Importing Pro/ENGINEER Assembly Files
To import a Pro/ENGINEER assembly file into SolidWorks:
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Click Open
(Standard toolbar) or File, Open.
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In the dialog box, set Files of type to ProE Assembly (*.asm;*.asm.*;*.xas).
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Browse to a file, and click Open.
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In the Pro/ENGINEER To SolidWorks Converter dialog box, set these options:
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Component Import Options section. Select one of the following:
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Use feature import for all parts. Imports all component parts as features.
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Use body import for all parts. Imports all component parts as bodies.
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Prompt for each part. Prompts you to import each individual component as a feature or a body.
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If same name SolidWorks file is found:
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Import material properties
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Import sketch/curve entities
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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.
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Set these options:
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Import geometry directly. Imports a model without features, either as a solid or as surfaces.
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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.
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Analyze the model completely. Determines the number of features that SolidWorks can recognize and import.
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Import material properties
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Import sketch/curve entities
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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:
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Features. Imports the model and attempts to recognize features. Attempt to correct invalid features attempts to correct problems such as reversed extrusions.
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Body. Attempts to import the model as a solid using Knitting. Attempt to correct invalid feature has no effect.
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Generate translation report. If you select Features, generates a report that includes the features plus the recognition and import status.
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Click Features or Body to import the model component.
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In the Translation Report:
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Close the dialog box.
SolidWorks imports the component. The Pro/ENGINEER to SolidWorks Converter dialog box prompts you to import the next component.
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Continue importing components until you have imported the entire assembly.