Eagle netlist export problems

Ben Berkowitz wrote on Wed, 03 May 2017 10:31

I'm trying to export my Eagle schematic as a netlist that is readable

by Altium Designer (I use Eagle to develop schematic, contractor uses

Altium to do layout). I used the UDP called "netlist_protel.udp", but it

looks like a lot of times this UDP for some reason will list the pin

connection by the pin's name (ie "U7-ADC7") rather than the pin number

(ie "U7-22"). We've also tried Altium's Eagle file importer, and that

also creates errors. Does anyone have a better netlist exporter for the

purpose of getting a netlist into Altium?

 

--

To view any images and attachments in this post, visit:

https://www.element14.com/community/message/221544

The ulp you quote was created in 2001 so I would not expect that to be the

ulp you would need.

If no one can help straight away, your next move would be provide the

format document for what Altium is expecting.

Your current problem is with pin/pad. In Eagle the board has pads that are

most commonly numbered, matching the pin numbers of the package. You can

make this turn out right for you by renaming the pin names in the symbols

in the libraries to match the numbering of pins of the package. What ever

you do the Altium numbering of pins/pads will need to match your Eagle

library numbering so every device will need to be checked.

HTH

Warren

--

EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.

warrenbrayshaw wrote on Wed, 03 May 2017 05:23

You can make this turn out right for you by renaming the pin names in

the symbols in the libraries to match the numbering of pins of the

package.

That would solve the problem, but would also make the EAGLE library less

usable as the schematics would be less readable with pin numbers rather

than names showing. It would get the OP out of a hole if this export is

needed urgently though.

The netlist format required probably isn't too difficult so an up to date

export ULP could be written to do this properly without too much pain I

would think so long as the format of the netlist is specified somewhere or

easily derivable for some example files.

Best Regards,

Rachael

--

EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.

Ben Berkowitz wrote on Tue, 02 May 2017 23:31

I'm trying to export my Eagle schematic as a netlist that is readable

by Altium Designer (I use Eagle to develop schematic, contractor uses

Altium to do layout). I used the UDP called "netlist_protel.udp", but it

looks like a lot of times this UDP for some reason will list the pin

connection by the pin's name (ie "U7-ADC7") rather than the pin number

(ie "U7-22"). We've also tried Altium's Eagle file importer, and that

also creates errors. Does anyone have a better netlist exporter for the

purpose of getting a netlist into Altium?

Does the EAGLE importer create the same errors? If not what are they? I

believe the importer generates some log files which might help give a clue

as to what else may be going on.

Best Regards,

Rachael

--

EAGLE support forums at http://www.eaglecentral.ca :: Where the EAGLE community meets.

On 3/05/2017 8:25 p.m., Rachael wrote:

Ben Berkowitz wrote on Tue, 02 May 2017 23:31

I'm trying to export my Eagle schematic as a netlist that is readable

by Altium Designer (I use Eagle to develop schematic, contractor uses

Altium to do layout). I used the UDP called "netlist_protel.udp", but it

looks like a lot of times this UDP for some reason will list the pin

connection by the pin's name (ie "U7-ADC7") rather than the pin number

(ie "U7-22"). We've also tried Altium's Eagle file importer, and that

also creates errors. Does anyone have a better netlist exporter for the

purpose of getting a netlist into Altium?

 

Does the EAGLE importer create the same errors? If not what are they? I

believe the importer generates some log files which might help give a clue

as to what else may be going on.

 

Best Regards,

 

Rachael

I don't think there are errors as such. Simply the netlist is being

taken from the schematic and needs to be taken from the board.

One of the file formats Altium designer could be expecting is IPC-D-356A

If so then the Eagle ulp export-ict-netlist-pad-coordinate.ulp  would

appear to have most of the code needed to write a ULP to create a

IPC-D-356A file.

The OP should run the ulp in the board which can be created with one

click from the schematic, no need to lay it out. Then inspect the file.

you can see it has both the pads and pins for each contact reference.

HTH

Warren

--

... use NNTP://news.cadsoft.de and a functional news reader like

Thunderbird!

... or http://www.eaglecentral.ca browser access to CadSoft EAGLE

support forums.

---

This email has been checked for viruses by Avast antivirus software.

https://www.avast.com/antivirus

On 3/05/2017 10:31 a.m., Ben Berkowitz wrote:

I'm trying to export my Eagle schematic as a netlist that is readable by Altium Designer (I use Eagle to develop schematic, contractor uses Altium to do layout). I used the UDP called "netlist_protel.udp", but it looks like a lot of times this UDP for some reason will list the pin connection by the pin's name (ie "U7-ADC7") rather than the pin number (ie "U7-22"). We've also tried Altium's Eagle file importer, and that also creates errors. Does anyone have a better netlist exporter for the purpose of getting a netlist into Altium?

 

--

To view any images and attachments in this post, visit:

https://www.element14.com/community/message/221544

 

Actually, there is already ulp that generates IPC-D-356A format files

See if that works.

ipc-d-356.ulp

All the best

Warrn

--

... use NNTP://news.cadsoft.de and a functional news reader like

Thunderbird!

... or http://www.eaglecentral.ca browser access to CadSoft EAGLE

support forums.

---

This email has been checked for viruses by Avast antivirus software.

https://www.avast.com/antivirus

This was the way to go. I generated the board from the schematic, exported with the netlist-protel.udp, and everything worked as needed. Thanks!