Merging Schematic and PCB files

Hi Mark , it seems like you have a problem of PCB  .  maybe you could send me your files to my email :sales1@alpcb.com.cn , i could let my engineer to solve your questions if you like .  -Emma

Erm, yeah - that's not going to happen!  I can't be just emailing out confidential design files to random people on the WWW.

And besides, its not a PCB problem.  Its me not understanding how to achieve what I want within the EAGLE package.

Mike

Erm, i c .

Then may god help you understand what you want .

Btw , i can make PCB through eagle file or gerber file , + assembly , if you need this help , just reply me .

Emma

Hi Mike,

maustin_solux  wrote:

 

OK, so I have three separate PCB designs, all generated from their respective schematic files (so I've got three schematic files and 3 PCB files)

 

I'm trying to develop a "sales demo" PCB that uses all three designs on the one PCB, but that has some level of interconnection (mainly the DC rails, GND signals, and a few other digital inputs) between each of the PCB designs.  As I understand it, I can do a File->Import->Eagle Drawing in PCB to merge all the PCB files into one, but is it possible to merge the schematics as well so that I get correct forward/backward annotation between schematic and PCB files?

 

I feel like I might be pushing excrement up a steep incline on this one, but thought I'd ask the question.

You are going about it the right way using the import EAGLE drawing function.

First things first, when you create your new empty board (or schematic) switch to the other editor to ensure the corresponding file is created and back annotation is happening.

Next load the DRC settings you wish to use to set up the layer count and design rules. You'll probably want to take the DRU file used for the most complex of the boards you have and load that up to configure the board.

Then when you import in either the board or schematic from one of your three designs, both the schematic AND board of that design will be imported. If you import from the PCB it's slightly easier as you get the choice of where to place the PCB right away rather than having to group and move it afterwards. Go ahead and do this for each of your boards in turn. You'll see it will prompt you to tell you when nets have been renamed to avoid them connecting together. You should find that global power nets will connect if they have the same name. You can then go and sort these out and connect them for the whole board as you require and you can also rename any other nets which you actually wish to be connected and route them in as normal.

There are a few things to watch out for that I can think of. Firstly, board stack up differences could make having global power/ground planes a bit more problematic and may require things to be altered a little to get that to work or to connect them up as you expect. Also, if there are conflicts in things like net classes and required DRC settings then you may need to do some manual fix-ups afterwards. It'll warn you of things like net class conflicts when you import although if you are importing fully complete designs that you don't plan to alter then you can probably ignore these as the routing wont change.

Run DRC and make sure there are no errors. If there are go in and sort them out and then hopefully you should be good to go get your board built. There may be other things to consider which I haven't thought of so please do as much checking as you need to make you feel comfortable that no errors have been introduced and clearly undertaking this is done at your own risk.

FYI, this import functionality is the underlying mechanism used by the Design Block feature of EAGLE so it should be fairly robust.

Best Regards,

Rachael

Awesome!  Thanks Rachael – worked a treat   You get a gold star!

The step I wasn’t doing was to have both the schematic and PCB files open (and hence activating the back annotation) before I started importing things.

Hey Mike, you're welcome! Glad to hear it worked for you