Best way to design a stacked PCBs circuits

Il 27/02/2017 14:42, Marco Trapanese ha scritto:

The mains drawbacks are:

 

• lot of signals are the same (those that go with the connectors) so any

changes to their names or net classes must be repeated in the second

project as well

 

• the same applies for the layout: the positions of mounting holes or

any milling layer must be kept in sync with the PCBs

 

• last but not least, in the lower PCB I have several tall components.

In the higher PCB I need to provide slots for them. Doing that in

different project is a pain because I need to write down the position of

each one and move the related slots every time I change their placement

I add that having a single schematic is better because from a functional

point of view no matter where a component is placed.

I'm going to try to add a couple of routing layers to "simulate" the

other PCB, then I will play with the CAM processor to make the two

different set of gerber files.

What do you think about this solution?

On 02/27/17 08:42, Marco Trapanese wrote:

Hello,

I'm going to develop a circuit that will be composed of two stacked PCB.

Several connectors will provide connections between the two layers.

 

I wonder which is the best approach in EAGLE to do this.

The simplest way is of course to make different projects, one for each PCB.

I've done this twice. Note that I'm a hobbyist and there may be better

ways to do this.

The first time I had one board hosting a microprocessor and a much

smaller one hosting the front-panel switches. The board with the

switches mounted above the uP board using standoffs and a pin header and

socket. I ended up creating one project and milled break-off tabs

between the two boards. Aligning the pins in one of the two dimensions

was easier because the two boards shared a common edge.

The second time I made a set of 5 boards that mount in a stack using

PC/104 style connectors. These were too large and too complicated to

implement in one project.

What I did was to create a separate sheet in the schematic for the

common connector interface. It was fairly easy to copy everything on

that sheet in the first schematic and paste it into the others. It would

be nice if Eagle allowed you to include a partial schematic into

multiple projects, but that wasn't possible when I started the project.

It may be now; I don't know.

To make sure the connectors all aligned properly I created a library

part that defined the basic board outline including the positioning of

the connectors and the mounting holes. Each project then pulls in the

basic board device on the common connector interface schematic sheet. In

the layout, the lower left corner of this device is placed at the lower

left corner of the board dimensions. I suspect you could use one of the

documentation layers of the device to define the location of your tall

components.

This approach developed over time, so there may be ways to optimize

this. For example, I didn't define any of the connector pins in the

device as having particular nets or functions; I did this in the common

schematic sheet. In retrospect it seems defining them in the device may

have been better.

-Reece

Il 28/02/2017 16:07, Reece R. Pollack ha scritto:

The first time I had one board hosting a microprocessor and a much

smaller one hosting the front-panel switches. The board with the

switches mounted above the uP board using standoffs and a pin header and

socket. I ended up creating one project and milled break-off tabs

between the two boards. Aligning the pins in one of the two dimensions

was easier because the two boards shared a common edge.

Right now I've used this approach, even if my case was more similar to

your second example.

The second time I made a set of 5 boards that mount in a stack using

PC/104 style connectors. These were too large and too complicated to

implement in one project.

 

What I did was to create a separate sheet in the schematic for the

common connector interface. It was fairly easy to copy everything on

that sheet in the first schematic and paste it into the others. It would

be nice if Eagle allowed you to include a partial schematic into

multiple projects, but that wasn't possible when I started the project.

It may be now; I don't know.

Interesting, but it could work if each layer is independent - sharing

only the PCB edges and board-to-board connectors.

My current project is composed of only two stacked PCB but I need to

provide holes in the top one to grant access to the lower PCB (i.e. to

reach a trimmer or a screw).

I need to inspect the coordinates (and the sizes that are not so easy to

measure in EAGLE) of the desired components to place slots and the other

components on the second PCB.

I know it is a different working approach but I'm wondering if any of

the other suite for electronic designs out there provide tool for

stacked PCBs.

Freely speaking: of course a complete support requires a lot of work,

but it could be simple enough to allow the background of an EAGLE Layout

window to be transparent and keep synced position and zoom of another

instance.

In this way it would be easier to design with the other(s) PCB in the

view (with of course a different value of transparency, to avoid to be

confused!)