Supply Chain Collaboration (On the Edge Solid Edge Tutorial)31 Dec, 2006 By: Russell Brook
Import JT files into Solid Edge.
JT files provide global partner networks with a product design collaboration workflow to improve designs and deliver products to market faster. They contain many different entity types, thereby enabling companies to include all the design details needed to collaborate in today's engineering world and protect intellectual property. JT files have a versatile data structure that can contain precise or faceted geometry, surfaces and construction curves as well as part property information. Communicating with customers and suppliers using easy-to-visualize, accurate and up-to date information reduces misinterpretation as designs pass through the supply chain.
Supplier CAD files are easily combined with OEM JT data using Solid Edge.
Importing JT Documents
There are two workflows for directly importing JT files into Solid Edge; both offer their own merits, depending on what you want to achieve. First, Interpart copy (insert part copy) enables you to import a single JT file or assembly into a single Solid Edge part or SheetMetal template. This method is beneficial when assembly structure and construction elements (surfaces and curves) are not as important as the overall geometry; for example, in mold tool design where you just need to subtract the JT data from a mold base. There are other useful options available when you use Interpart Copy to import JT files into Solid Edge that provide even more control, such as the ability to scale the design in x,y and z directions, apply a shrink factor (mold tooling) and copy colors. You are also able to copy the design body or copy it as a construction body, choose a family of parts members (if one exists) or attach it to a coordinate system to further control placement within the Solid Edge file. As with the second method (opening a JT file directly), you can link interpart copies back to the original JT file to provide associativity.
The Solid Edge JT Part property dialogue allows you to create an associative link, or scale or shrink JT files.
The second method uses the File / Open command. By directly opening the JT file, you can open single parts or assemblies into Solid Edge. You can open a single part into a Solid Edge Part/SheetMetal file or as the initial part in a Solid Edge assembly. With this method, options for feature recognition are also available to add parametric features not included in the JT file.
The Solid Edge flexible JT import options dialogue.
JT files that contain multiple bodies and assembly structures that you can open directly into a Solid Edge assembly template with all the relative component positions maintained, provided the included assembly structure is maintained. JT files with multiple bodies can also be opened into Solid Edge part files, effectively creating a new part with all the bodies fused together into one new solid. The direct-open method always imports Solids if they are available, with further options to allow you to import and surfaces or curves that may be present.
Whichever workflow you use to import JT files into Solid Edge, choosing the Link to File option maintains associativity with the imported JT documents. This allows for an iterative design process when the original JT documents are constantly changing. Notification is provided when JT part data changes, with options to update the part document. (Note: this is not supported in monolithic JT files.) Associativity is maintained for both Precise Geometry and Facet Bodies.
An imported JT file that contains precise geometry.
An imported JT file that contains lightweight faceted data.
An imported JT file that contains only surface and spline data.
JT Document Structures
JT has a variety of supported document structures for parts and assemblies depending on how you use the data and the level of detail required. You can export assembly files into a monolithic or single JT document that stores only the space envelope that removes individual components and assembly structure to protect intellectual property and reduce file size. Assemblies can also be saved as a single JT assembly document with all individual parts within the JT files; when this document is imported into Solid Edge users only see a flat assembly structure. A third option creates a single JT file that contains all of the parts and subassemblies and preserves the assembly structure (all parts and subassemblies are as they were in the original CAD system).
This image shows the different ways JT files manage assembly structure. This is used to protect intellectual property or simplify the assembly structure. You can "wrap" the whole assembly into a single body, flatten the assembly structure or preserve the original assembly structure, depending on what the file is intended for.
Using Precise Geometry
When importing JT data, Solid Edge first looks for precise geometry, but if none exists it can read faceted data. Importing JT files that contain precise geometry allows full reference of the 3D data cantained within the JT file. With precise data, you are able to create assembly constraints (mates, alignments, etc.) to the imported JT data to create associativity with adjacent components or for use in motion studies. Physical properties are maintained and can be used in mass or volume calculations, for example. Full interference checking capabilities are supported. Parts can be used to create high-quality drawing views, and you can integrate exact dimensions and create PMI (product manufacturing information) data with precise dimensions to the imported JT data.
This is an example of a JT file with precise geometry. You can create assembly constraints with adjacent components and motion studies. Physical properties for mass or volume calculations, full interference checking capabilities, and parts can be used to create high-quality drawing views and create PMI.
Using Facet Bodies
Lightweight faceted bodies contain only tessellated representations of parts which very closely approximate the components' size, shape and volume. Facets are for viewing, and are also used as reference while working on assemblies. You can calculate physical properties for facet bodies, locate them when checking for interference in assemblies and create draft-quality drawing views. Faceted bodies in JT files contain the least amount of data and deliver the smallest file size.
This is an example of a JT file containing only faceted geometry. These are useful for protecting intellectual property by filtering out data not relevant to suppliers; they are small, lightweight files that save disc space.
See you On the Edge next month.