Problem in importing netlist

[eirij]

Hello,

I am having the same issue with cmd-net-list2sch. I created nets in my schematic, export as Netlist, remove all of the nets from the schematic, and 

RUN cmd-net-list2sch name.lst to draw them again. But it only draws two nets in my schematic.

Can anyone provide me with the complete description of Netlist format and also help me to solve this problem of importing netlist to a schematic.

Best Regards,

Muhammad Eirij

[jorge_garcia]

Hello @eirij,

I hope you're doing well. First from the EAGLE schematic you can export either a netlist or a netscript. If the netlist ULP is giving you trouble, try exporting a netscript and then running cmd-netscript2sch.ulp. To export either a netlist or a netscript from a schematic click File > Export > Netlist or Netscript.

Keep in mind that for these ULPs to work all of the components must exist on your schematic and they must have the same names as in the schematic from which the netlist or netscript was created. This is all to say that if your are trying to use these as a way to quickly recreate a schematic, this is not the best option. For those scenarios you are better off using the export schematic.ulp that can be downloaded here.

Let me know if there's anything else I can do for you.

Best Regards,

[eirij]

Hello @jorge_garcia

Thank you so much for your reply.

Actually, I am trying to develop my own symbols and patches and then placed them according to the product specification. Where, i have provided with the connection file with source and destination pins and pad numbers. My idea is to use this information to create a toolbox which can generate Eagle-Netlist file or Net-Script file.

While, from my experience if i create a random schematic with the components library provided by the Eagle, the export Netlist or Netscript files shows some errors.. e.g. wrong or empty pin and pads numbers. However, if I correct the errors manually, and import the Netlist again then it only draws one or two Net and merge the rest of them. Where, If i use RUN cmd-net-list2sch In1 R1 1 C1 then it automatically connects pins and pads. Do you know this problem? 

Right Now, my toolbox is generating a text file with each line a Command for connecting pin and pads like (RUN cmd-net-list2sch pinS padS pinD paD).

Is it Possible to run all these commands through a single run, except copy and paste?

Can you also provide me a document which shows the complete Formation of the Netlist and Netscript ? 

So that i can use that to improve my toolbox to generate them.

Best Regards,

Muhammad Eirij

CADsys

[eirij]

Hello @jorge_garcia

Thank you so much for your reply.

Actually, I am trying to develop my own symbols and patches and then placed them according to the product specification. Where, i have provided with the connection Excel file with source and destination pins and pad numbers. My idea is to use this information to create a toolbox which can generate Eagle-Netlist file or Net-Script file.

While, from my experience if i create a random schematic with the components library provided by the Eagle, the export Netlist or Netscript files shows some errors.. e.g. wrong or empty pin and pads numbers. However, if I correct the errors manually, and import the Netlist again then it only draws one or two Net and merge the rest of them. Where, If i use RUN cmd-net-list2sch In1 R1 1 C1 then it automatically connects pins and pads. Do you know this problem?

Right Now, my toolbox is generating a text file with each line a Command for connecting pin and pads like (RUN cmd-net-list2sch pinS padS pinD paD).

Is it Possible to run all these commands through a single run, except copy and paste?

Can you also provide me a document which shows the complete Formation of the Netlist and Netscript ? 

So that i can use that to improve my toolbox to generate them.

Best Regards,

Muhammad Eirij

CADsys

[jorge_garcia]

Hi @Anonymous,

I hope you're doing well. Perhaps your application would be better served using Designblocks? I don't have any document detailing the format of the netlist but if you generate one from EAGLE you can get a good feel for the format.

A netscript is just a bunch of calls to the signal command.

Please let me know if there's anything else I can do for you.

Best Regards,

[eirij]

Dear @jorge_garcia,

Thank you for your reply. I hope you are doing well too.

I have already understood the concept of the Netscript & Netscript.

Currently, I am having a problem with misconnection while using "Run cmd-net-list2sch net part pin part pin".

