PTC Granite™, IGES, or STEP file formats can be used to transfer Alias models to or from Pro/ENGINEER Wildfire.
When using Alias two types of model information can be sent to and read by Pro/ENGINEER. Those two types are geometry information and topology information.
The Alias-created IGES file includes only the description of the geometry information. The Alias-created STEP and Granite file supports both the geometry information as well as the topology information.
The geometric data describes the basic shape of the object and in both Alias and Pro/ENGINEER, geometric data is represented using NURBS.
Topological data describes how the geometric components are connected together to form a solid. The Alias STEP file format has advantages over IGES when transferring Alias models to Pro/ENGINEER because there is more information describing the model that is being transferred.
Set Preferences > Construction Options 
- Construction Presets to Pro/ENGINEER.
Alias set information is only exported in files for IGES, VDAIS, or JAMA-IS, if the option Level Mapping is set to SET. If an Alias set is given a name of the form of LEVEL<n>, where <n> is an IGES level number (and greater than 0), then the corresponding IGES entity for each member of the Alias set is assigned to level<n> in the IGES file. For example, the IGES entities corresponding to each member of the set LEVEL245 is assigned to level 245 in the IGES file.
If an Alias object is a member of several multisets that conform to this naming convention, then the IGES file contains a Property Entity 406 form 1 (Definition Levels) listing the IGES levels to which the corresponding entity belongs.
Information specific to Granite
- Construction Presets
> Tolerances > Fitting is based on testing done
translating models between Alias and Pro/ENGINEER.
Before transferring geometry between Alias and Pro/ENGINEER, consider the purpose of the transfer to plan an appropriate workflow. When you import your Alias model into Pro/ENGINEER, you provide the geometric and topological information of the model. When creating a solid model, the Pro/ENGINEER system must create a valid Pro/ENGINEER data base from the Alias supplied data. The Alias supplied data must satisfy the Pro/ENGINEER's rules for topological and geometric data.
To achieve the tolerance required by solid modeling it's important to manage the modeling units and tolerances when creating your model. Most engineering organizations use the millimeter or inches units as the base linear unit and have developed standards for tolerances that they apply to their CAD systems.
If you are not clear as to which standards your companies or clients use, seek out your CAD system manager. Set up your units and tolerances at the beginning of your modeling session and save them in your usr_options file.
A recommended tolerance to maintain during transfer from Alias to Pro/ENGINEER is dependent on the size of the part being described. Alias uses an absolute tolerance system to describe geometry which means that every piece of geometry in a particular wire file is built to plus or minus a given value (tolerance). Pro/ENGINEER uses a system of relative tolerance, referring to the fact that the acceptable gap between pieces of geometry is based on the relative size of the geometry.
The default accuracy in Pro/ENGINEER is set to .0012 and the range available is .01 to .0001. Using the default accuracy, the maximum allowable distance between two surfaces when the longest edge of the surface is five inches would be less than 5 * .0012 = .006 inches. You must create surfaces in Alias that adhere to this accuracy to be successful in creating a Pro/ENGINEER solid model.
Whether you are creating a model, verifying a model, or debugging a translation, there are some tools within Alias to check the quality of the geometry you have created. The most useful tool is the min/max measurement tool in the Locators menu. Use this tool to check the maximum distance between any two surface boundaries.
The Alias stitching operation is recommended to be done on geometry being prepared for transfer to Pro/ENGINEER.
The Surface Edit > Stitch> Shell Stitch feature within Alias creates a valid solid model topology within the Alias modeling environment. The stitching of surfaces within Alias greatly improves the robustness of the interface to Pro/ENGINEER. The stitching process also identifies surface boundaries that exceed the prescribed tolerances. The designer can correct these problems before translating the data to Pro/ENGINEER.
In addition, the stitching process also identifies duplicate surfaces in the model and orients the surface normals of the completed shell.
When models are constructed using the advance surface tools (swept, Rail Surface and square) it is common to create some smaller surfaces along the edge of one larger surface. This modeling technique does not create the twin edges required for a solid model. The stitching feature automatically creates the twin edge topology required by Pro/ENGINEER.
One case that cannot be solved topologically is the closed or periodic surface (a primitive sphere is an example of a closed surface). The reason for this is that in most solid modelers, a face cannot be joined to itself. The presence of closed or periodic geometry in Alias (not true for Granite) is another reason that geometry intended for transfer to Pro/ENGINEER must be stitched before export. Using stitch has the same effect as detaching the geometry to create two surfaces before writing the IGES or STEP file for Pro/ENGINEER.
