EAGLE Central Forums
Where the EAGLE community meets. Sponsored by Stratford Digital.

Home » CadSoft Support Forums » eagle.support.eng » Eagle netlist export problems
Eagle netlist export problems [message #170359] Tue, 02 May 2017 22:31 Go to next message
Ben Berkowitz
Messages: 2
Registered: May 2017
Junior Member
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
Re: Eagle netlist export problems [message #170364 is a reply to message #170359] Wed, 03 May 2017 04:23 Go to previous messageGo to next message
warrenbrayshaw
Messages: 1742
Registered: January 2010
Location: New Zealand
Senior Member
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
Re: Eagle netlist export problems [message #170365 is a reply to message #170364] Wed, 03 May 2017 06:28 Go to previous messageGo to next message
rachaelp
Messages: 551
Registered: March 2015
Location: UK
Senior Member
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
Re: Eagle netlist export problems [message #170366 is a reply to message #170359] Wed, 03 May 2017 08:25 Go to previous messageGo to next message
rachaelp
Messages: 551
Registered: March 2015
Location: UK
Senior Member
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
Re: Eagle netlist export problems [message #170367 is a reply to message #170366] Wed, 03 May 2017 08:40 Go to previous messageGo to next message
warrenbrayshaw
Messages: 1742
Registered: January 2010
Location: New Zealand
Senior Member
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
Re: Eagle netlist export problems [message #170368 is a reply to message #170359] Wed, 03 May 2017 09:39 Go to previous messageGo to next message
warrenbrayshaw
Messages: 1742
Registered: January 2010
Location: New Zealand
Senior Member
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
Re: Eagle netlist export problems [message #170408 is a reply to message #170367] Mon, 08 May 2017 22:23 Go to previous message
Ben Berkowitz
Messages: 2
Registered: May 2017
Junior Member
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!

--
To view any images and attachments in this post, visit:
https://www.element14.com/community/message/221770
Previous Topic: Hierarchical Component Numbers on PCB - how to renumber/get rid of module prefix?
Next Topic: Design block
Goto Forum:
  


Current Time: Tue May 30 07:12:56 GMT 2017