How can I handle this situation?

Best Regards,

Muhammad Eirij

[jorge_garcia]

Hello @Anonymous,

I hope you're doing well. Could you post the misconnection you are observing? If you could create a screencast showing you running the script and the flaw you are observing.

Please let me know if there's anything else I can do for you.

Best Regards,

[eirij]

Hello @jorge_garcia,

Thank you so much for always helping me.

In the Screenshot 2 you can see that I have used a command RUN cmd-net-list2sch net1 PART1 PAD1 PART2 PAD2;. These are the experimental devices I have been using right now.

The Problem can be seen in the screenshot 1, a net is not connected to the pins. Where its also not connected in the brd file.

I have also attached the connection chart of the component I have used.

Best Regards,

Muhammad Eirij

[jorge_garcia]

Hello @Anonymous,

I think the issue might be with your symbols. Are these symbols made to 0.1" grid? The images you attached don't make it clear that they are. Scripts don't have the benefit of the pin-snapping functionality so if you are off grid the connections won't happen.

Please let me know if there's anything else I can do for you.

Best Regards,

[eirij]

Dear @jorge_garcia,

When I was creating the symbol i selected the grid size 1mm, and even while connecting the pins automatically the grid size was 1mm.

I have tried that command with the predefined libraries and its working fine. The problem is only when I make my own symbols and packages.

I am attaching the test library I have just created. This time I made the symbol with 0.05mm but still having the issue of misconnection. 

Thank you so much for the wonderful support.

Best Regards,

Muhammad Eirij

[one-of-the-robs · Accepted solution]

This is a very common newbie mistake with Eagle.

You must NEVER define schematic symbols on a mm grid. They must ALWAYS be defined on a 0.1" grid. The packages for use in the board editor can be on any grid you like because they must match the real world package, but schematics are schematics - there is never any reason to want to use non-standard grid. Eagle's schematic editor really doesn't like non-standard grids for pin placement so always place your pins on the 0.1" default grid.

[Anonymous]

The topic is importing netlists yet the admins post listed as a first response is about exporting netlists.  At the same time the site will not allow me to create my own topic.  God this is painful.

Eagle 5.11.0

Netlist import ULP:  import-tango.ulp

Like a million other users I need to take an OrCAD schematic, export a netlist of some kind (while in OrCAD), then import that netlist into Eagle under the following proposed conditions:  In Eagle, I will have only a board file loaded.  That board will have all of the parts already created (and placed) on the board.  I will have used the same names and pin numbers for all of those parts that were used on the Orcad Schematic so that Eagle should have enough information to generate flying-wire connections on my board.

If that is not how this would work, I hope somebody can clue me in.  This is just common sense from a low to mid level user's perspective.  It would be nice to generate a schematic at the same time, but it is not necessary, and that would probably not work.  There are temporary unrouted flying wires on the board that can be created in this process, but there is not similar for the schematic.  The wires on the schematic would be a mess that could not be untangled easily without deleting most wires.

Orcad exports schematic netlists in a large number of different formats.  One is (ancient defunct) Tango.  I would like to be able to use that Tango netlist as an intermediate.  If it matters, I own licenses to Tango, and Eagle, and the company I am working for owns a license to OrCAD.  It should all be legal.  I found a ulp to run to accomplish this using the Tango netlist intermediate, and it does not work.  A few flying wires resulted, and some of those were correct, but it appeared to be wanting to create it's own parts rather than use the ones I had placed on the board... or something like that, and so complained about parts already existing.  It also mistook values as names... etc..  Not sure where it was getting the physical part data from if it was wanting to create it's own parts since it is just a schematic netlist... but maybe it was looking at my libraries.  So... I tried removing all the parts off of my board.  The result was that it placed a single part.  It was a fuse.  But it labeled it R1 rather than F1 and gave it the value of my R1, 100 Ohms.  So now I have a 100 ohm fuse that is a nice fuse package but a very different package from the one I had in my immediate library.

