this comes up all the time
we use your method #1 almost every day with no troubles
using this method you also get full DRC checking as well whereas if you use the paste special method you do not
don't forget that not only is pcb cost lower but overall
handling and assembly costs are lower (assuming the boards are used as a 'set' which is what we do)
something you have to think about however is how you are going to singulate the boards
as you get into tab routing, mouse bites and other features which may not otherwise be needed you start to erode a bit of the benefit
we have been scoring some of these things lately
before you say it is crummy method please realize that scoring has come a long way in the last decade just like the rest of pcb fab tech
they can now do jump (or skip) scoring, hold accuracy to maybe 10 thou and other stuff
for todays NC scoring machines due to FR4 fringing leave 20 thou (mils) min between the score line and the edge of an outer trace or Cu
40 is probably a smarter choice so that is one down side to scoring
nominal score depth s.b. 1/3 T from each side
this varies with how big a piece you have to grab though (leverage) narrow breakoffs need to be scored deeper very heavy big bds with a score in the middle may be scored less deeply
also there are stresses to consider during the singulation whatever method is used
if the board has slots or routing operations anyway then maybe drop a few obrounds in the scored areas to reduce the stresses of the singulation process
also the edges will not be extacly pristine but may be suitable for many purposes and don't have to be cleaned up like the tab & mouse bite routine
Dennis Saputelli
_______________________________________________________________________ Integrated Controls, Inc. Tel: 415-647-0480 EXT 107 2851 21st Street Fax: 415-647-3003 San Francisco, CA 94110 www.integratedcontrolsinc.com
é wrote:
Hello everyone,
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.
(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.
Thank you for any advice.
____________________________________________________________ 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]