To import Alias models into Pro/ENGINEER
Define Absolute Tolerance Process (STEP and IGES only)
Before importing any foreign geometry (such as models created in Alias) the Pro/ENGINEER user can change from the default Relative Tolerancing process to the Absolute Tolerance process. Before a foreign model (that is created anywhere other than Pro/ENGINEER) is imported into Pro/ENGINEER, the desired absolute tolerance can be set to the value that the incoming model was built to.
For example if the Curve Fit Distance in Alias was set to 0.002 mm, then set the Absolute Tolerance in the Pro/ENGINEER work session to 0.002 mm.
This option can be enabled by writing the line:enable_absolute_accuracy yes into the config.pro file of the working directory.
Once the option is enabled, go to the Setup section of the Pro/ENGINEER application and choose Absolute Accuracy, and set the units and numerical value of the tolerance you wish to work at, each time a new part is created.
This is important to ensure that the Alias-created model can be used in further downstream operations in Pro/ENGINEER.
Advanced data sharing techniques
The following are some suggestions for Alias modeling that provide enhanced inter-operability with Pro/ENGINEER.
Export individual “Features” from Alias
Because Pro/ENGINEER creates each element of a model as a feature, it can be very useful to import components of the Alias model as individual export files that can be manipulated in Pro/ENGINEER as individual import Features. Major components of your Alias model can be transferred separately so that they can be used to construct individual features within Pro/ENGINEER.
The advantage of this technique is that individual features can be “reordered” in Pro/ENGINEER to give added flexibility to the engineer. The Feature > Reorder command allows the user of Pro/ENGINEER to modify the sequence feature construction. This is useful during the engineering process. Additional “mechanical” features are added to the industrial design model and the result is based on geometry previously created.
The surface replacement technique can be very useful when the model is a mix of mechanical elements defined by an engineer and styling elements defined by an industrial designer. By replacing the styling elements of a Pro/ENGINEER model all of the parametric/feature information is retained for the mechanical elements. This allows for continued parametric editing, automatic dimensioning, and so on.
Exporting assemblies from Pro/ENGINEER in IGES format
When exporting assemblies from Pro/ENGINEER, there are four types of IGES output available: Flat, One Level, All Levels and All Parts.
With the Flat option, Pro/ENGINEER exports the entire geometry of the assembly in a single IGES file. All components are transformed into model space before exporting, but no hierarchy is contained in the IGES file. All geometry of the assembly exists in the Flat IGES file, and is correctly positioned in model space.
To help organize these files that have the potential of being very large, place each instance of a part within an assembly into its own layer in Pro/ENGINEER before exporting the assembly as IGES Flat. The layers are transferred as “levels” along with the assembly in the IGES file. The IGES levels are translated into ALIAS Sets. This means that the members of one set are all of the surfaces that comprise an instance of a part in the assembly.
The interface ID that was specified for each layer is the means by which Pro/ENGINEER layer information is transferred via IGES. IGES does not support names for layers. Layers in IGES are called “levels” and a level is identified by a number, not a name. This is why Pro/ENGINEER asks you to assign a number as well as a name to a created layer. The name is more useful within Pro/ENGINEER, but the number is important for data transfer.
When the IGES file is imported into Alias, the IGES level information is created as Alias Sets. To display the level information, go the Set Lister (Pick > from lister > SETS). Sets exist whose names have the format LEVEL#n, where n is the interface id that was specified in Pro/ENGINEER.
Outputs an assembly IGES file with external references pointing to the IGES files of its components. This contains only top-level geometry.
With the All Levels option, Pro/ENGINEER outputs n+ 1 IGES files, assuming that there are n parts or subassemblies in the assembly. There will be one IGES file for each part or subassembly (for a total of n IGES files) and one master IGES files that contains external references (IGES entity 416 form 1) to the n-component IGES files. Each external reference to a component IGES file within the master IGES file is contained within an IGES Subfigure Definition (entity 308), which is instanced once by an IGES Subfigure Instance (entity 408). The model of each component referenced by the master IGES file is in definition space; that is, placed at the origin. Each component is transformed into model space via the transformation contained in the Subfigure Instance (entity 408) in the master IGES file.
If the n-component IGES files are individually imported into Alias, the resulting model will be incorrect, since each component will be placed at the origin, rather than the correct spot in model space.
If the master IGES file is imported into Alias, there will be no model at all! This is because Alias does not support the IGES External Reference (416 form 1) entity. This entity is generally frowned upon because it contains the filename of the component IGES file, and filenames are generally not portable between operating systems.
Outputs an assembly to IGES as multiple files containing geometry information of its components and assembly features. These parts use the same reference coordinate system to ease reassembly in the receiving system.
