> -----Original Message-----
> From: Tim Fifield [mailto:[EMAIL PROTECTED] 
> Sent: Tuesday, September 02, 2003 3:07 PM
> To: Protel EDA Forum
> Subject: [PEDA] Paneling
> When making a panel is it best to do it in Protel or a gerber 
> tool such as Camtastic?


Depends what you want to do and if the board will be large volume or

Some pcb suppliers will prefer to panel themselves in which case you
will need to supply them with any data you might need such as waste
strips for conveyor clearances, tooling holes for auto insertion
machines, breakouts, slots/routs/v scores and so on. PCB houses do this
all the time as most production is panelled anyway, they just supply it
to you as single circuits.

If you want to do it yourself, you will need to sacrifice an electrical
DRC as Protel does not support DRC properly of arrays as no net
information is retained on the copied array, when the panel is built up
in the PCB editor.

Usually if I am going to supply panel instructions or prepared panels I
will copy the original PCB after complete DRC, to a new file with a
different name. I would then, after making all layers active &
primitives visible, copy the images into the format of array I wanted
and add all waste strips, tooling holes, scores, fiducial markings, bad
marks etc.

If you do not want to actually panel the image completely, then you
could add the panel instructions on different mechanical layers on the
original PCB file, such as set the image relative origin within the
board outline (such as on a fiducial mark or hole) and just mark the
origins for the pasted images and let the PCB house apply their edits to
the single image (which you can still DRC) and then they can past the
array as you instructed. 

The process is more or less the same in Camtastic or other cam tool if
you do it yourself.

But most importantly the panelled image should be engineered for the
production environment that it will be used in as the DFM rules for
those processes / plant will dictate the actual array construction
somewhat more than normal.

When designing the method to 'break out' the panels, consider also the
force that needs to be exerted to snap off from a V score (board
flex/torsion, undue stress on fine pitch parts, BGA or ceramic/MLC
parts) after assembly or at least allow clearance for a PCB
separator/shears. If you make routs with key ways for break out,
remember to keep them small enough to avoid flex in the wave, or solder
floods (mixed tech boards) and also you might need some fixed tooling
under a badly panelled board for some placement machines (usually just a
temporary 'table' which snugs the underside of the board before
placement) or automatic printers (vac platform) as you may experience
'bounce' during print / placement as the board will not be as rigid as
you might think.

Depends on the board of course, as a panelled 60 x 100 mm board panelled
3 x 3 up with a V score will have completely different characteristics
than a  3 x 3 up with routs / break outs.

Hope this helps in some way.

Best Regards

John A. Ross

RSD Communications Ltd
8 BorrowMeadow Road
Springkerse Industrial Estate
Stirling, Scotland FK7 7UW

Tel     +44 [0]1786 450572 Ext 225 (Office)
Tel     +44 [0]1786 450572 Ext 248 (Lab)
Fax     +44 [0]1786 474653
GSM     +44 [0]7831 373727

WWW     http://www.rsd.tv

> Tim Fifield

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* http://www.techservinc.com/protelusers/leave.html
* Contact the list manager:
* Forum Guidelines Rules:
* http://www.techservinc.com/protelusers/forumrules.html
* Browse or Search previous postings:
* http://www.mail-archive.com/[EMAIL PROTECTED]
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to