importing netlist

[earwig37]

I have an existing board layout and I wish to add a new circuit.  How do I handle the netlist for the new circuit?  Will the importing process adjust net names/numbers for the new circuit so as not to connect to any existing nets that might have a common net name/number?

[lacy]

I just tried this on a test board and Ultiboard will destroy the old netlist in favor of the new netlist and actually gives you are warning to that effect before the import. I did not hurt my existing board by attempting this so long as I don't save it at this point. This isn't going to allow you to import an net list and merge it with another. It just won't work. 

[nestor-sg]

Are you trying to add a new board layout to an existing project file (e.g. 2 or 3 board designs in the same project file)?... or do you have a board layout for which you want to add more parts and nets?...

If you have the first option... then in Multisim select Transfer > Export to PCB Layout... (not Ultiboard)... and save the EWNET file in Ultiboard 10 format... then in Ultiboard... once you have the new blank design added to your project just go to File > Import > UB Netlist... and that is how you may have two or more independent netlist in the same project... however they are on different board designs (or outlines).

If you want to add to an existing layout (one PCB) more components... then do it first in the schematic in Multisim and then forward annotate to Ultiboard... it will keep whatever parts of the netlist are the same and add the ones that are not in the current netlist...

[lacy]

Hi Nestor, I  think I understand your procedure. Basically your are just adding another board to the project. I do not believe this is what this user wanted to do. If I understood his post correctly, I believe he wants to merge two boards into one board. He already has both boards but wants them both on one larger board. If I am correct about this, then this is something that Ultiboard will not allow through importing a separate net list. It just overwrites the current net list.

I think he may be able to do this through Multisim as you outlined in the last part of your post. But he made no mention of whether or not he had schematics for the layouts. If he doesn't then I have no idea on what can be done at that point.

Thanks though for your procedure.This will come in handy for a lot of users. Very nice procedure.

[nestor-sg]

That is correct Lacy, if you just have two different netlists and you want to merge them together I would rather do that at the schematic level, however there is a nice workaround...

So... this workaround works for the case in which you have one single PCB design, and you wish to add a new netlist to the current netlist, assuming you are not doing so at the schematic level...

1. Import the new netlist into a new Ultiboard project... (have the target project open as well).
2. With the two projects open, go to the design that has the new netlist...
3. You have not routed or placed components yet (you still see the ratsnest)... so you can go ahead and select all the components, and right-click select Copy.
4. Go to the original project (target), and select Edit >> Paste Special... >> Paste with Net.
5. Your new components and nets are now part of the original project.

IMPORTANT NOTES:
a) RefDes will be renumbered to avoid conflicts.
b) Netnames will not change... so if you have a "TXpos" net in the first project and a "TXpos" net in the second project they WILL BE merged... most likely you don't really want this, so you have to make sure that you rename your nets before doing this process.
c) You will not be able to forward annotate changes from Multisim to Ultiboard in the future since the netlists will not match and your components will be sent out of the board boundaries...

So, in other words, only do this if you can't work this out at the schematic level which is the preferred way, since your one PCB should be one project in Multisim as well... I will indeed file a feature request to have the ability to merge netlists in an easier way...

Message Edited by nestor on 03-12-2008 06:53 PM

[lacy]

Thanks Nestor. That was brilliant. I think all bases have been covered here. I hope the user can take this information and accomplish his goal. I know I learned a few things from this post. These procedures were very enlightening for me. Of course, I have only made changes to my project at the schematic level and use the annote features, so this was something new I have learned.

Thanks a bunch Nestor.

[lacy]

While we are both discussing this, I noticed that Ultiboard's Project view operates differently than Multisim's Project view. In Multisim the project view allows you to add files to the project. You can have as many schematics in the list as you want. There is no easy option to do this in Ultiboard. I am not sure how this would affect the export to gerbers. This is a feature request (I guess). This way you can save many boards under one project simply.

[nestor-sg]

Hi Lacy, is very simple actually, in Ultiboard, where you see your project... in that same design toolbox you'll see that there is a small toolbar... click the "New" button, this will bring up the dialog to add a new design to your existing project.... once you have your new design in the same project, this is where I mention previously that instead of "transferring" (the first time) your design from Multisim to Ultiboard, you need to "export to pcb layout" from Multisim and then on this design do a File > Import > UB Netlist.

[earwig37]

Here is the scenario with the +imported netlist question:

I have two schematics and two boards - one big and one small.  I wish to pick up the layout of the small board (all layers, copper, nets etc.) and place it on the larger board.  Some of the nets of the two circuits will interconnect --- I can do that with the netlist editor, but retaining the layout and layers seems to be the problem.  You all have given me some ideas on things to try, so I will do that.  Of course, in the worst case, I will have to just add components and nets and layout the smaller board again.  The smaller board is a prototype circuit; it works; and it is a "hairy" layout --- I am trying to maximize the probability that it will continue to work when placed on the big board!!

[nestor-sg]

I see... make sure that you match the copper layers from the small design into the larger design... then also make sure that you do not duplicate netnames that you do not want to connect on both designs... then... go to the small layout, select all components and nets... Edit > Copy... then go to the larger design... and do a Edit > Paste Special > Past with Net....  it will do most of the work for you.

The paste operation will not create layers that do not exist... that is why you must make sure that if you have Top, Inner 1, Inner 2, Bottom in the small design... you must also have "at least" the same layers in the larger design... when you paste all copper on all layers will be pasted as well...