Possible to layout Orcad schematics in Kicad?

[vulcanraven188]

I was thinking about using Kicad for laying out boards from now on, but I had an issue. All of my schematics are in Orcad. Is it possible for kicad to take an orcad schematic and start laying it out? Or do I have to recreate schematics on kicad. I know pads can take orcad schematics, but I wasn’t sure about kicad. An answer to this would be so helpful.

[coolp_jim]

You’ll need to compare netlist output via Kicad vs. Orcad and make sure the Orcad netlist matches up to what Pcbnew expects to import. If it were me I’d just redraw it in Eeschema and stop paying for the Orcad license.

Unless there’s a tool that exists to convert them, no you can’t. I just keep editing… I just checked, PADS netlist import needs some plain text format, Pcbnew netlist import is more .xml based.

[PCB_Wiz]

@vulcanraven188

Is it possible for kicad to take an orcad schematic and start laying it out?

As above, I’d export all the NETLIST choices from OrCAD, and then use the one that is easiest to parse, or has the most information.
NETLIST formats are usually quite simple.

Because KiCAD can import PADS (some minor header fixups may be needed), that’s probably a good place to start.

What you will likely need to do, is some sort of table for footprints mapping, so that whatever name OrCad used, can be replaced by the KiCAD library name.
Then, you need to check for things like alpha-pin names, and how those match up.

Some useful reading around NETLISTS

Pcbnew without eeschema (again)

Hi All, I have never used KiCAD, and I am trying to determine whether it’s the right tool for me. From other threads, I understand that the standard KiCAD practice is to feed pcbnew with a schematics file generated from eeschema, i.e. pcbnew is not stand-alone. For a number of reasons, instead of that, I’d like to create any of this (like for example netlist information and footprint details) from non-graphical tools such as a text editor, custom scripts, etc. I’d then use pcbnew to draw my a…

[erichVK5]

there are a few possible options

1)(a) see if your schematic converts to a gEDA gschem schematic with an Orcad->gschem utility called Sarlacc, which requires an older 16 bit export format, it seems, consisting of

sarlacc_schem and sarlacc_sym

found in the geda-gaf package, i.e. see

rlutz/geda-gaf/blob/master/utils/README

rlutz/geda-gaf

followed by

1(b) exporting a kicad netlist from gschem

i.e. with something like:

http://www.gedasymbols.org/user/frank_miles/gnet-kicad.scm
or
http://gschemfinalizer.sourceforge.net/
or easiest of all
load the gschem generated netlist into pcb-rnd, which can save as a KiCad layout

or

2. generate some good example screenshots of some schematics that go with some corresponding generated netlists, zip them up, and have a chat with the lead dev at http://repo.hu/projects/pcb-rnd/ who has developed some very modular netlist import module code for pcb-rnd. With your help, a netlist import module could be coded very quickly, after which pcb-rnd can then layout the board, or export a layout in KiCad format for you. Mentor graphics netlist import was recently implemented very quickly with the aid of exemplar schematics and screenshots provided by a Mentor graphics user.

3. implement orcad netlist import code in KiCad

4. write a conversion script, or modify Sarlacc if the Orcad format hasn’t changed much since Sarlacc was written, to convert the schematic directly into an eeschema schematic.

5. further reading:

http://thread.gmane.org/gmane.comp.cad.geda.user/44292

FOSS ftw.

Regards,

Erich.