Not recommended unless this is the way you want to do it:
The only reason I've done it this way is because I didn't want to learn Camtastic.
The way I have done it within P99SE was to do make a separate project called the tiled PCB. Then I'd do a select & copy from each of my separate PCB projects, then do a "Paste Special" enabling "Duplicate designator", on to the tiled PCB document. This will retain the component names without adding the duplicate name -#.
For anticipated future changes to 1 or all of the sub-PCB projects, I have a fixed outline on 1 of the mechanical layers and a registry mark so that I can easily cut out a lemon PCB & paste in a modified one easily exactly on target.
____________ Brian Guralnick
----- Original Message ----- From: <[EMAIL PROTECTED]>
To: <[EMAIL PROTECTED]>
Sent: Tuesday, October 26, 2004 8:02 AM
Subject: Re: [PEDA] how to merge three PCB to one
In a message dated 2004-10-26 07:49:22 AM Eastern Daylight Time, [EMAIL PROTECTED] writes:
I have three small PCB and I want to merge them to one PCB in order to decrease the cost. I am thinking about two method as following but either has demerit. Could you please give me some advice?
(1) Design the three PCB in one project. But the designator name cannot
repeat so I must name the parts of the1st PCB from "U1" to "U5" then the 2nd
PCB from U6 to U10 (for example) and so on.
At a minimum, keep some separation between the projects. That is, use a
separate schematic page for each project, and number all of page 1 "U101,
U102,....", page 2 "U201, U202..." etc. There's no penalty I've ever found for skipping
numbers, and you can then insert parts without renumbering everything;
indeed, I have long used a system where particular sections of a project get
specific hundreds, and subsections get a whole decade. Many of my clients prefer that
the hundreds digit match the page number, just for ease in finding a
reference later. This automatically avoids any conflicts.
You'll also need to watch out for common net names, such as gnd and vcc.
Prefix or suffix those with a page number as well. If you use a suffix, it's easy
to look at the netlist file and see that you got things sorted out correctly.
(2) Design the three PCB in three projects. But when I output the three gerber data files I cannot merge them into one gerber data file.
I believe Camtastic has the capability to merge gerbers. Alternatively, you
can bet that your PCB house can do so, because they do that routinely to get
the best yield from the raw materials. But they probably change extra for that
merge, which defeats your purpose in doing so. You might want to ask them if
you can get a discount by running all three boards together; it might still be
the cheapest way to get the job done in the long run, and you don't end up with
artifacts that don't belong in your designs.
Steve Hendrix
____________________________________________________________ You are subscribed to the PEDA discussion forum
To Post messages: mailto:[EMAIL PROTECTED]
Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com
Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[EMAIL PROTECTED]
Browse or Search Current Archives (2004-Current):
http://www.mail-archive.com/[EMAIL PROTECTED]
____________________________________________________________ You are subscribed to the PEDA discussion forum
To Post messages: mailto:[EMAIL PROTECTED]
Unsubscribe and Other Options: http://techservinc.com/mailman/listinfo/peda_techservinc.com
Browse or Search Old Archives (2001-2004): http://www.mail-archive.com/[EMAIL PROTECTED]
Browse or Search Current Archives (2004-Current): http://www.mail-archive.com/[EMAIL PROTECTED]
