Japan Automobile Manufacturers Association (JAMA) IGES is a subset of IGES. Therefore any receiving system, including Solid Edge, will read JAMA IGES files.

While IGES is large and broad in nature, JAMA was designed to be a trimmed back, more robust version of IGES. Because it is a subset, it does not support some entity types, such as type 120 Surface of Revolution. This means that almost all surface types in JAMA will be spline surfaces.

Before you save Solid Edge files to IGES, you should become familiar with the capabilities of the receiving system. Review a list of supported entities from the system's translator documentation, such as a user's manual. Check to see if there are specific entities that the receiving translator has difficulties reading.

When you create an IGES file, be sure to avoid entities the receiving system cannot handle. Set options to customize your IGES file for specific entities based on the capabilities of the receiving system. For example, you may find that the receiving system does not support the Manifold Solid Brep entity type 186. Therefore, it is necessary to output the Solid Edge model as trim surfaces.

After you save a file to IGES, review the resulting IGES output and the data in the log file. Compare the options used in the translation to the options you intended to set.

Open the resulting IGES file in Solid Edge to see if it contains what you expect. Request a report, such as a copy of the log file, from the receiving system.

Record the options and maintain these records. They will be useful in future translations.

It is important that you get the best possible results when you import IGES files into Solid Edge. To do this, the IGES file must be clean and free from discrepancies of the sending system.

To ensure that the IGES file is valid for the translation, use proper options when you transmit the file between systems or from differing media. If the sending system is able to check or validate its geometry for errors, do so. Fix any existing problems before translating the file.

You should clean up the file you want to translate before conversion. Delete items such as associated drawings, annotations, or construction geometry. Keep only the information that you intend to translate.

When setting the options to export to Solid Edge, the following IGES entities should be exported:

• All Rational B-Spline Surfaces as type 128

• All Rational B-Spline Curves as type 126

• All B-Spline surfaces as type 128

• Trimmed surfaces as type 144

If the above entity options are not available, set the export option to Unigraphics if available.

Once the file is translated, be sure to check the output. Review the data in the log file. Check the options you selected for translation and make sure the results are correct. If you find errors, investigate the cause.

Save the translated Solid Edge file in IGES (.IGS) format and check the resulting file to see if it contains what you expect.

Record the options and maintain these records to use in future translations.

If you discover errors in your translation, you should analyze the problem and determine where the problem occurred. When analyzing the problem, you should consider:

• Are there any errors in the IGES log file?

• Was there a problem in the loop test back into the sending system?

• Did you receive errors from the receiving system?

If the log file contains error messages, try to remove the feature causing the problem. After removing the feature, try to resave the file in IGES format. If this solves the problem, investigate the geometry in the problem feature. Consider using another method to construct the feature. If no other creation methods exist and the feature is not necessary for the translation, remove it. As a general rule, the problem must be resolved before you can continue with the translation.

Although this is not always a conclusive test, it does serve as a good indicator that you are on the right track. If this process fails to read the file correctly, investigate the failed features. Determine if the failed features are necessary for the translation, and if they can be created with less complexity.

The receiving system may complain or list entities that are not supported. Use different options to change unsupported entities to other corresponding entities. The receiving system may also report errors and record numbers of the unsupported entities in the IGES file. These record numbers may be useful when you research the problem.

Most CAD systems do not support the IGES definition of a Manifold Solid Brep Object (IGES Type 186). Therefore, they must rely on translating solid models as Trim Surfaces Type 144. Trim surfaces are simply a surface and a trimming curve. During IGES to Solid Edge translation, these surfaces are stitched, and the surface normals are then oriented to form a solid.

Stitching is performed on the entire collection of trim surfaces in the IGES file. Several passes at stitching are attempted based on a starting and ending tolerance and a number of attempts value. The following are examples of how these tolerances are defined.

Start At:1e-006 meters 
End At: 0.001 meters
Number of Attempts: 10

Beginning with the starting stitch tolerance, Solid Edge attempts to sew the collection of trim surfaces. If Solid Edge cannot create a valid solid body, it makes a second attempt by adjusting the stitch tolerance by the predetermined tolerance value. This process continues until a valid solid body is created or the ending stitch tolerance is achieved.

Geometry that fails to stitch is usually related to tolerances, poor surface quality, or an open surface definition.

Geometry that fails to stitch becomes construction geometry. Because it is construction geometry, you cannot add new features or remove existing features. However, this does not mean that you cannot use the translated data in Solid Edge.

You can use construction geometry in the following Solid Edge commands:

If the translated geometry forms a single sheet, you can use the Thicken command to apply a uniform thickness to the sheet and create a solid from the construction geometry.

If the geometry represents a sheet metal part, such as a flange or tab, you can use the Save as Flat command in the Sheet Metal environment to flattened and convert it to a solid. You can use the Save as Flat dialog box to save the geometry as a sheet metal (.PSM) file. Solid Edge converts the construction geometry to the flat state of a solid and creates a sheet metal file. The bends are added automatically, and you can use the Rebend command to fold the file into a 3-D sheet metal model. You can then add sheet metal features like flanges and dimples to the converted model.

You can use the Drawing View Wizard command to create a drawing view of the construction geometry. In most cases, you can use this geometry to create a detailed drawing.

You can use PathFinder to place construction geometry in an assembly just as you would use solid geometry.

Perhaps your workflow only consists of building enclosures or fixtures from the imported geometry. You can use the Create In-place command to place the construction geometry in an assembly file and create a new part file. The Create In-place command allows you to use the Include command to include edges from the construction geometry to create a new part file.

The seiges.exe executable, found in the Solid Edge Program folder, allows you to translate multiple IGES files for both import and export through a standalone interface. The executable is not referenced from the Solid Edge product, but it does contain options similar to the IGES Import and IGES Export Translation Wizards, except it allows you to specify a list of files to be translated.

The following is a list of IGES entities that are supported by Parasolid.

*Only for IGES Read

• Saving Solid Edge documents to other formats

• OLE for Design and Modeling and Translation

• Working with foreign data

• Opening foreign files in Solid Edge

• Open command

• Open command

• Save command