Orcad capture to expedition PCB

[mauriziomontesi]

orcad to expedition

Hello, I have a Orcad Capture schematic. I'd like to use expedition PCB as a routing tool. I need information about the procedure to do that. In Orcad capture I can generate lots of netlist but I don't know how to link parts (I have build again symbols in dxdesigner format, then create parts, or I can use the orcad symbols + cell in library manager??
Thanks in advance

 

[senilicus]

expedition pcb

Integrate OrCAD schematic with Expedition PCB layout


Solution

WG2000.5 and earlier:

There is no direct integration between OrCAD and Expedition PCB.

Have the necessary Padstacks, Cells, and Parts ready to go in the attached Central Library.
Create an EDIF 2.0.0 netlist in OrCAD.
In Expedition, use File>Import>EDIF netlist to import the netlist. This creates a CAE netlist that can be used to drive the layout.
On the Project Integration dialog, edit the Project File. On the Netlist tab, select type "CAE Netlist" and then browse the file system to the location of the netlist created in step 2.
Note: Customers using the EDIF 2.0 Netlist need to be aware of its limited character set. Typically, the EDIF 'cell' will translate to Expedition as the Part Number. The EDIF 'instance' becomes the Reference Designator. If the EDIF import fails, consult the edif_nr.txt file. The following characters, when used in the EDIF cell and netnames will stop the design: whitespace ' ', a period or dot '.', the minus sign '-', the plus sign '+', forward_slash '/', back slash '\' and number sign '#'. If these exist in the EDIF 2.0 netlist, the translation will not complete and the EDIF netlist file will need to be modified and these EDIF special characters replaced.



OrCAD can generate an Intergraph .net netlist. This is essentially a keyin netlist and can be renamed to .kyn. Using the the Project Integration's Project Editor (see above), select the netlist type to "Keyin Netlist" and then browse the the file system for the .kyn file.


WG2002 and later:

The OrCAD to Expedition Interface is a separate product that needs to be installed. The software is located on the WG2002 Service Pack 1 CD. The Product is called "OrCAD-Expedition interface". It uses a separately purchased license that requires a "wgorcadexpif" feature in the license file. There are also a number of constraints to the interface that are covered in the OrCAD to Expedition PCB Interface on-line help.

The interface requires the following installations:

OrCAD Capture 7.2 or above
Expedition PCB WG2002.1
The interface works on the following Operating Systems:

Windows 2000
Windows XP
Constraints of using the interface:

OrCAD capture and the interface need to be located in the same system.
The entire directory tree of the OrCAD schematic and Expedition PCB designs must be located on the same system.
The interface assumes that the Expedition WG2002.1 and OrCAD Capture version 7.2 or above are used.
Does not address the library translation between OrCAD and Expedition.
Constraints of using OrCAD Capture with Expedition PCB:

Expedition PCB requires unique part names. You cannot have two parts in a schematic with identical names and a different number of pins.

 

[mauriziomontesi]

orcad capture expedition pcb

Thank you very much!!!