Dealing with multiple boards?

On 11/30/2009 9:44 AM, Josh wrote:

Hi all. I've been using Eagle for a few years, but mainly for small, stand

alone boards. Now I'm working on a project that will require multiple small

boards that all interconnect. I'm thinking about upgrading to a version

that supports multiple schematic sheets so each board can have its own

schematic. What's the best way to deal with the multiple boards though?

Presumably when you create a design with multiple schematic sheets all of

those parts end up in the board file too right?

 

Thanks!

 

Josh

Best thing to do is have separate sch/brd files for each board.

You could do it all in one sch/brd pair, but you will always have

airwires between all the common signals on the separate brds, which

would drive me crazy so I do it in separate files.

If you do it all on the same brd, just surround each brd with lines on

the dimension layer, and space them about 50mils apart so you can have

the board house build them and tab route between the boards.

Ah, that's what I was afraid of. I like to keep the schematics together to

help me make sure I'm wiring connectors the same, etc. Not a huge deal, but

it helps me to avoid stupid mistakes. What I've done in the past is to

create a large schematic with all the parts on it, then cut and paste the

remote board ones into a new schematic file. It's a bit messy as my main

schematic then ends up with a bunch of unconnected things, but I could

always delete them too if I was really worried about it.

Thanks!

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Josh wrote:

Ah, that's what I was afraid of. I like to keep the schematics together to

help me make sure I'm wiring connectors the same, etc. Not a huge deal, but

it helps me to avoid stupid mistakes. What I've done in the past is to

create a large schematic with all the parts on it, then cut and paste the

remote board ones into a new schematic file. It's a bit messy as my main

schematic then ends up with a bunch of unconnected things, but I could

always delete them too if I was really worried about it.

 

Thanks!

Use good and constant net names between boards then if you export the

net list by device the mating connectors from each export should be easy

to check.

Paul R.

On Mon, 30 Nov 2009, Travis G wrote to us saying :

 

You could do it all in one sch/brd pair, but you will always have

airwires between all the common signals on the separate brds, which

would drive me crazy so I do it in separate files.

What I have done in the past is design a single schematic with the

inter-board connectors shown, so that some net wires on the schematic

have a plug-socket pair in the middle of them. This meant that I was

explicitly NOT putting each board on a separate sheet - if you're doing

that you may as well use a separate schematic. I had sheets with bits of

each board, because the boards were stacked to make a single final

assembly.

Then I laid out the two PCBs next to each other, having placed the

connectors and mounting holes as required.

This worked great except for one thing. The board house I use don't

really like two separate boards in one set of Gerbers. I thought I had

agreed a suitable solution with them (using a milling pattern to

separate the two halves after PCB production) but actually they ended up

supplying the fully populated boards still joined together. Oh well, a

few minutes with a hacksaw fixed that.

These days I use a separate schematic for each board, but I might do the

single schematic trick again if the boards are tight-coupled.

--

Rob Pearce                       http://www.bdt-home.demon.co.uk

The contents of this | Windows NT crashed.

message are purely   | I am the Blue Screen of Death.

my opinion. Don't    | No one hears your screams.

believe a word.      |

My approach depends on the project.

You could do it all in one sch/brd pair, but you will always have

airwires between all the common signals on the separate brds, which

would drive me crazy so I do it in separate files.

 

What I have done in the past is design a single schematic

For ease of understanding the schematic, I had a project with 3 boards

contained within a single schematic on 2 sheets.

 

Then I laid out the two PCBs next to each other, having placed the

connectors and mounting holes as required.

I laid all three boards out next to each other: this made aligning

mounting holes and connectors and any pin swapping very easy.  I also

had the outline of the case so I could arrange the boards properly with

respect to the heatsinks etc.

 

This worked great except for one thing. The board house I use don't

really like two separate boards in one set of Gerbers.

Once I've completed the design (ignoring any airwires between boards) I

copied the board file ONLY into my "Manufacturing" directory 3 times and

renamed for each individual board.  Then I deleted the other boards to

leave a single board per file.  I used common Drill & CAM files to

create the manufacturing files for each board.  Works fine for me and

enforces change control since the schematic is detached from each of the

3 boards. YMMV.

Cheers

Neil

"Josh" <joshybear@gmail.com> wrote in message

news:hf0lo5$sm7$1@cheetah.cadsoft.de...

Hi all. I've been using Eagle for a few years, but mainly for small, stand

alone boards. Now I'm working on a project that will require multiple

small

boards that all interconnect. I'm thinking about upgrading to a version

that supports multiple schematic sheets so each board can have its own

schematic. What's the best way to deal with the multiple boards though?

Presumably when you create a design with multiple schematic sheets all of

those parts end up in the board file too right?

 

Thanks!

 

Josh

--

Browser access to CadSoft Support Forums at http://www.eaglecentral.ca

Have a look at "merging.zip" (download --> ulp), you can merge designs

easily (both schematics and layouts).

Maurice