6

Pro/Engineer Data Transfer

In This Section:

• ALIAS to Pro/ENGINEER via IGES/STEP 140
• Pro/ENGINEER to Alias via IGES/STEP 150
• Pro/ENGINEER to Alias via Pro/RENDER 154

ALIAS to Pro/ENGINEER via IGES/STEP

Studio surface models can be transferred to Pro/Engineer via either IGES or STEP, depending on the availability of the transfer formats to the Studio and Pro/Engineer user. Using Studio, there are two types of model information that can be sent to and read by Pro/Engineer: geometry information and topology information.

The Studio IGES file includes only the description of the geometry information. The STEP entities that Studio supports means that both the geometry information as well as the topology information can be transferred and read into Pro/Engineer. 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 STEP file format has advantages over IGES when transferring Studio models to Pro/Engineer because there is more information describing the model that is being transferred.

Creating the IGES file in ALIAS

Follow these steps to create an IGES format file for Pro/ENGINEER:

1

Select the object to be exported so that it is the "active" object.

2

From the File menu, select Export > Active As.

3

Select IGES from the File Format pop-down menu.

4

Select pro_engineer from the IGES by Vendor browser.

The configuration of the output variables for Pro/ ENGINEER have been determined through data exchange testing to provide the best conditions for the creation of a solid model within Pro/ENGINEER. You can alter the output variables to achieve different results.

5

Select the Save icon and specify the IGES file name. ALIAS automatically appends the .igs extension to the file name.

The file is now ready to be read into Pro/ENGINEER.

Creating the STEP file in ALIAS

Follow these steps to create an STEP format file for Pro/ENGINEER:

1

Select the object to be exported so that it is the "active" object.

2

From the File menu, select Export > Active As.

3

Select STEP from the File Format pop-down menu.

4

Select AP214 from the Application Protocol.

5

The Studio model should have already been stitched into a solid shell (volume) or a shell (group of stitched surfaces that do not describe a volume.

Select under the Model Type either:

Manifold Shells- A collection of stitched surfaces that do not describe a volume is saved out as a G3 Manifold Shell.

or

Brep Solids-Stitched geometry that describes a closed volume is written out as a G5 Brep Solid.

6

Select the Save icon and specify the STEP file name. Studio automatically appends the .stp extension to the file name. This file is now ready to be read into Pro/ENGINEER.

Importing the IGES/STEP file into Pro/ENGINEER

This section provides a few instructions for importing Alias IGES/STEP files, viewing, and converting them to a solid model. This is not a substitute for having real training with Pro/ENGINEER, but basically a "cheat sheet".

Importing a 3D IGES/STEP file into Pro/ENGINEER and creating a solid from the surface geometry is a two-step process.

First, the import file is read into Pro/ENGINEER and a wireframe model is created from the data. This is known as an IMPORT FEATURE.

The second step depends on what data is available from the import file for converting the wireframe model into a Pro/ENGINEER solid model. Surfaces need to be joined or "quilted" in order to construct a solid model.

Step 1: Creating an IMPORT FEATURE from the IGES/STEP file

Follow these steps to import the IGES/STEP file into Pro/ENGINEER and create an IMPORT FEATURE.

1

To starting Pro/ENGINEER from the shell window, type pro

2

From the MODE window, choose Part

3

From the ENTERPART window, choose Import

4

Type in a filename and hit Return

5

From the IMPORT menu, choose IGES In/STEP In

Type in the pathname relative to your login home directory with the filename. You may also enter a "?" character, and then choose the Unix file name and path from a file lister.

Once the file has been loaded, an import log is displayed. For testing purposes, it is important to note is any entries show up in the "unconverted" list. These entries indicate an entitythat is not coming across and may need to be investigated depending on the results of the translation. In most cases, entities that are not processed are associative rather then geometric and do not affect the results of the translation.

6

Type "q" to quit

This action closes the log window and the system displays the result of the translation as an IMPORT FEATURE. A message appears indicating that an IMPORT FEATURE has been created successfully.

