Pro/ENGINEER
 
 
 

PTC Granite™, IGES, or STEP file formats can be used to transfer AliasStudio models to or from Pro/ENGINEER Wildfire.

Pro/ENGINEER Requirements

Model Preparation

Units

When working in Pro/ENGINEER set the Units to be the same as what was used in the AliasStudio model.

Geometry/Topology

When using AliasStudio two types of model information can be sent to and read by Pro/ENGINEER. Those two types are geometry information and topology information.

The Studio-created IGES file includes only the description of the geometry information. The Studio-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 AliasStudio and Pro/ENGINEER, geometric data is represented using NURBS.

Topological data describes how the geometric components are connected together to form a solid. The AliasStudio STEP file format has advantages over IGES when transferring AliasStudio models to Pro/ENGINEER because there is more information describing the model that is being transferred.

Tolerances

Information specific to IGES

Information specific to Granite

NoteThe translation time of rational geometry (for example, exact radius surfaces) is longer than the translation of non-rational geometry. In AliasStudio, you can create non-rational surfaces and translate them into PTC Granite.
TipCurve Fit Distance is the key to translation quality. The recommended tolerance in the Preferences > Construction Options - Construction Preset - Tolerances > Fitting is based on testing done translating models between AliasStudio and Pro/ENGINEER.
TipMaximum Gap Distance is the value that is used to check if the adjacent boundaries are built closely enough to each other.They should never be smaller than the Curve Fit Distance.

Workflow

Before transferring geometry between AliasStudio and Pro/ENGINEER, you should consider the purpose of the transfer to plan an appropriate workflow. When you import your AliasStudio 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 AliasStudio supplied data. The AliasStudio supplied data must satisfy the Pro/ENGINEER's rules for topological and geometric data.

Get the geometry right

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.

NoteThe maximum distance or gap between the surfaces of your model must be less than the accuracy defined within Pro/ENGINEER for successful joining of surfaces. The Pro/ENGINEER system defines accuracy as a value less than the ratio of the length of the smallest edge of a part divided by the length of the largest side of a part.
NoteYou can lower the part accuracy to join surfaces successfully when the gap exceeds the required tolerance. However, we recommend that your AliasStudio models are constructed to within the accuracy defined by the engineering requirements of your organization.

A recommended tolerance to maintain during transfer from AliasStudio to Pro/ENGINEER is dependent on the size of the part being described. AliasStudio 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 AliasStudio 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 AliasStudio 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.

Get the topology right

The AliasStudio stitching operation is recommended to be done on geometry being prepared for transfer to Pro/ENGINEER.

The Surface Edit > Stitch> Shell Stitch feature within AliasStudio creates a valid solid model topology within the AliasStudio modeling environment. The stitching of surfaces within AliasStudio greatly improves the robustness of the interface to Pro/ENGINEER. The stitching process also identifies surface boundaries that exceed the prescribed tolerances. These problems can then be corrected by the designer prior to the translation of 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 will automatically create 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 AliasStudio (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 AliasStudio models into Pro/ENGINEER

Define Absolute Tolerance Process (STEP and IGES only)

Before importing any foreign geometry (such as models created in AliasStudio) 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 AliasStudio was set to 0.002mm, then the Absolute Tolerance in the Pro/ENGINEER work session should be set to 0.002mm.

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 you must 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 AliasStudio-created model can be used in further downstream operations in Pro/ENGINEER.

Advanced data sharing techniques

The following are some suggestions for AliasStudio modeling that provide enhanced inter-operability with Pro/ENGINEER.

Export individual “Features” from AliasStudio

Because Pro/ENGINEER creates each element of a model as a feature, it can be very useful to import components of the AliasStudio model as individual export files that can be manipulated in Pro/ENGINEER as individual import Features. Major components of your AliasStudio 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.

Surface replacement

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.

Flat

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 there will be no hierarchy contained in the IGES file. All geometry of the assembly exists in the Flat IGES file, and it will all be 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 will be 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 AliasStudio, the IGES level information is created as AliasStudio Sets. To display the level information, go the Set Lister (Pick > from lister > SETS). You will notice there exists sets whose names have the format LEVEL#n, where n is the interface id that was specified in Pro/ENGINEER.

One level

Outputs an assembly IGES file with external references pointing to the IGES files of its components. This contains only top-level geometry.

All levels

With the All Levels option, Pro/ENGINEER outputs n+ 1 IGES files, assuming that there are n parts or sub-assemblies in the assembly. There will be one IGES file for each part or sub-assembly (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 AliasStudio, 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 AliasStudio, there will be no model at all! This is because AliasStudio 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.

All parts

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.

Detailed file format information

PTC Granite format (Windows Only)

STEP format

IGES format