At 01:08 PM 7/09/01 +1200, you wrote:
>I am currently trying to create an A3 panel of 10 PCB designs I have
>created using Protel99SE. This saves cost by prototyping several PCB boards
>at once.
>When I try to copy and paste the PCB designs using Protel99SE the designs
>lose their connections to the Internal Plane (which I am using as a Ground

Yep - this will happen as when you copy and paste you do not bring over the 
design rules or the plane assignments.  You may get a better result by 
taking one of the boards and using the Copy-As function to create a new PCB 
which will become the panelised PCB.  This preserves the design rules and 
other stuff not copied by the Copy and Paste.  But it doesn't help if the 
other boards in the set have wildly different design rules or layer stackup.

The potential for incorrect rules causing problems with connections to 
internal planes is very real.

You can export a set of rules from one of your designs (use the Menu button 
on the Design rules dialog) and then import this rule sset into all the 
other designs and re-run DRC and confirm that each design is OK.  Then this 
same rule set can be used in the panelised board and you should/might/may 
be OK.

Make sure in the new design the GND net is tied to the internal plane 
(Layer Stack manager), and you keep the nets (and allow duplicates) using 
the Paste Special command (rather than Paste) when you do the pastes.

>Is there any way around this?

If all the boards are similar in construction it may be possible to do but 
is not for the faint-hearted (panelising the same PCB over and over is 
simpler).  A detailed knowledge of the program and the PCBs and the 
manufacturing process is required.

You could use Camtastic to do the panelising as this is the sort of thing 
it is good at.  It deals with the Gerbers, so doesn't try to get too smart 
with rules and layer stack-ups.  This is what I'd do, I think, even though 
I have been panelising in Protel for years.

Ian Wilson

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* To post a message: mailto:[EMAIL PROTECTED]
* To leave this list visit:
* Contact the list manager:
* Forum Guidelines Rules:
* Browse or Search previous postings:
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * *

Reply via email to