IMPORTANT: The Pro/E user must change from the default Relative Tolerancing process to the Absolute Tolerance process. If you have imported any foreign geometry (such as Alias Studio models) into Pro/E, you should change the tolerance process from the default Relative Tolerancing process to the Absolute Tolerance process. 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/E application and select Absolute Accuracy each time a new part is created.

Step 2: Creating a Solid

The resulting IMPORT FEATURE may be defined as a closed solid, surface quilt or a partial surface quilt. The color of the wireframe display indicates the status of the object: white for closed solid; pink for quilted surfaces; yellow for unquilted surfaces.

Closed Solid - A white wireframe display indicates a closed solid model and no further steps are required. Additional solid features may be added to the IMPORT FEATURE and manipulated parametrically.

Closed Surface Quilt - A closed surface quilt must have all wireframe edges displayed in pink. A closed surface quilt can be converted to a closed solid using the following steps:

1

From the PART menu, choose Feature

2

From the FEATURE menu, choose Redefine

3

From the REDEFINE IMPORT menu, choose Attributes > Make Solid > Done

• After a few moments, the wireframe display color changes to white indicating that a solid BASE FEATURE has been created.

Surface Quilt - A complete surface quilt has all internal edges displayed in pink (quilted) and a closed outer boundary displayed in yellow (unquilted). A surface quilt can be converted to a thin solid. A thin solid is defined as a surface or surface quilt that is offset to form a closed volume solid.

A surface quilt can be converted to a thin solid using the following steps:

1

From the PART menu, choose Feature

2

From the FEATURE MENU, choose Create > Solid > Protrusion > Use Quilt

3

Select the Thin option, and then choose Done.

4

"Pick" is the default selection in the GetSelect menu. Select the object at an edge with your mouse. It will be highlighted to indicate that it has been selected. An arrow appears indicating the direction of the solid model. Use the Flip or Okay menu to continue. At the prompt, enter the width of the thin feature.

5

The wireframe display color changes to white indicating that a solid BASE FEATURE has been created.

Partial Quit - A partial surface quilt may contain a combination of pink and a yellow edges. A pink wireframe display indicates quilted surfaces and yellow wireframe display indicates edges that may be quilted. All of the yellow edges must be quilted to construct a thin solid or closed solid. Surfaces can be quilted using the following steps:

1

From the PART menu, choose Feature

2

From the FEATURE menu, choose Redefine

3

From the REDEFINE IMPORT menu, choose Attributes > Fix Boundaries > Zip Gaps

4

From the SELECT CHAINS menu, choose Auto Select Surfaces boundaries that may be joined will be selected.

5

From the SELECT CHAINS menu, choose Zip Gaps > Accept

The wireframe display color will be redrawn in pink indicating that a surface quilt has been created.

Modeling for successful Pro/ENGINEER data transfer

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.

Getting 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 mm or inch unit 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 a number of 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.

Getting the topology right

The Surface Edit > Stitch feature within Alias creates a valid solid model topology within the ALIAS modeling environment. The stitching of surfaces within Alias can greatly improve the robustness of the interface to Pro/ENGINEER. The stitching process will also identify 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 will also identify duplicate surfaces in model and orientate the surface normals of the completed shell.

When models are constructed using the advance surface tools (swept, birail and square) it is quite common to create a number of 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.

Not all models are improved by stitching because some modeling techniques, such as trim intersect and round, create twin edges.

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 is another reason that geometry intended for transfer to Pro/E 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.

High Degree Surfaces

Surfaces that are greater then degree 3 are not supported by Pro/ENGINEER and are rebuilt during import of the transfer file. Within the ALIAS modeler, high degree surfaces are created when they constructed from high degree curves. Geometry being built in Studio with the intention of being exported to Pro/ENGINEER should not contain higher than degree 3 (cubic) surfaces or curves.

Advanced techniques

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

Exporting "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 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.

Incorporating Alias model changes in Pro/ENGINEER

This document will provide you with instructions on how to take specific IGES/STEP files created from stitched models in Alias, import them into Pro/Engineer, add details such as rounds and shells, then replace the import file with a new one that has been modified in Alias.

