Importing Pro/ENGINEER Assembly Files
To import a Pro/ENGINEER
assembly file into SolidWorks:
Click Open
(Standard toolbar) or File,
Open.
In the dialog box, set Files
of type to ProE
Assembly (*.asm;*.asm.*;*.xas).
Browse to a file, and click Open.
In the Pro/ENGINEER
To SolidWorks Converter dialog box, set these options:
Component
Import Options section. Select one of the following:
Use feature import for all parts. Imports
all component parts as features.
Use body import for all parts. Imports
all component parts as bodies.
Prompt for each part. Prompts you to
import each individual component as a feature or a body.
If
same name SolidWorks file is found:
Import
material properties
Import
sketch/curve entities
Import
component constraints (Mates) Pro/ENGINEER
constrains are translated into SolidWorks assembly mates. All the basic
types, plus Pro/ENGINEER Point on Surface,
Point on Edge, and Edge
on Surface constraints are supported.
Only Pro/ENGINEER high level motion constraints such as Gear mates are not supported.
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Click Import.
SolidWorks converts and imports the file.
If you selected Prompt for each
part in the Component Import Options
section, SolidWorks redisplays the Pro/ENGINEER
To SolidWorks Converter dialog box.
Set these options:
Import geometry
directly. Imports
a model without features, either as a solid or as surfaces.
BREP. Imports the model using Boundary
Representation data. In general, BREP
mode is faster than Knitting,
especially for complex models. BREP
attempts to import the model as a solid.
Analyze the
model completely. Determines
the number of features that SolidWorks can recognize and import.
Import
material properties
Import
sketch/curve entities
-
Click OK.
If you select Import geometry directly,
SolidWorks imports the model. If you select Analyze
the model completely, SolidWorks parses the imported file and redisplays
the Pro/Engineer to SolidWorks Converter
dialog box with the following options:
Features.
Imports the model and attempts to recognize features. Attempt
to correct invalid features attempts to correct problems such as
reversed extrusions.
Body.
Attempts to import the model as a solid using Knitting.
Attempt to correct invalid feature
has no effect.
Generate
translation report. If you select Features,
generates a report that includes the features plus the recognition and
import status.
Click Features or Body
to import the model component.
In the
Translation Report:
Close
the dialog box.
SolidWorks
imports the component. The Pro/ENGINEER
to SolidWorks Converter dialog box prompts you to import the next
component.
Continue
importing components until you have imported the entire assembly.