I will try making sure I have the relevant library loaded... but here is what I would hope to find somewhere on this forum:  The instructions for using that tango netlist import ulp were non-existent.  Why?  Why would you bother to post the ulp and then not explain how it works?  Is there a way to make it use the parts that I placed on the board rather than scan all my libraries for the first one with a name or value that lines up with a name or value in orcad?  Must I have a library loaded with parts that have names but no values so that it won't get confused...  My packages don't have any values yet it got 100 ohms from somewhere?  There is a 100 Ohm resistor in the schematic, but again, that schematic was not loaded nor even present in the directory where the board and ulp files were located.  Why is it even looking at my symbols?  I am not trying to generate a schematic, just a board, which is apparently a very common situation.  I like Eagle much better than OrCAD, but the company I am consulting for has been using OrCAD capture for 25 years, they are all very old, and they aren't going to change over any time soon.  Currently they are sending their PCB work to someone who can import their netlists into his (not eagle) layout program.  This doesn't make any sense that I can't accomplish the same with Eagle, if only through one of the many possible intermediate netlist formats such as Tango.

I am willing to buy the latest version of eagle if I am sure it will work, but I would have to see it work on the free version first.

[one-of-the-robs]

I'm sorry you're finding the forum painful. It could certainly be better.

On the issue you asked about, the biggest problem is that you're looking at the way some other (quite old) tool works and assuming it's the only way. It's not, and it's not the best, either.

Don't get me wrong, I quite understand why you would make that assumption. We all fall into the trap of thinking what we're accustomed to is the only right way - just like we complain that somebody else's Lasagne recipe isn't the same as mum's! In this case, though, as, indeed, in most cases, you'd be better putting all your assumptions aside.

OrCAD, like many other eCAD programs, only did half the job. It allowed you to draw a nice set of schematics and export their "essence" as a netlist. You would then use some other software (at my day job it's Mentor Pads) to finish the job off by creating a board layout.

Eagle has never worked that way. It treats the creation of an electronic circuit as a single, seamless process, albeit carried out in stages. So you start with a schematic in Eagle and lay it out on a board in the same instance of Eagle, because you're still doing the same job, really. This is, to my mind (having used a few eCAD packages) a much better approach (I will resist the temptation to say "clearly the one true and right approach"). Unfortunately for you, this means it makes the assumption that you will have both schematic and board loaded, and that assumption influences all the ways it works.

I'm afraid my recommendation would be to convert the schematic to Eagle and go from there, rather than force it into an inferior way of working. However, perhaps one of the "millions" of other OrCAD users who "need to" work the way you first envisaged will be able to suggest an alternative.

[Anonymous]

I think you are right, and that was my initial instinct.  Having gone full circle, just having gotten the tango netlist importer ulp working, I am not going to use it.

The problem is that my boss didn't want me building a board in Eagle unless it could import an OrCAD Capture netlist.  Well, it can... I can tell him that truthfully now.

One of the problems with using a netlist import to setup flying wires on a board with no schematic is that the flying wires on the PCB can then be deleted.  So the guarantee that my boss is expecting of matching nets doesn't exist.

So I will just duplicate the OrCAD Capture schematic in Eagle as you suggest.  But I do need to find a ulp or other tool for cross-checking that OrCAD netlist (or Tango export) with my Eagle netlist.  I don't want to rely entirely on doing that by eye.

[deepak_elango]

Hi @jorge_garcia 

Is there any provisions for importing Netlist in the Schematic Editor?

If there is any way can you suggest how to do it?

Best Regards,

Deepak Elango

[jorge_garcia]

Hello @deepak_elango,

I hope you're doing well. I responded in detail to the thread you created on this. We can keep the conversation going there.

Let me know if there's anything else I can do for you.

Best Regards,