To Replace the IGES/STEP file with a new one:

1

From the FEATURE window, choose Redefine > By Table

2

From the SELECT FEATURES window, choose IMPORT FEATURE

3

From the BY TABLE menu, choose Done

4

From the REDIFINE IMPORT window, choose File

5

From the INTERFACE IMPORT menu, choose IGES/STEP

6

Type in the pathname relative to your login home directory with the filename. You may also enter a "?" character, then choose the Unix file name and path from a file lister

7

Type q to quit

This action closes the log window and the system displays the result of the translation as the replacement IMPORT FEATURE.

8

From the REDIFINE IMPORT window, choose Done

The new file appears in the main window and a smaller window in the upper right displays the old Import Feature. The default pairs of edges are highlighted.

9

Accept the default pairs by entering [Y]. If the topology of the replacement Import Feature has been altered, additional steps are required create a complete set of edge pairs. Use the Set Pairs command from the IMPORT PAIRS menu.

10

From the IMPORT PAIRS menu, choose Done

The features added to the original Import Feature will be placed on the modified Import Feature.

Pro/ENGINEER to Alias via IGES/STEP

Creating/Exporting an IGES file in
Pro/ENGINEER

Follow these steps to export a Pro/ENGINEER part file to the IGES file format:

1

From the PART menu, Choose Interface > Export > IGES

2

Type in a filename and hit Return

3

From the EXPORT OPTIONS menu, choose Done

4

Select a coordinate system to be used in the IGES file.

A message appears indicating that the export file has been created. Pro/ENGINEER creates an IGES file with the .igs extension. This file is now ready to be read into ALIAS.

When creating the IGES file in Pro/ENGINEER the igs_config.pro file should be used. You can access this file from the EXPORT OPTIONS menu. Edit your igs_config.pro file so that the options are as shown below:

Iges_out_all_srfs_as 128
Iges_out_spl_crvs_as_126 Yes
Iges_out_spl_srfs_as_128 Yes
Iges_out_trim_xyz No
Iges_out_mil_d_28000 No
Iges_out_trm_srfs_as_143 No
Iges_out_JAMIS_compliant No
Iges_out_trim_curve_deviation DEFAULT
Intf_out_blanked_entities Yes Intf3d_out_extend_surfaces No

Exporting Pro/ENGINEER Assemblies via IGES

When exporting assemblies from Pro/ENGINEER, there aree 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. See also the Pro/ENGINEER Interface Guide 18.0 page 3-9.

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). 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 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 (e.g. Unix > DOS).

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.

Creating/Exporting a STEP file in Pro/ENGINEER

Follow these steps to export a Pro/ENGINEER part file to the STEP file format.

1

From the PART menu, choose Interface > Export > STEP

2

From the EXPORT OPTIONS menu, choose "#" Done

3

Select a coordinate system to be used in the STEP file.

4

Type in a filename and hit return

A message appears indicating that the export file has been created. Pro/ENGINEER creates an STEP file with the .stp extension. This file is now ready to be read into ALIAS.

STEP configuration options

When creating the STEP file in Pro/ENGINEER the STEP configuration options are as shown below.

For more information see the Export Configuration Options for STEP table in the Pro/ENGINEER Interface Guide.

step_export_format

this can be set to either AP203_IS or AP214_CD

intf_out_max_bspl_degree

this value sets a maximum degree between 3 to 16 of exported bspline surfaces into STEP

intf_out_blanked_entities

filters export of entities based on their display status

intf_out_blank_layers

filters export of layers based on their display status

intf_out_layer_ids

allows the Pro/ENGINEER operator the option of assigning interface ID's for layers which were not assigned ID's during export

intf_out_layer_rename_table

enables user to assign interface ID's to layers during export

intf_out_as_bezier

exports B-spline and spline surfaces as Bezier

intf_out_default_option

controls the type of 3D data output through Pro/BATCH to a STEP file

intf3d_out_extend_surface

controls the extending of surfaces during export

intf3d_out_surface_deviation

sets a maximum allowable deviation in the process of converting Pro/ENGINEER surfaces to STEP

Pro/ENGINEER to Alias via Pro/RENDER

Creating the Render file in Pro/ENGINEER

Follow these steps to export a Pro/ENGINEER part file to the Render file format.

1

From the PART menu, choose Interface > Export > Render

2

From the RENDER menu, choose Output

3

Select a coordinate system to be used for the RENDER file.

