Allegro Netlist import

Schematic
1

Hi,

after using OrCAD/Allegro for over 25 years, we decided to slowly
go away from OrCAD and use KiCAD for our schematic/layout system.
We want to start drawing the schematics in KiCAD, generate a Allegro
netlist and do the layout in Allegro.
I created a small design, to test the Allegro netlist export in KiCAD Schematic.
The netlist is generated without errors.
However if I load the netlist in Allegro, I get lots of errors.
I use my own symbols and footprints. I know they are working as I use
the footprint from OrCAD.
Has anyone successfully been able to import a netlist in Allegro?
I have attached the KiCAD schematics and the logfile from Allegro.

Cheers,

Ralf

clock_recovery.kicad_sch (115.7 KB)
netin.log (10.6 KB)

2

There have been a few issues opened on gitlab for the allegro exporter:

But there are not many issues. I guess it’s not used very much.

I can’t do much with your log file (It’s also something I don’t know much about). It seems more sensible to me to do a KiCad export, and a netlist generation from allegro itself, and then compare them. The netlist can be very simple to start, such as a single shorted resistor, or a resistor parallel to a capacitor.

The issue that resulted in the creation of the Allegro netlist exporter is:

And it would be nice if “stuff” can be exchanged between all software, but combining the schematic program of one EDA suite with the PCB module of another is likely to raise issues. To me it makes more sense to start with a whole KiCad project (both schematic and PCB) for evaluation.

You are also mentioning:

but KiCad has two different netlist exporters. One for “Allegro”, and one for “OrcadPCB2”

3

Hmm yes I see some format errors in the output

4

Can you try this netlist after fixes to the exporter?
clock_recovery.txt (1.1 KB)

5

@paulvdh
Yes, it looks like not many people use OrCAD/Allegro. The last Issue from Mr. B " exporter netlist allegro", makes me wonder if the netlist generation is correct and I think he is right. If I export a netlist from Allegro I have footprints in the first field.
Using KiCAD for Layout is currently not an option. As I wrote I use OrCAD/Allegro since several years and have created footprints, which are verified and proven to work and are verified.
I use KiCAD 9.04 and the Allegro netlist exporter.

@marekr
Thanks for the netlist. I tried it and I get less errors. But it is still not working.
I have attached the error logfile from Allegro. Maybe it helps.

netin.log (2.5 KB)

I also have attached a netlist from a simple Allegro Layout, where you can see
the first field has the footprint.

netlist.txt (1.4 KB)

Ralf

6

So I guess your experience from your experiment is allegro ma non troppo? :wink:

Anyway hope your efforts result in a better exporter. :crossed_fingers:

7

@marekr
I played with your netlist and find out instead of “$NET” it should be “$NETS”.
I also removed the ROOM section in “$A_PROPERTIES” after I still got errors
during import.
With these changes I was able to import the netlist.

Ralf

ps: I have attached the netlist generated from Allegro, after successfully
read your changed netlist in. As you can see, the first field contains the
footprint.
netlist.txt (1.2 KB)

1 Like
8

Got it, adjusted NET to NETS. That should all be fixed in the later 9.0.5 release.

Can you try this one? $A_PROPERTIES should actually have been right after $PACKAGES rather than $NETS
clock_recovery.txt (1.1 KB)

1 Like
9

With your latest attachment I was able to successfully import the netlist into Allegro
and place the components. I’ll wait till 9.05 is out (hopefully soon) and try it again
with a more complex board.

Thanks,

Ralf