EDIF 200 Migration

The EDIF 200 Migration dialog allows you to import an EDIF 200 file to eCADSTAR Schematic Editor. EDIF (Electronic Design Interchange Format) is a vendor-neutral format in which electronic netlists and schematics are stored as a nested list of data. If successful, then the imported design is opened in a new instance of eCADSTAR Schematic Editor. Launch this dialog by clicking File > Migration > EDIF 200 on the ribbon.

File Setting

Value	Description
Edif File	Displays the path to the EDIF file that you specify by clicking .
	Allows you to select a .eds or .edf file in the displayed Open dialog. The path to the file is displayed in the EDIF File box.
Design Name	Enter the name of the design that is created in eCADSTAR Schematic Editor from the imported EDIF file. If an existing design name is specified, then the conversion is not done when you click Execute and an error message is displayed.
Design Location	Displays the path to the design that is created in eCADSTAR Schematic Editor. Specify the path by clicking .
	Displays the Select Folder dialog. This allows you to set the path to the design that is created in eCADSTAR Schematic Editor.
Scale	Allows you to change the scale of the imported design. Enter a Scale (multiplier) value between 0.01 and 100.0 by typing it in the Scale box or using the calculator. The default value is 1.0. Launch the calculator by pointing the cursor in this box and clicking the displayed Calculator button. A scale value (Scale (divisor)) is also defined in the EDIF file. The actual scale is produced as follows: Actual scale = Scale (multiplier)/Scale (divisor).

Results

Value	Description
Error log	Displays any errors relating to the migration. This indicates whether it was successful. If successful, then the message "Migration successful. There are no errors to report" is displayed.
View log	Displays the Migration View Log dialog. This shows any messages that are created when the EDIF file is imported, and allows you to copy them, print them or save them as a .rep file.

 

Value	Description
Back	Displays the File Setting section of the dialog.
Next	The schematic design is created in the specified location. It is named using the value in the Design Name box.
Finish	Closes the EDIF 200 Migration dialog after importing an EDIF file. The imported design is opened in a new instance of eCADSTAR Schematic Editor.
Cancel	Closes the EDIF 200 Migration dialog without importing an EDIF file.

 

 

Value	Description
Power and Ground symbols	POWER/GROUND components are converted to hierarchy connectors. This is because the EDIF file cannot distinguish between hierarchy and POWER/GROUND connectors. Hand editing is required after migration. OrCAD data does make this distinction, however, using the value in the OrCAD ground list, in the property conversion table.
Instance property	If multiple blocks of the same design are used with different property values in them, then these properties are not converted.
Character size	Only character height information is exchanged through EDIF. Character width and interval are not converted.
Duplicate component	Duplicate components are not converted.
Bitmap	Bitmaps in OrCAD data are not converted.
Color	The default value specified in the data resource for conversion is used as the color for each object.
Line Width	The default value specified in the data resource for conversion is used as the width for each object.
Line Type	The Solid Line Type is used in the data resource.
Hatching	The hatching pattern for polygons is always Solid.
Joined in Ripper symbol	Ripper symbols are supported that have two terminals (multiple pins). Rippers with two cross-connected pins are not supported.
Multiple Expressions	EDIF migration converts range notation characters that show multiple expressions. However, it does not fully cover the specifications of each vendor.
Net expression	eCADSTAR does not fully support all specifications of the various vendors, such as those including duplicate expressions. EDIF migration can only load those that conform to eCADSTAR’s expression method.
Pins on a schematic sheet	eCADSTAR does not place pins on a schematic sheet. Pins are generated on a schematic sheet, and data for connecting nets is generated after being replaced with connector symbol pins.
Negative logic expression characters	Negative logic expression characters are not converted.
Variable net label and frame	Variable repetition expressions (frame and net in MENTOR EDIF) are not converted.
Design variation	Design variation data is not converted.
Gate and split symbol	Because eCADSTAR uses different gate and split symbol expressions from OrCAD, they cannot be converted as gates and split symbols. Manual correction is therefore required after conversion.
Composite symbol (*)	Because eCADSTAR does not have a concept of OrCAD composite symbols, symbols contained in composite symbols are placed individually. Unlink OrCAD, eCADSTAR does not handle composite symbol as single symbols. Note that in OrCAD, even if symbols are registered as separate in the library, a symbol can be combined with another on a sheet, and handled as a single symbol.
Compound type	Only Single-thickness lines are supported by eCADSTAR.
Begin arrow type and End arrow type	Arrows are not supported in eCADSTAR.
Hierarchy block	In EDIF, there are no other concepts than link-type blocks. However, eCADSTAR converts them as embedded type blocks. After conversion, it is recommended that the Definition block is deleted.
Multiple circuits	If there are multiple circuits at the top of a design, then only the circuit set at the top is edited.
Footprint settings on local parts	The generated local part has no footprint settings. There are also no pin assignment settings. Set these using Library Editor.