4

Type in a filename and hit Return

A message appears indicating that the RENDER file has been created. Pro/ENGINEER creates an RENDER file with the .slp extension. This file is now ready to be imported into Alias.

Importing Pro/RENDER Files

The Pro/RENDER can be imported into Alias using FILE > Retrieve. Additional control for the translation is available from FILE > Retrieve > Pro/E Render Options.

The Pro/RENDER triangle data is converted into Alias Polysets. It is important that the Pro/ENGINEER designer assign each part of an assembly a different color, so that each part will become a separate Polyset in Alias. The colors are also translated into simple Alias shaders and these shaders are assigned to the appropriate objects.

Retrieve Options

Specifying Units

The units of the data in the Pro/ENGINEER Render File are not specified in the file. PRenderToAlias needs to know what the units are so that the model will be at the correct scale after it is imported into Alias. By default, PRenderToAlias assumes the data is in inches.

If the model was created in Pro/ENGINEER based on other units, these units should be specified using the -u option when the Render file is converted.

The -s option allows an arbitrary scale factor to be specified if desired.

The -g option simply groups all of the polysets created for a particular Render file. This allows several files to be retrieved in a row, with the geometry from each file in a separate group.

Specifying Tolerances

By default, PRenderToAlias may merge the vertices of triangles along apparent shared edges. If two vertices have the same x, y, z position within a tolerance and have the same normal within a tolerance, they are merged into one vertex. This allows Alias to do smooth shading across the edges. If two vertices have the same x, y, z position, but have different normals, then these vertices are not merged to maintain the hard edge.

The tolerance used for comparing vertex positions can be specified using the -t option. The value specified is in the same units as the data. For example, if you specified -uMM -t0.01, the tolerance for comparing vertex positions is 0.01 millimeters. If you change the units from the default inches, then the default tolerance of .0001 may have to be changed to make sense for the units specified.

The tolerance used for normal comparisons can be specified using the -a option. The value is specified in degrees and is the angle between the normals of two vertices. The default is that two vertices will be merged if their positions are equal within tolerance and the angle between the normals is less than 1 degree.

Specifying Vertex Normals

Vertex normals in Pro/ENGINEER Render Files all point towards the inside of objects. For rendering purposes in Alias, these normals must point towards the outside of objects. Consequently, the PRenderToAlias translator flips all vertex normals during the translation.

The vertex normals of polysets are usually recalculated by the Alias renderer before it renders polysets. By default, PRenderToAlias freezes the normals assigned to vertices in the Pro/ENGINEER Render file so that they are used by the renderer rather than discarded and recalculated. This allows the renderer to produce a better quality rendering. To suppress this behavior, specify -r so that the renderer will discard the Pro/ENGINEER assigned normals and recalculate them.

The stand-alone PRenderToAlias program

The stand-alone PRenderToAlias program converts a Pro/ENGINEER Render Format file into an Alias wirefile. PRenderToAlias can be executed in a Unix shell window.

Type PRenderToAlias -h to see the usage information:

PRenderToAlias

Arguments: [<options>] [<infile> [<outfile>]]

Options:

-s

scale Input scale factor (for example. -s2.0)

-u

Input units. Aceptable values are MI,FT,IN,MIL,UIN,KM,M,CM,MM,UM]. The default is
-uIN

-g

Group the geometry

-n

Do not merge vertices

-r

Recalculate vertex normals

-p

Merge vertices according to xyz position only

-t pos_tol

Specify merge vertices position tolerance value in input units. The default is 0.0001.

-a nrm_tol.

Specify merge vertices normal tolerance value in degrees. The default is 1 degree.

Where:

<infile> is a Pro/Engineer Render file. If it is absent, input comes from stdin.

<outfile> is an Alias wire file. If it is absent, output goes to stdout.

By default all vertices are merged according to their positions and normals.

Executing from the command line in a Unix shell window is outlined in the previous description, and the resulting wire file can then be retrieved into Alias V8.2.

Examples:

PRenderToAlias crankshaft.slp crankshaft.wire

PRenderToAlias -g -t0.001 hammer.slp hammer.wire