Pads Netlist generation

External Plugins
1

Hi Guys,

I have installed KiCad 7.0.9, I am trying to generate PAD PCB netlist from the KiCad. But i observed there is no pads plugins available in the pluggins folder. Could someone guide how to generate the Pads supporting files(.asc format) and if someone have PADs script please share with me.

Thanks in advance

2

Have you already read this?

3

In this 7 year old thread, someone wrote a python script to generate a pads netlist.

4

You appear to want to get an “.asc” file from a PCB.

“.asc” is an LTSpice file and, Kicad cannot Export Netlists from a Kicad PCB. Kicad exports Netlist from the Schematic, not from PCB.

If you create a kicad schematic, you can export a Netlist then (with a couple of click’s) use it for LTspice (I won’t post here how to do that - it’s pretty easy to do).

Is that what you want to do? If so, first create your schematic and we can continue from that…

First, do a very simple circuit to ensure you grabbed usable Symbols for Spice…

5

Hi @BlackCoffee

Thanks for your quick response.

i am looking for the pads supporting netlist (.asc file) from the schematic not from the PCB. But i am unable to find Pads netlist option from the netlist generator tab. Could you please guide how to generate .asc file from the kicad schematics.I have designed a small circuit. i have generated the netlist but it is in .net format but i want .asc format. Please help me to generate .asc file from the schematic.

Thanks in advance.

6

@Srikanth

These are a bit outdated but still contains what you need to know and how to do it.
Link 1

Link 2

Let me know if needing help…

7

You may have been looking for the PADS PCB ASC plugin from previous versions, which has been replaced with a Python only version per export netlist to PADS_PCB does not work (#12057) · Issues · KiCad / KiCad Source Code / kicad · GitLab

but the Python version should be able to be loaded, though perhaps you need to import it first? The file still appears in the source code at eeschema/python_scripts/netlist_form_pads-pcb-asc.py · master · KiCad / KiCad Source Code / kicad · GitLab

8

Please note that this Not the LTSpice file type in this case, OP apparently really does want a PADS netlist file that happens to have the same file extension as the LTspice .asc.

9

thanks… I guess there are different kinds of Motorcycles, too! I know only Harley’s

10

@Srikanth Setting aside ‘why’ and for ‘what purpose’, Generating a Netlist from schematic is:

  1. In the Schematic, File>Export>Netlist

Choose the one you want. If it’s not listed, Add Generator (and find you script). This creates a new Tab…

11

I managed to get a PADS netlist (I think), but you have to download the script from gitlab, put it into the hidden Kicad folder, then add the generator. It produces a .net not a .asc file.

It would be a lot easier if the script was installed with Kicad, perhaps the reason it isn’t is because it is buggy/unsupported?

12

Hi @BlackCoffee. I am planning to use kicad for schematic design. But my layout team is using pads software. They are importing .asc file to the pads. So now i am planning to generate .asc file from the KiCad schematics. Now i am trying to find script for the pads netlist.

Thank you.

13

Hi @bobc,

Thanks for the response.
If you have pads script, could you please share with me?

i have searched in Github unbale to find the proper script.

Thanks in advance.

14

Download that file and copy to C:\Users\bobco\AppData\Local\Programs\KiCad\7.0\bin\scripting\plugins or whatever the equivalent is on your system.

15

It is odd that PADS netlist is no longer included in the normal install as a tab in the Netlist Export section… I think you might be right that the netlist scripts don’t all work. I don’t even see any of the netlist export scripts shown on the master branch in my installation of KiCad v7.0.8 or the nightly installation of v7.99.

image
image3084×1994 693 KB

The OrCADPCB netlist export just generates a .net from KiCad, so that one doesn’t seem to work. The CADStar netlist export does generate something unique, so I assume that one works. Presumably Spice and Spice Model work, as the ngspice integration relies on them. (I’m not even sure how the CADStar netlist export is working, since there isn’t an obvious python script in the relevant folder.)

I tried manually installing the PADS PCB netlist generator linked above, it does not work for v.7.0.8, but does appear to work for v7.99.

All in all, seems like there’s at least one bug here. One issue is that the Python scripts for netlists are not getting copied into the installers during release build. (Maybe intentional?) The second issue is that the netlist exporters have regressed from v6 in the sense that the default tabs do not all work and the PADS PCB netlist default option is missing.

EDIT: A warning for OP, please make sure you make a backup in case you choose to use the development nightly version v7.99 to do this netlist export, as you Cannot return to the stable v7.0.x series after saving your files in v7.99.

16

Thanks everyone.
This python script is working for generating netlist which is compatible to pads.

17

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.