Pin numbers in Schematics

radgoate wrote on Thu, 11 February 2010 08:46

Hi, Can anyone throw some light on how I can get the components' Pin

Number (not name) for a NET from within a ULP?

I've looked at the object definitions in the Help pages, but pin

numbers are not mentioned at all.

If you just want a netlist and don't care about the format (other than

being readable) then from the PCB editor (and schematic too I think) choose

File->Export->Netlist.

If you're trying to create your own netlist using a ULP then I'd suggest

finding one in the ULP download area at CadSoft and then using that as a

starting point.  It definitely can be done that way, I have done it myself

though I don't remember the exact details off the top of my head.

Cheers,

James.

--

James Morrison  ~~~  Stratford Digital

email:  james@eaglecentral.ca

web: http://www.eaglecentral.ca

Specialising in CadSoft EAGLE

• Online Sales to North America

• Electronic Design Services

• EAGLE Enterprise Toolkit

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

James,

Thanks for swift reply. Maybe I should have said that I've downloaded the

netlist_protel_ulp, but it outputs pin names, and protel requires pin

numbers... I want to modify the code so it works correctly.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Dave schrieb:

Thanks for swift reply. Maybe I should have said that I've downloaded the

netlist_protel_ulp, but it outputs pin names, and protel requires pin

numbers... I want to modify the code so it works correctly.

Maybe it's just a question of nomenclature...

The information you are looking for is called the "pad name" in EAGLE.

It should be possible to get the associated package from the schematic

device, then access its pads and then their names.

In many (most of the) cases the pad names are numerical. However, you

should think about what to do when they are not, if Protel really needs

numbers there...

Tilmann

Thanks Timann - I'll look for this in the help files.

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Tilman,

The pad name only applies to boards, not schematics.

It must be possible to obtain the pin number, because the in-built netlist

exporter outputs those values as 'pad' in column 3...

Can someone explain how to navigate the object hierarchy to get the pin

numbers from the package relating to pinref of the the component in the net

being processed here:

   SCH.nets(N) {

     numeric string Part[], Pin[];

     int cnt = 0, index[];

     N.pinrefs(P) {

       Part[cnt] = P.part.name;

       Pin[cnt] = P.pin.name;

       cnt++;

       }

     if (cnt) {

        sort(cnt, index, Part, Pin, PinText);

        printf("%s\n","(");

        printf("%s\n",N.name);

        for (int i = 0; i < cnt; i++)

            printf("%s%s%s\n",Part[index[i]],"-",Pin[index[i]]);

        printf("%s\n",")");

        }

     }

   }

Thanks

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Dave schrieb:

The pad name only applies to boards, not schematics.

But it is referenced in the schematic as well (and is also displayed in

the schematic as well, even if there's no board at all).

It must be possible to obtain the pin number, because the in-built netlist

exporter outputs those values as 'pad' in column 3...

 

Can someone explain how to navigate the object hierarchy to get the pin

numbers from the package relating to pinref of the the component in the net

being processed here:

I'm pretty sure it is possible, but I'm not used to writing ULPs...

Perhaps you have a look at the following object hierarchy:

- UL_SCHEMATIC has a loop member named "part", of type UL_PART

- UL_PART has a loop member named "device", of type UL_DEVICE

- UL_DEVICE has a loop member named "gates", of type UL_GATE

- UL_GATE has a data member named "symbol", of type UL_SYMBOL

- UL_SYMBOL has a loop member named "pins", of type UL_PIN

- UL_PIN has a data member named "contacts", of type UL_CONTACT

- UL_CONTACT has a data member named "pad", of type UL_PAD

- UL_PAD has a data member named "name", of type string

- UL_PIN also has a data member named "net", of type string,

  as well as a data member named "name", of type string

By following this hierarchy with the appropriate loops and references,

you get all pin/pad/net relations you need.

Tilmann

Tilmann,

Thanks for the help. This now works:

if (schematic) schematic(SCH) {

   output(filesetext(SCH.name, ".NET")) {

   SCH.parts(P) {

     printf("%s\n","[");

     printf("%s\n",P.name);

     printf("%s\n",P.value);

     printf("\n\n\n%s\n","]");

     }

   SCH.nets(N) {

     numeric string Part[], Pad[];

     int cnt = 0, index[];

     N.pinrefs(P) {

       Part[cnt] = P.part.name;

       Pad[cnt] = P.pin.contact.name;

       cnt++;

       }

     if (cnt) {

        sort(cnt, index, Part, Pad);

        printf("%s\n","(");

        printf("%s\n",N.name);

        for (int i = 0; i < cnt; i++)

            printf("%s%s%s\n",Part[index[i]],"-",Pad[index[i]]);

        printf("%s\n",")");

        }

     }

   }

}

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Dave schrieb:

Thanks for the help. This now works:

Thanks for the feedback. However, your "attachment" can't directly be

accessed since that stupid web interface puts it UUencoded into the

message body. If you want to share it, please provide it to CadSoft for

their downloads webpage.

Tilmann