Techniques
Import
File Menu
Use this command to import non-VX files types such as IGES, STEP, DWG, etc. into VX as parts, sketches, or drawing sheets. Use the Import Form to select the file type to import. You can also use this form to save (i.e., make active) import settings including filters and format specific options.
Saving the settings will make them available to the Open File command or drag and drop functionality if you choose to open a non-VX file. For the Open File command, set the File Browser to the required file extension type. See below for more about the Import Form.
Basic Operational Sequence
- Select the file type to export to.
- Set the filter and format specific settings as desired. See below for the forms that are used for each file type.
- Save the settings if desired.
-
Pick OK to begin the export, Reset or Cancel as desired.
 Import Form - Type
This list contains the import file types supported by VX. Those listed on the VX Tab are included with each VX license. Those listed on the TM Tab (TransMagic) and the CCE Tab (cadcam-e) require third-party translator passwords to be installed. Ask your VX sales representative about these options.
The selections are VX level dependent. That is, only the file types compatible with the active VX level (i.e., part, sketch, drawing sheet) as well as the selected Target (see below) are available for selection. Select from the list of file types to import.
Import Form - Target
-
Part, Sheet, Sketch
This option allows you to select the target object type to create. If no VX file is active (i.e., you are at the file level), a VX file and object are created using the same name as the import file.
If a VX file is active but no object is active (i.e., you are at the object level), an object is created using the same name as the import file and then activated. If an object is active (i.e., part, sketch or Drawing sheet), this option is not active. It is assumed that the target will be an object type compatible with the active object. When active, select from part, sketch or sheet.
See CAD Tips & Techniques about Importing Geometry with Dimensions into a Sketch.
Import Form - Settings
Sub-Part
The imported geometry is converted to a sub-part. A sub-part is a component that does not show up in the Assembly Manager or in the root object list of the active file. It is automatically deleted when the parent part is deleted, and may be flagged with Auto Regen on or off. Sub-parts are merged with their parent parts automatically. Sub-parts will inherit the tolerance and units of their parent part instead of using the configuration defaults. The import is NOT repeated during a History Replay.
If your import needs to be healed, Right-click on the sub-part history item and select Redefine. While in the sub-part run any heal commands that you require. When finished Exit Part and you will be back in your original part object. The import and heal commands should never need to be regened.
Backup
The imported geometry is converted to a Backup Feature. This speeds up history regeneration functions (see History Manager). All data generated from the Import is backed up with the feature.
Encapsulate
The imported geometry is converted to an Encapsulate History feature. Encapsulating is similar to a Backup Feature, but the encapsulated geometry looses its parametric history. In the case of imported geometry, it has no history anyway. The import is NOT repeated during a History Replay.
Import
The imported geometry is handled as an Import Feature. The import
IS repeated during a History Replay so make sure the import file remains in its current location.
Use encapsulate before editing imported assembly parts.
The "SubPart", "Backup" and "Encapsulate" options above are handled the same way when you import an assembly. That is, the history of every part in an imported assembly is automatically encapsulated. Only this "Import" option is different. In this case, the history of each imported part is not encapsulated and you will not be able to edit the imported parts until you encapsulates the history of each.
See also: History Editing
See also: Why will my imported assembly NOT regenerate?
Import Form - Other Options
-
OK
Accepts the current settings and begins importing the file. For all formats except Parasolid, the status will be displayed in the Translator Progress Window. For the Parasolid format, the Parasolid Import Form is displayed. Export will begin and the status displayed when you select OK from this form. Refer also to the description section of this topic for more information about exporting to the Parasolid format.
-
Reset
Reset all filters and options to their previous defaults.
-
Cancel
Keep the current settings but close this form without importing.
For Parasolid Imports
If you select Parasolid as the format type and then pick the OK button, additional Parasolid options are available from the Parasolid Import Form after the file is selected from the File Browser.
No matter which HISTORY option is picked, we use ENCAPSULATE. If we let the Assembly use the IMPORT option, REGEN would re-import and overwrite all the components.
When a ParaSolids assembly is imported, we do not encapsulate the histories of component parts automatically. If we do, the file size is automatically doubled, which can be substantial for a large assembly. With an assembly, it is assumed that the user is not likely to edit every part in the assembly, so we wait until a user tries to edit an imported assembly part and then we prompt them to encapsulate the history first.
A history regen recreates a model from scratch using information encoded in the history. If the history does not contain the original imported geometry in the form of an encapsulated operation, there is no way to regen the part.
The above explanation may beg the question of why we do not encapsulate imported geometry automatically when the user tries to edit the part. It is because we have to ensure VX is finished executing all pending events before doing the encapsulation. Presently, the safest approach is to require that the user initiate the encapsulation, which guarantees VX is not processing any other events that might conflict with the encapsulation. It is a little bit like Windows prompting a user to restart his computer after updates are installed instead of doing it automatically.
Tips & Techniques
Working with large files after being imported into the VX sketcher
This is handled efficiently by turning off automatic constraint solving using the
Sketch Preferences Form
. VX does this automatically. The only way the constraint system will then be loaded is with an explicit
Solve Current Sketch
command. The setting is local to the large imported sketch so that other sketches will continue to operate as usual.
Supported file types and extensions
Refer to Import/Export Formats for file extensions and additional information about each file type.
Do not forget to keep your translator passwords current
For CATIA, Pro/E and Unigraphics, you are prompted for a required password if your translator license has expired. Contact your VX dealer to obtain new passwords.
You can import multiple files at the same time.
You can select multiple files during one import session. If you are IN a Part, Sketch or Drawing Sheet, ALL files will be combined into that Part, Sketch or Drawing Sheet. If you are NOT in a Part, but you have "Auto activate" (refer to the Import Options Form for each format) enabled, then ALL files will be combined into a Part of the first file name. If you are not in a Part and auto activate is not enabled, then each file will be created in its own part.
You can create surfaces from imported STL data
An imported STL object can be selected as input for the Face from Point Cloud command. It is important to note that this is not a general purpose STL to NURBS conversion and/or translation tool. It can be used to that effect, however, for certain supported cases.
The supported cases include those that the Surface from Point Cloud command supports. Base faces can still be used, including ones with seam edges. You will need to provide a base face in cases where the STL data cannot be projected to a common plane adequately. See Finite Element Method (FEM) for Surface Creation section for more information.
Do not forget to keep your translator passwords current
For CATIA, Pro/E and Unigraphics, you are prompted for a required password if your translator license has expired. Contact your VX dealer to obtain new passwords.
You can import multiple files at the same time.
You can select multiple files during one import session. If you are IN a Part, Sketch or Drawing Sheet, ALL files will be combined into that Part, Sketch or Drawing Sheet. If you are NOT in a Part, but you have "Auto activate" (refer to the Import Options Form for each format) enabled, then ALL files will be combined into a Part of the first file name. If you are not in a Part and auto activate is not enabled, then each file will be created in its own part.
You can create surfaces from imported STL data
An imported STL object can be selected as input for the Face from Point Cloud command. It is important to note that this is not a general purpose STL to NURBS conversion and/or translation tool. It can be used to that effect, however, for certain supported cases.
The supported cases include those that the Surface from Point Cloud command supports. Base faces can still be used, including ones with seam edges. You will need to provide a base face in cases where the STL data cannot be projected to a common plane adequately. See Finite Element Method (FEM) for Surface Creation section for more information.
Notes
- Imported STL data is stored in the VX Part as a 3D block entity. It can be selected by setting the Pick Filter to Block.
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